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Legal Notices....................................................................................................................vi Introduction.......................................................................................................................ix
The SolidWorks Software........................................................................................................................ix Intended Audience.............................................................................................................................ix System Requirements........................................................................................................................ix Document Structure...........................................................................................................................ix Conventions Used in this Document..................................................................................................x
1 SolidWorks Fundamentals...........................................................................................11
Concepts................................................................................................................................................11 3D Design.........................................................................................................................................11 Component Based............................................................................................................................12 Terminology...........................................................................................................................................14 User Interface........................................................................................................................................15 Windows Functions..........................................................................................................................15 SolidWorks Document Windows......................................................................................................15 Function Selection and Feedback....................................................................................................17 Design Process......................................................................................................................................22 Design Intent..........................................................................................................................................22 Design Method.......................................................................................................................................23 Sketches................................................................................................................................................23 Origin................................................................................................................................................24 Planes...............................................................................................................................................24 Dimensions.......................................................................................................................................25 Relations...........................................................................................................................................28 Features.................................................................................................................................................31 Assemblies.............................................................................................................................................32 Drawings................................................................................................................................................33 Model Editing.........................................................................................................................................33
2 Parts.............................................................................................................................36
Overview................................................................................................................................................37 Countertop.............................................................................................................................................37 Design Approach..............................................................................................................................37 Create the Base Feature with an Extrude........................................................................................38 Add an Extrude to the Base.............................................................................................................39 Remove Material with the Cut-Extrude.............................................................................................39 Use a Loft to Make a Solid...............................................................................................................40
Shell the Part....................................................................................................................................41 Round Sharp Edges with Fillets.......................................................................................................41 Faucet....................................................................................................................................................42 Design Approach..............................................................................................................................42 Create the Sweep.............................................................................................................................43 Faucet Handle........................................................................................................................................43 Design Approach..............................................................................................................................44 Revolve the Sketch...........................................................................................................................44 Cabinet Door..........................................................................................................................................46 Design Approach..............................................................................................................................46 Create Beveled Edges with the Chamfer Tool.................................................................................47 Moldings.................................................................................................................................................47 Design Approach..............................................................................................................................47 Design a Mid-Plane Extrude.............................................................................................................48 Sketch a Profile for the Cut-Extrude.................................................................................................48 Mirror the Cut....................................................................................................................................48 Use Configurations of a Part............................................................................................................49 Hinge......................................................................................................................................................49 Design Approach..............................................................................................................................50 Create Sheet Metal with the Base Flange........................................................................................50 Make the Tab....................................................................................................................................50 Generate the Linear Pattern.............................................................................................................51 Add the Hem.....................................................................................................................................52 Alternate Design Approach..............................................................................................................52
3 Assemblies...................................................................................................................54
Assembly Definition...............................................................................................................................54 Assembly Design Methods....................................................................................................................55 Bottom-up Design.............................................................................................................................55 Top-down Design.............................................................................................................................55 Prepare an Assembly.............................................................................................................................56 Mates.....................................................................................................................................................57 Faucet Subassembly........................................................................................................................58 Faucet Subassembly - Alternate Design Approach..........................................................................61 Door Subassembly...........................................................................................................................62 Cabinet Subassembly.......................................................................................................................63 In-Context Design..................................................................................................................................64 Create an Assembly Component In-Context....................................................................................65 Modify a Part In-Context of an Assembly.........................................................................................65 Load an Assembly.................................................................................................................................66 Examine the Assembly..........................................................................................................................66 Hide and Show Components............................................................................................................66 Explode the Assembly......................................................................................................................68 Detect Collisions Between Components..........................................................................................68
.......................................................................................................................................................................................................................................................................................72 Vanity Cabinet Drawing Sheet.....................................................................70 Drawing Templates..................95 Examining and Editing Model Geometry................................................................................................89 Loading the Latest Models......................................................................72 Drawing Views..........................................79 Faucet Assembly Drawing Sheet..........................................................................................................................94 Animating Assemblies.............92 Sharing Models..............................................................................99 Opening a New Part........................................................................................................................................................................................................................102 Extruding the Sketch......................................................................................84 Bill of Materials.....................................86 5 Engineering Tasks..............................................................................................................................71 Drawing Sheets............................................................................100 Sketching a Rectangle.............................................................................................................................................89 Replacing Referenced Models........................................................................................................................92 Creating Photo-Realistic Images of Models.................................................................................................................................85 Balloons and Stacked Balloons...................95 Accessing a Library of Standard Parts.................................................................................73 View Display and Alignment..................................................................................................................................102 iv ........................................................................................................................................................................................................................................................................................................................................................96 A Step-by-Step Lesson............................................................................................................................................................................................87 Building Multiple Configurations of Parts.......................................................................................................................................................................................................................................................................................................................................91 Performing Stress Analysis..............70 Drawing Documents....................................................................................................................................................................................................................................98 Getting Ready for the Lesson.............................................................................100 Dimensioning the Sketch.............................................................................................................................................................................94 Managing SolidWorks Files.............................................................................................................Contents 4 Drawings....................81 Derived Views...........................75 Dimensions...................................................................................................100 Setting the Drafting Standard and Units....90 Recognizing Features in Non-SolidWorks Parts............................................................................................................71 Sheet Formats.............90 Importing and Exporting Files...................................76 Annotations......................................98 Creating a Box.......................................................................................................................................................................................................................................................................................................................................80 Explode Lines..........................................84 Exploded Views.......................73 Standard Views.......................................................................................................83 Vanity Assembly Drawing Sheet..................................................................................................................................................................................................................................................................87 Updating Models Automatically...........................................................................................................................................................81 Notes and Other Annotations...............................................................91 Customizing SolidWorks.......................................................................................................
...118 Opening a New Drawing...............104 Opening a New Part........119 Inserting Standard 3 Views.............................................................106 Extruding the Sketch............................................................... and Nut......123 Bolt.................................................................................................................................................................................................................................103 Saving the Part...........................................109 Extruding the Sketch.................................................................................................................................................................................................................105 Dimensioning the Sketch............................................................112 Putting the Box and Lid Together....................................................................................................................................................................................................................................................................................................................................112 Inserting Parts into the Assembly...................................................................................................................................................................................................................................................114 Mating the Components.......................Contents Creating a Hollow Model....................................................................................................107 Creating a Lip on the Cover............113 Moving a Component.............120 B Exercises........................... Washer................................123 Covered Can..................................................................................................................................................................................................................................................................................................114 Rotating a Component..............119 Inserting an Isometric Model View..........................................................................108 Dimensioning the Sketch...........................................................................................................................................................110 Saving the Part.........................................................................118 Setting the Drafting Standard and Units...........................................................................................................................................................................................................................................................................................112 Opening a New Assembly....................................................................................................................125 v .........................115 Saving the Assembly...............................................................................104 Creating a Lid for the Box..................................................................................................................................................................................................................................................................105 Setting the Drafting Standard and Units....................................105 Sketching a Rectangle.............................................................................................................................................................................118 Creating a Drawing...................................120 Dimensioning the Drawing.........................................................................................
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Throughout the document.com/sw/support/videocardtesting. and 3 in the SolidWorks tutorials. System Requirements For system requirements.com/sw/support/SystemRequirements. you are introduced to concepts and design processes in a high-level approach.html card requirements Document Structure This document is organized to reflect the way that you use the SolidWorks software. see the SolidWorks Web site: System http://www. and drawings. a faucet. progress to Lessons 1.Introduction This chapter includes the following topics: • The SolidWorks Software The SolidWorks Software The SolidWorks CAD software is a mechanical design automation application that lets designers quickly sketch out ideas.solidworks. assemblies.solidworks. This document discusses concepts and terminology used throughout the SolidWorks application. For example.html requirements Graphics http://www. ® Intended Audience This document is for new SolidWorks users. and produce models and detailed drawings. 2. and pipes) illustrates various tools and functions available to you in the software: ix . It is structured around the basic SolidWorks document types: parts. In this document. After you complete the Step-by-Step Lesson in this document. a bathroom vanity (including a cabinet. a countertop. you create a part before you create an assembly. The Step-by-Step Lesson on page 98 is hands-on training that guides you through each step in a process and shows the results. It familiarizes you with the commonly used functions of SolidWorks. experiment with features and dimensions. SolidWorks Help contains a comprehensive set of tutorials that provide step-by-step instruction on many of the features of SolidWorks.
annotations. Parts Assemblies Drawings Engineering Tasks Demonstrates design methods. and provides an overview of help options. specify mates. SolidWorks terminology.Section 1 2 3 4 5 Step-by-Step Lesson Exercises Title Topics Discussed Fundamentals Introduces design concepts. dimensions. or to emphasize text Reference to online tutorial Access the Online Tutorial from the Help menu in the SolidWorks software. Reference to Help Access Help from the Help menu in the SolidWorks software. Discusses drawing sheet formats. and features commonly used to make parts. utilities. Tip x . Conventions Used in this Document Convention Bold Italic Meaning Any SolidWorks user interface element that you can select such as a tool or menu item References to books and other documents. and use in-context design methods. Provides guided instruction to perform basic tasks. Provides sample exercises to practice the material. and bills of materials. tools. views. Examines add-in applications. and other resources to complete advanced tasks. Shows how to add parts to an assembly.
and surfaces. you can create 2D drawings or mate components consisting of parts or subassemblies to create 3D assemblies. When designing a model using SolidWorks. you create a 3D model. from the initial sketch to the final result. You can also create 2D drawings of 3D assemblies. Assemblies contain parts or other assemblies.1 SolidWorks Fundamentals This chapter includes the following topics: • • • • • • • • • • • Concepts Terminology User Interface Design Process Design Intent Design Method Sketches Features Assemblies Drawings Model Editing Concepts Parts are the basic building blocks in the SolidWorks software. A SolidWorks model consists of 3D geometry that defines its edges. the way the model exists once it is manufactured. The SolidWorks software lets you design models quickly and precisely. faces. From this model. 11 . SolidWorks models are: • Defined by 3D design • Based on components 3D Design SolidWorks uses a 3D design approach. you can visualize it in three dimensions. As you design a part. called subassemblies.
SolidWorks Fundamentals SolidWorks 3D part SolidWorks 3D assembly SolidWorks 2D drawing generated from 3D model Component Based One of the most powerful features in the SolidWorks application is that any change you make to a part is reflected in all associated drawings or assemblies. 12 .
SolidWorks Fundamentals This section uses the following terminology for the models: 13 .
For example.0) coordinate of the sketch. for example.0. Straight line used to create model geometry. features. a sketch origin appears in red and represents the (0.0.0) coordinate of the model. A face is a selectable area (planar or nonplanar) of a model or surface. You can add dimensions and relations to a model origin. but not to a sketch origin. for example. Flat construction geometry. including intersecting two planes. or patterns. You can select edges for sketching and dimensioning. The SolidWorks application creates temporary axes implicitly for every conical or cylindrical face in a model. Boundaries that help define the shape of a model or a surface.SolidWorks Fundamentals Faucet: Faucet handle: Waste pipe: Terminology These terms appear throughout the SolidWorks software and documentation. You can use planes for adding a 2D sketch. Plane Axis Face Edge 14 . You can create an axis in different ways. When a sketch is active. Origin Appears as two blue arrows and represents the (0. a rectangular solid has six faces. Location where two or more faces intersect and are joined together. section view of a model. or a neutral plane in a draft feature.
SolidWorks Document Windows SolidWorks document windows have two panels. or Manager Pane. assembly. such as dragging and resizing windows. edit the feature. cut. such as print. Many of the same icons. 15 . open. and suppress and unsuppress the feature or component. contains: FeatureManager design tree ® Displays the structure of the part. including: Windows Functions The SolidWorks application includes familiar Windows functions. for example. save. User Interface The SolidWorks application includes user interface tools and capabilities to help you create and edit models efficiently. or drawing. and paste are also part of the SolidWorks application.SolidWorks Fundamentals Vertex Point at which two or more lines or edges intersect. The left panel. for example. You can select vertices for sketching and dimensioning. Select an item from the FeatureManager design tree to edit the underlying sketch.
and assembly mates.SolidWorks Fundamentals PropertyManager Provides settings for many functions such as sketches. fillet features. and view multiple configurations of parts and assemblies in a document. you can use configurations of a bolt to specify different lengths and diameters. select. 16 . You can split the left panel to display more than one tab at a time. ConfigurationManager Lets you create. For example. Configurations are variations of a part or assembly within a single document. For example. you can display the FeatureManager design tree on the top portion and the PropertyManager tab for a feature you want to implement on the bottom portion.
SolidWorks Fundamentals The right panel is the graphics area. 17 . Menus You can access all SolidWorks commands using menus. It also provides feedback as you perform a task such as sketching an entity or applying a feature. including submenus and checkmarks to indicate that an item is active. or drawing. assembly. where you create and manipulate a part. inference lines. SolidWorks menus use Windows conventions. Examples of feedback include pointers. and previews. Function Selection and Feedback The SolidWorks application lets you perform tasks in different ways. You can also use context-sensitive shortcut menus by clicking the right mouse button.
tools related to features appear. similar to toolbars. The content of the tabs is customizable. for example. or drawing. Tooltips display when you hover over each icon. You can also add or delete tools to customize the CommandManager. such as Rotate View. if you click the Features tab. and sketch mode. You can display or hide toolbars. the Sketch or Assembly toolbar. assembly. such as part. it updates to show the related tools. Tooltips display when you hover over each icon. CommandManager The CommandManager is a context-sensitive toolbar that dynamically updates based on the active document type. For example. Shortcut Bars Customizable shortcut bars let you create your own sets of commands for part. the S key. dock them around the four borders of the SolidWorks window. Circular Pattern. The SolidWorks software remembers the state of the toolbars from session to session. 18 . assembly. Each toolbar comprises individual icons for specific tools. Each document type. you press a user-defined keyboard shortcut. and Circle. To access the bars. Toolbars are organized by function. drawing. You can also add or delete tools to customize the toolbars.SolidWorks Fundamentals Toolbars You can access SolidWorks functions using toolbars. by default. has different tabs defined for its tasks. or float them anywhere on your screen. When you click a tab below the CommandManager.
and sketches. entities in the graphics area. 19 . you can use mouse gestures to invoke mapped commands quickly. Mouse You can use a mouse gesture as a shortcut to execute a command. right-drag in the gesture direction that corresponds to the command. Displays the context-sensitive shortcut menus. similar gestures to a keyboard shortcut.SolidWorks Fundamentals Context Toolbars Context toolbars appear when you select items in the graphics area or FeatureManager design tree. pans. and pans in a drawing. They provide access to frequently performed actions for that context. Mouse Buttons Mouse buttons operate in the following ways: Left Right Middle Selects menu items. Once you learn command mappings. To activate a mouse gesture. assemblies. Rotates. Context toolbars are available for parts. and zooms a part or an assembly. and objects in the FeatureManager design tree. from the graphics area.
Handles You can use the PropertyManager to set values such as the depth of an extrude. 20 .SolidWorks Fundamentals When you right-drag. Customizing the User Interface You can customize the toolbars. keyboard shortcuts. and other elements of the user interface. Sketch guide with eight gestures Drawings guide with eight gestures The guide highlights the command you are about to select. showing the command mappings for the gesture directions. see the Customizing SolidWorks tutorial. For a lesson on customizing the SolidWorks user interface. a guide appears. You can also use graphic handles to drag and set parameters dynamically without leaving the graphics area. menus.
or a face. a vertex. cut extrudes. For example: Indicates a rectangular sketch. providing data about the type of sketch entity and the position of the pointer relative to other sketch entities.SolidWorks Fundamentals Previews With most features. Loft preview Pointer Feedback In the SolidWorks application. Previews are displayed with features such as base or boss extrudes. Indicates the midpoint of a sketch line or edge. and surfaces. the pointer changes to show the type of object. for example. sweeps. patterns. the pointer changes dynamically. an edge. 21 . In sketches. the graphics area displays a preview of the feature you want to create. lofts.
For example. You can also use the selection filter to select specific drawing annotations. For more information on using filters. if you make a boss with a hole in it. Develop the model based on the concepts. The tool hides the obscuring entities or lets you select from a list of obscured entities. see Selection Filter in the Help. Edit the model. Additionally. Conceptualize the model based on the identified needs. Construct the model. and geometric tolerances. a feature that rounds off edges. Design Process The design process usually involves the following steps: • • • • • • • Identify the model requirements. if needed. thereby excluding selection of other entity types in the graphics area. surfaces. such as notes and balloons. the hole should move when the boss moves: Original part Design intent maintained when boss moves Design intent not maintained when boss moves 22 . Filters are not restricted to entities such as faces. Analyze the model. you can select a loop composed of multiple adjacent edges. to apply a fillet. For example. or axes. Design Intent Design intent determines how you want your model to react as a result of the changes you need to make to the model. Prototype the model. you can select multiple entities using selection filters. For example. weld symbols. Select Other Use the Select other tool to select entities that are visually obscured by other entities. to select an edge in a complex part or assembly. select Filter Edges to exclude other entities.SolidWorks Fundamentals Selection Filters Selection filters help you select a particular type of entity.
A sketch is a 2D profile or cross section. you use a plane or a planar face. determine the best features to apply. you can combine and mate the appropriate parts to create an assembly. The closer your design implementation is to your design intent. you can create features. Then. however. and decide in what order to apply those features. Anticipate potential requirements to minimize redesign efforts. you can develop the model: Sketches Features Create the sketches and decide how to dimension and where to apply relations. you can also create 3D sketches that include a Z axis. include assemblies. To create a 2D sketch. From the sketch. In addition to 2D sketches. After you identify needs and isolate the appropriate concepts. From the parts or assemblies. including: Current needs Future considerations Understand the purpose of the model to design it efficiently. Various factors contribute to the design process. There are various ways of creating a sketch. such as extrudes and fillets. Design Method Before you actually design the model. Select the components to mate and the types of mates to apply. you can then create drawings. How you create the model determines how changes affect it. it is helpful to plan out a method of how to create the model. Select the appropriate features. Assemblies Sketches The sketch is the basis for most 3D models. the greater the integrity of the model. as well as the X and Y axes. You can combine one or more features to make a part. Creating a model usually begins with a sketch. Not all models. All sketches include the following elements: 23 .SolidWorks Fundamentals Design intent is primarily about planning. A model almost always includes one or more sketches and one or more features.
24 . which provides an anchor for the sketch. Symmetry is an important tool to help create your axis-symmetric models quicker. selecting the correct initial plane on which to sketch helps you create a more efficient model. On some models. The centerline is sketched through the origin and is used to create the revolve. You can sketch on planes with sketch tools such as the Line or Rectangle tool and create a section view of a model. The sketch on the right also includes a centerline. With other models. You can also use a centerline to apply a mirror relation and to establish equal and symmetrical relations between sketch entities. see Where to Start a Sketch in the Help. You can also add and position planes as needed. top. you start the sketch at the origin. Planes You can create planes in part or assembly documents. the plane you sketch on affects only the way the model appears in a standard isometric view (3D). It does not affect the design intent. a centerline helps to establish symmetry. Choose a plane on which to sketch. This example uses the top plane.SolidWorks Fundamentals Origin In many instances. and right orientations. For more information on planes. Although a centerline is not always needed in a sketch. The standard planes are front.
See Design Intent on page 22. in the faucet handle. you can change the height of the faucet handle from 40mm to 55mm. For example. Note how the shape of the revolved part changes because the spline is not dimensioned. you need to dimension the spline.SolidWorks Fundamentals Dimensions You can specify dimensions between entities such as lengths and radii. Depending on how you dimension the part. 25 . To maintain a uniform shape generated by the spline. The software uses two types of dimensions: driving dimensions and driven dimensions. Driving Dimensions You create driving dimensions with the Dimension tool. the size and shape of the part changes. you can preserve the design intent. Driving dimensions change the size of the model when you change their values. When you change dimensions.
See Relations on page 28 for more information. You control design intent by where you place the driving dimensions and relations. if you dimension the total height as 40mm. the vertical segment above the spline is calculated as 8mm (as shown by the driven dimension).SolidWorks Fundamentals Driven Dimensions Some dimensions associated with the model are driven. for informational purposes using the Dimension tool. In the faucet handle. the vertical section below the spline as 7mm. Changing the 25mm dimension to a driven dimension removes the conflict and shows that the spline length must be 26mm. You cannot modify the values of driven dimensions directly unless you convert them to driving dimensions. and the spline segment as 25mm. The 25mm vertical dimension conflicts with the other dimensions and relations (because 40-7-7=26. if you dimension the total height as 40mm and create an equal relation between the top and bottom vertical segments. or reference dimensions. not 25). 26 . For example. The value of driven dimensions changes when you modify driving dimensions or relations in the model. the top segment becomes 7mm. You can create driven.
You do not have to fully define sketches before you use them to create features. Over defined sketches include redundant dimensions or relations that are in conflict. This sketch is over defined because both vertical lines of the rectangle are dimensioned. are described by dimensions or relations. only one 35mm dimension is necessary. 27 . You can delete over defined dimensions or relations. entities in under defined sketches are not fixed within the sketch. Over defined sketches appear in yellow. a rectangle has two sets of equal sides. By displaying the entities of the sketch that are under defined. In fully defined sketches. In addition to color cues. Fully defined sketches appear in black. but you cannot edit them. so you can drag them. By definition. and their positions. However. or over defined. under defined. Therefore.SolidWorks Fundamentals Sketch Definitions Sketches can be fully defined. all the lines and curves in the sketch. you can determine what dimensions or relations you need to add to fully define the sketch. You can use the color cues to determine if a sketch is under defined. or both. Under defined sketches appear in blue. you should fully define sketches to maintain your design intent.
For example. The green symbols indicate that there is an equal relation between the horizontal lines: Relations are saved with the sketch.SolidWorks Fundamentals Relations Relations establish geometric relationships such as equality and tangency between sketch entities. 28 . You can apply relations in the following ways: Inference Some relations are created by inference. as you sketch the two horizontal entities to create the base extrude for the faucet base. as well as other types of slots. This example shows the concept of relations. For example. You can dimension each horizontal entity individually. but by establishing an equal relation between the two horizontal entities. you need to update only one dimension if the length changes. you can establish equality between the two horizontal 100mm entities below. horizontal and parallel relations are created by inference. The SolidWorks application has a sketch slot tool to make this shape easily.
to create the faucet Add Relations stems. you also add a concentric relation between the inner and outer arcs. You can also take advantage of repetition and symmetry. For each stem. One way to simplify sketching is to apply relations as you sketch.SolidWorks Fundamentals You can also use the Add Relations tool. and it rebuilds quicker. For example. Sketch Complexity A simple sketch is easy to create and update. you add a tangent relation between the outer arcs and the top construction line horizontal (displayed as a broken line). the faucet stems on the faucet base include repeated sketched circles: Here is one way you can create this sketch: 29 . you sketch a pair of arcs for each stem. For example. To position the stems.
30 . Construction geometry is used only to assist in creating the sketch entities and geometry that are ultimately incorporated into the part. Finally. dimension and add a concentric relation between one of the circles and the outer arc of the base. sketch a circle by inferencing the sketch origin. When you use dynamic mirroring with the centerline. Second. This centerline is considered construction geometry. Centerlines help to create symmetrical sketch entities. You create the circles on the left and they are mirrored to the right of the centerline. which is different from actual geometry that is used in creating a part. anything you sketch on one side is mirrored on the other side of the centerline.SolidWorks Fundamentals First. use the Dynamic Mirror tool to designate the centerline as the entity about which to mirror the sketched circles. and then use symmetry for the other. Next. sketch a centerline through the origin.
cuts. For example. Create the sketch Dimension the sketch Extrude the sketch 10mm Some sketch-based features are shapes such as bosses. you create parts by including sketch-based features such as bosses and holes. you can create a 3D model using features such as an extrude (the base of the faucet) or a revolve (the faucet handle). Typically. Other sketch-based features such as lofts and sweeps use a profile along a path. Another type of feature is called an applied feature. you can import a body or use a derived sketch.SolidWorks Fundamentals Features Once you complete the sketch. Then you add applied features. 31 . Applied features include fillets. It is possible to create a part without sketch-based features. or shells. They are called "applied" because they are applied to existing geometry using dimensions and other characteristics to create the feature. and holes. which does not require a sketch. chamfers. The exercises in this document show sketch-based features.
Assemblies You can combine multiple parts that fit together to create assemblies. For more information on features. With tools such as Move Component or Rotate Component. To ensure that the assembly functions correctly. you can select between different features such as sweeps or lofts to achieve the same results and you can add features to a model in a specific order. In the faucet assembly. Mates define the allowable direction of movement of the components. For example. 32 . you can see how the parts in an assembly function in a 3D context. you can use assembly tools such as Collision Detection. Collision Detection lets you find collisions with other components when moving or rotating a component. see Parts on page 36.SolidWorks Fundamentals Sketch-based features: Base sweep for the waste pipe Applied feature: Fillets for rounding off edges Several factors influence how you choose which features to use. the faucet base and handles have concentric and coincident mates. You integrate the parts in an assembly using Mates. such as Concentric and Coincident.
Editing capabilities include: Edit sketch You can select a sketch in the FeatureManager design tree and edit it. view or delete existing relations. change dimensions. You can import the dimensions from the model document and add annotations such as datum target symbols. parts. For example. add new relations between sketch entities. Drawings are available in multiple views such as standard 3 views and isometric views (3D). you can edit sketch entities. or assemblies. You can also edit features and sketches by selecting them directly from the graphics area. drawings. Model Editing Use the SolidWorks FeatureManager design tree and the PropertyManager to edit sketches. or change 33 . Stop at collision option enabled Drawings You create drawings from part or assembly models.SolidWorks Fundamentals Faucet assembly with Collision Detection. This visual approach eliminates the need to know the name of the feature.
Use Edit Feature to display the appropriate PropertyManager.SolidWorks Fundamentals the size of dimension displays. You can also select the feature to edit directly from the graphics area. For example. No fillet feature Fillet feature: 12mm applied Fillet feature: 18mm applied Hide and show With certain geometry such as multiple surface bodies in a single model. if you apply a Constant radius fillet to an edge. Edit feature Once you create a feature. You can also edit dimensions by double-clicking the feature or sketch in the graphics area to show the dimensions and then change them in place. you can hide or show one or more surface bodies. you display the Fillet PropertyManager where you can change the radius. you can change most of its values. You can hide and show 34 .
Moving the rollback bar displays all features in the model up to the rollback state. and views. you can roll the FeatureManager design tree back to a prior state. Rollback When you are working on a model with multiple features. You can suppress and unsuppress components in assemblies as well (see Assembly Design Methods on page 55). Rollback is useful for inserting features before other features. until you revert the FeatureManager design tree back to its original state. 35 . Suppress You can select any feature from the FeatureManager design tree and and suppress the feature to view the model without that feature. or learning how a model was built. The feature disappears from the model view. and components in drawings. and axes in all documents. When a feature unsuppress is suppressed. it is temporarily removed from the model (but not deleted).SolidWorks Fundamentals sketches. You can then unsuppress the feature to display the model in its original state. planes. lines. speeding up time to rebuild a model while editing it.
2 Parts Parts are the building blocks of every SolidWorks model. Each assembly and drawing you create is made from parts. This chapter includes the following topics: • • • • • • • Overview Countertop Faucet Faucet Handle Cabinet Door Moldings Hinge 36 .
Extrude 2. including a high-level overview of the tools that create the part. This countertop uses several common SolidWorks tools. First you create the counter. so you can skim those that you already understand. you learn about common tools for making parts in the SolidWorks software. You will see these parts in later sections.Parts Overview In this section. Fillet 37 . Loft 5. These tools are used for many parts. Countertop The countertop is a single part that includes a sink and counter. then you make the sink. Design Approach 1. and fillets. Extrude 3. waste pipe. so they are discussed in detail only the first time they appear. including extrudes. Shell 6. The cabinet. and supply pipes used in the vanity are not discussed in this section because they repeat the tools already presented. Cut-Extrude 4. a sweep. a shell. The overview provides an outline of the features. Each section begins with the design approach for each part.
0) coordinate of a 2D sketch. The sketch is extruded 34mm normal to the sketch plane. When you add dimensions and relations to the sketch. This model is displayed in an isometric view so you can see the model structure. The origin is a helpful reference point for sketches. If you begin a sketch at the origin. 38 . first make the 2D sketch. this rectangular sketch is dimensioned at 600mm x 580mm. it becomes fully defined. For example. the sketch position is set. After you sketch the rectangle. The sketch begins at the origin. the (0. To design a 3D model. you need to make a sketch. then create the 3D feature. use the Extrude tool to create a 3D base feature.Parts Create the Base Feature with an Extrude Before you create an extrude feature.
the left and upper edges are projected. The Convert Entities tool lets you create a sketch by projecting a set of edges onto the sketch plane.Parts Add an Extrude to the Base The second extrude adds material to a part by building upon the base. In this example. the countertop has an opening for the sink. except that it removes material from the model instead of adding material. Next. First you create a 2D sketch. Remove Material with the Cut-Extrude The Cut-Extrude tool is similar to an extrude feature. In this example. then you make the cut-extrude. 39 . you create the sketch for the extrude with the Convert Entities tool. When the cut-extrude is complete. you use the Ellipse tool to make an oblong sketch. First. you extrude two of the countertop edges. you use the Extrude tool to create the countertop edges. In this example.
First. Second. Now that you have two sketch profiles. see the Lesson 1 . create a new plane. by offsetting it from the Top plane. the loft creates the sink by connecting an elliptical sketch and a circular sketch. In this example. Plane1.Parts For a lesson that includes extrude features. you create the sink with the Loft tool.Parts tutorial. This tool creates a sketch by projecting the existing ellipse from the Cut-Extrude onto the bottom of the countertop. Plane1 is parallel to the Top plane. The SolidWorks software uses a shaded preview to illustrate what the model will look like before you accept the feature. use the Loft tool to connect them. A loft creates a feature by making transitions between two or more sketch profiles. use the Circle tool to sketch a circle on Plane1. Use a Loft to Make a Solid After you make the cut-extrude feature. Next. When you create a loft. the sketch profiles must reside on different planes (or planar faces). 40 . create a sketched ellipse on the bottom of the countertop with the Convert Entities tool.
you round off sharp edges by adding fillet features to the model.Parts tutorial. see the Lesson 1 .Parts For a lesson on lofts. When you shell a part in SolidWorks. and create the fillet. For a lesson on fillets. Instead. you need to cut out material to make the sink. see the Lofts tutorial. not sketch features. The Shell tool hollows out the sink and removes the top face. This means that fillets do not require you to create a sketch. Round Sharp Edges with Fillets To complete the countertop. after all of the geometry is in place. Fillets are applied features. It is best to save cosmetic fillets for the last step. selected faces are removed and thin faces remain on the rest of the part. the edges or faces become rounder. you set the radius to determine the smoothness of the edges. set the fillet radius. 41 . see the Fillets tutorial. For a lesson that includes shells. Models rebuild faster when fillets are made at the end of the design process. When you create a fillet. Shell the Part Because the loft creates a solid feature. As you increase the radius. you select the edges of an existing feature.
Design Approach 1. Extrude 3. a sweep creates the faucet spigot. The faucet uses these tools. Extrude 2.Parts Faucet Most parts have extrude and fillet features. In the following example. Sweep 4. in addition to a sweep. Additional Extrudes and Fillets 42 .
the profile is a circular sketch. In this example. although the revolves require detailed sketches. Sweep preview: After you create some additional extrudes and fillets as shown. and the path is a sketched arc that is tangent to a vertical line.Parts Create the Sweep The faucet base is made from two extrude features. The Revolve tool revolves a 43 . When you sketch the profile and path. The model uses a simple design approach. The circular profile remains the same shape and diameter for the entire sweep. Use the Sweep tool to make the spigot by projecting a profile along a path. the model appears as shown. After you create the two extrudes. make sure the starting point of the path lies on the same plane as the profile. Faucet Handle The faucet handle is built with two revolve features. the faucet is complete.
Revolve 2. 44 .Parts sketch profile around a centerline at a specified angle. Revolve 3. Fillets Revolve the Sketch Create the First Revolve A revolve creates the base of the handle. the revolve angles are set to 360°. In the following examples. Design Approach 1. and completes the first feature in the faucet handle.
Parts First. you create a sketch with the Line and Spline tools. 45 . you can add an axis of revolution with the Centerline tool. A centerline creates an axis that is construction geometry. In some cases. You then use the Revolve tool to rotate the sketch and create a solid feature. Create the Second Revolve You create a second revolve feature to add the faucet handle. it is not built into the feature.
For a lesson on revolves. as shown. After you add cosmetic fillets. Chamfer 46 . you begin with a sketch. Cabinet Door The cabinet door uses an extrude and a cut-extrude to make the exterior detail. the faucet handle is complete. see the Revolves and Sweeps tutorial. and Spline tools. This sketch uses the Line. Design Approach 1. Extrude 2. then create a 3D solid with the revolve. The Revolve tool revolves the sketch to generate a solid. Cut-Extrude 3.Parts Again. Tangent Arc.
Mirror 4. although there are four pieces of molding on the door. you create the different molding lengths within one part. and a mirror feature. is an applied feature. like a fillet. Configurations 47 . With configurations. and does not require you to make a sketch to create the feature. A chamfer.Parts Create Beveled Edges with the Chamfer Tool The Chamfer tool creates beveled faces. Moldings The moldings around the edges of the door use an extruded sketch. Cut-Extrude 3. see Chamfer Feature in the Help. In this example. the face with the extruded cut has chamfered edges. Extrude 2. Design Approach 1. Only one part file is created. For more information on chamfers. an extruded cut.
Mirror the Cut Finally.Parts Design a Mid-Plane Extrude The molding sketch uses a mid-plane extrusion. you cut the molding at a 45° angle. you extrude the sketch equally in both directions perpendicular to the sketch plane. The 45° cut ensures that the molding pieces fit together accurately. use the Mirror tool to mirror the original cut about the plane of symmetry. Instead of extruding the sketch in one direction. to cut the model at the same angle on the opposite side. 48 . When you sketch a profile to cut. it ensures that you have equal lengths of material on both sides of the sketch. Sketch a Profile for the Cut-Extrude Next. make the sketch larger than the model so that you make a clean cut through the entire molding. Although you do not have to use a mid-plane extrusion.
and it designates the part as sheet metal. The SolidWorks ConfigurationManager displays the two configurations in the document. When you design sheet metal in the SolidWorks software. The SolidWorks software has several tools that are specific to sheet metal. rename the default configuration to short. When you design a part. the default configuration matches the length of the shorter sides of the door. By definition. When you double-click a configuration name. the graphics area displays that configuration. In the molding that you created. The base flange is the first feature in a sheet metal part. you insert different configurations of the same part into an assembly.Parts Use Configurations of a Part Configurations create multiple variations of a part within a single part file. see the Advanced Design tutorial. the SolidWorks software automatically creates the Default configuration. For a lesson that includes mirroring and configurations. 49 . To easily identify the configuration. Hinge The hinge connecting the cabinet door to the vanity is a sheet metal part. you can use a base flange instead of an extrude to create the base of the part. which you use in the hinge design. including the tab and the hem. sheet metal parts are constructed of uniform thickness and have a specified bend radius. This configuration increases the length to match the longer sides of the door. In the same document you create another configuration and name it long. Later on.
In the hinge. you first create a sketch. Hem Create Sheet Metal with the Base Flange As with other base features.Parts Design Approach 1. Make the Tab The Tab tool adds a tab to the sheet metal part. 50 . Next. The base of the hinge is an example where a simple sketch allows for easier creation of the model. you use the Base Flange/Tab tool to automatically create a sheet metal part. you make a sketch with the Rectangle tool. Tab 3. Base Flange 2. The depth of the tab automatically matches the thickness of the sheet metal part. The direction of the depth automatically coincides with the sheet metal part to prevent a disjoint body. Linear Pattern 4.
see Sheet Metal Tab in the help. After you complete the sketch. When you create the second piece. In the hinge. use the Linear Pattern tool to copy the original tab a specified number of times. The linear pattern creates multiple instances of a selected feature along a linear path. When you make a linear pattern. 51 . you specify the number of instances and the distance between each tab. For more information on tabs. use the Base Flange/Tab tool to add the tab. You make this sketch with the Rectangle tool on the front face. you change the location of the tabs so both pieces fit together.Parts When you make the sketch for the tab. Generate the Linear Pattern To make tabs that span the length of the hinge. there are 13 tabs separated by 50mm. This is the first piece of the hinge. you sketch on the face where you want the tab to appear.
Parts For more information. Alternate Design Approach Another way to design the hinge is to build the rolled section as part of the base flange. In this example. you do not need the Hem tool. Add the Hem A Hem is a sheet metal tool that folds the edge of a part and uses the same model thickness as the base flange. For a lesson on sheet metal. see Linear Patterns in the Help. In this example. see the Sheet Metal tutorial. 52 . you add a rolled hem to each tab to curl the sheet metal.
and position. 53 .Parts First. Next. create a sketch with the Line and Tangent Arc tools. Second. Finally. use the Linear Pattern tool to create multiple cuts. create the first tab with an extruded cut. Using the Hem tool gives you more flexibility if you need to change the radius. extrude the sketch with the Base Flange tool. hem type.
you use the vanity cabinet parts described and built in Parts on page 36 to build subassemblies. Then you bring the subassemblies together to create an assembly. This chapter includes the following topics: • • • • • • • Assembly Definition Assembly Design Methods Prepare an Assembly Mates In-Context Design Load an Assembly Examine the Assembly Assembly Definition An assembly is a collection of related parts saved in one SolidWorks document file with a . Assemblies: • Contain anywhere from two to over one thousand components. such as the spigot and the faucet handles.3 Assemblies In this section. which can be parts or other assemblies called subassemblies • Display movement between related parts within their degrees of freedom 54 .sldasm extension. the vanity.
Then you open an assembly document. the fixture is updated automatically. The mated components create the spigot subassembly. Working top-down. mating it to the other components in the vanity assembly. so you can control the dimensions of the fixture by creating geometric relations to the original part. insert them into an assembly. It is a good method to use if you do not need to create references that control the size or shape of parts with respect to each other. For instance. and add various mates. then design the parts referencing these definitions. With either method. your objective is to mate the components to create the assembly or subassembly (see Mates on page 57).Assemblies The components in an assembly are defined in relation to each other using assembly mates. off-the-shelf parts. For example. For example. the faucet handle components are mated to the faucet base component using concentric and coincident mates. Working bottom-up allows you to focus on the individual parts. You create the components such as the sink and the spigot in their own part windows. Later. 55 . if you change a dimension of the part. and mate them as required by your design. Most of the vanity cabinet uses bottom-up design. You can also use a combination of the two methods. concentric. you can insert a part in an assembly. Assembly Design Methods You create assemblies using two basic methods: bottom-up design and top-down design. you include this subassembly in the main vanity assembly. You attach the assembly components using various types of mates such as coincident. Bottom-up design is the preferred technique when you use previously constructed. their relationships and regeneration behavior are simpler than in top-down design. you start your work in the assembly. bring the components into the assembly. and distance mates. The vanity cabinet also uses top-down design. Top-down Design In top-down design. You create the two supply pipes within the context of the assembly. or to create machined features that are added only after the parts are assembled. to create features that affect multiple parts. That way. you create parts. You can use the geometry of one part to help define other parts. allows you to reference model geometry. Top-down design is also known as in-context design. creating the fixture in context. you can start with a layout sketch or define fixed part locations. An advantage of bottom-up design is that because components are designed independently. Bottom-up Design In bottom-up design. Then you reference the size and location of the faucet subassembly and the vanity cabinet to define the supply pipes. then build a fixture based on this part.
you need to prepare the assembly components. The vanity includes the following subassemblies: • Faucet and faucet handles • Door and moldings • Door subassembly. and hinge 56 .Assemblies Supply pipes Prepare an Assembly Before you build an assembly. you use the parts for the vanity cabinet created in Parts on page 36. Throughout this section. cabinet.
and hinge For each subassembly document. perpendicular. and extrusions. concentric. cabinet. the valid types of mates you can use include coincident. and distance (see Coincident Mate on page 60). if you mate a cone to another cone. planes. you do the following prior to mating the components: • Load and anchor the first component to the assembly origin • Load the additional components • Move and position the components Mates Mates position the components in an assembly precisely with respect to each other. 57 . Mates create geometric relations. For example. cylinders. Each mate is valid for specific combinations of geometry such as cones. such as coincident. Positioning the components defines how they move and rotate with respect to each other. and tangent.Assemblies Faucet and faucet handles Door and moldings Door subassembly.
To position the components. you need to open a new assembly document into which you bring the components.sldasm document. you can open one or all of your components. This is the component you anchor or fix to the assembly origin. Anchoring the first component ensures that the planes in both documents are aligned. you apply a coincident mate and a concentric mate.Assemblies Faucet Subassembly Depending on the complexity of the assembly (the number of separate components). there are only two components (the faucet and the handle). so the handle sits on the faucet. start with the component that does not move with respect to the other components. so you can tile the two documents.sldprt document and drag it into the . 58 .sldasm document as follows: • Select the component name in the FeatureManager design tree of the . you anchor the faucet component. In the example of the faucet subassembly. drop it on the origin in the graphics area or anywhere in the FeatureManager design tree.sldasm document. • To position the first component on the origin of the . Dropping it in the FeatureManager design tree requires less fine mouse movement and will automatically align the part's origin and the assembly origin. In the faucet example. You want to place the bottom of the handle component on the flat base of the faucet component. After you open the components. You can add more than one instance of the same part to an assembly. You do not have to create a unique part for each component in the assembly. Bring the first component into the . You also need to center the handle components over the faucet stems to position them correctly. Load the First Assembly Component When creating an assembly.
Load the Additional Components You load the other components of the assembly by selecting the component in the FeatureManager design tree of the . which is useful for mating of components.sldasm document. you can change which component is fixed later.sldasm document. The first component you add to an assembly is fixed in space by default. It is common to choose a component that you wish to be fixed. however. the component appears in the FeatureManager design tree.sldprt document. and dragging the component into the graphics area of the . you drag in two instances of the handle. In the example of the faucet subassembly.Assemblies As you bring each component into the . Faucet component with origin (assembly origin and component origin) First handle component added Second handle component added 59 .
Concentric Mate Select any round face on the faucet handle. indicating that a second mate is required to further define the position of the two components. Leave some space between components to view the relevant component areas. • Middle mouse button with Ctrl: Pans all components. Coincident Mate To create a coincident mate between the handle component and the faucet component. Then you can use the left mouse button to drag a component closer to the first. attach the flat bottom face of the handles to the flat top face of the faucet. • Middle mouse wheel: Zooms all components in or out.Assemblies Position the Additional Components When you bring the additional components into the assembly. You can use the right mouse button to rotate a component into the proper orientation. Note that you can still slide the handle anywhere along the top face of the faucet by dragging it with the left mouse button. You can use the following methods to change the orientation of the components: • Middle mouse button: Rotates all components. 60 . or other entities needed to apply mates. These mouse functions help select edges. anchored component. the faucet handle component moves closer to the faucet component. you can position them anywhere in the graphics area. faces. Flat bottom face of the faucet handles Flat top face of the faucet base component When you apply the coincident mate. Then select the round face of the faucet stem (the portion of the component that slides into the counter top. and connects to the supply pipe).
SmartMates automatically infer mate partners and eliminate the need to use the Mate PropertyManager. use the left mouse button to drag the faucet handle on its axis. With SmartMates. however. Faucet Subassembly . SmartMates are based on the entity you use to drag the component. For a lesson on assembly mates.Assemblies Round face on the faucet handle Round face on the stem Once you apply the concentric mate between the faucet handle component and the faucet component. you infer the geometry of existing components to create mates. You can use geometry-based SmartMates to create coincident mates between planar faces. Use Alt and drag the bottom face of the handle to create a coincident mate between the handle and faucet. You can. There are different types of SmartMates. For example. use SmartMates to create a coincident mate between the faucet component and each of the faucet handles in the faucet subassembly.Alternate Design Approach Another approach to mating the faucet and handle components is to use SmartMates. the system automatically creates some mates. 61 . When you drag components into assemblies. see the Assembly Mates tutorial. you can no longer move the faucet handle along the top face of the faucet to shift its position.
or other parameters (see Use Configurations of a Part on page 49). 62 . Configurations provide a convenient way to develop and manage families of models with different dimensions. see SmartMates Overview in the Help. including feature-based SmartMates and pattern-based SmartMates. Configurations let you create multiple variations of a part or an assembly within a single document. As stated earlier. The door subassembly uses configurations.Assemblies You can use another type of geometry-based SmartMate to create the concentric mate between the two round faces to completely define the faucet subassembly. Two of the instances use the short configuration and fit across the short sides of the door. There are other types of SmartMates. components. Door Subassembly The cabinet door uses coincident mates between the door component and the four molding components. The other two instances use the long configuration. It also uses configurations of the molding as a time-saving design step. For more information. Each instance of the part can also use a different configuration. There are four instances of the molding component. you can use the same part more than once in an assembly.
so that it functions freely. you can position the hinge using a distance mate. It also uses a distance mate between the cabinet and one of the hinge components. you can determine at what position to place the hinge so that it does not bind when you open the cabinet door.Assemblies Door subassembly with molding components Cabinet Subassembly The cabinet subassembly uses concentric and coincident mates. By measuring the entities of different components. In the vanity cabinet. 63 . You determine the correct mate distance using the Measure tool. Distance Mate A distance mate uses a value you assign to separate the two entities. Once you know the thickness of the door opening and the width of the hinge. the distance mate positions the hinge optimally.
Measure the width of the inside for the cabinet door opening.
Measure the width of the hinge that you attach to the inside of the cabinet door opening.
Apply a distance mate, based on measurements of the cabinet and of the hinge.
In-Context Design
You can create a new part within an assembly document (in the context of an assembly). In addition to creating or editing components in their own part windows, the SolidWorks software lets you create or edit components in the assembly window. The advantage is that you can reference the geometry of one component to create or modify another component. By referencing the geometry of another component, you ensure that the components fit together correctly. This method of design is called top-down or in-context design because you are working in the context of the assembly. In the vanity assembly, there are two examples of in-context design. One example is the diameter of the supply pipe component and the waste pipe component. The pipe components are both new parts that you create in the context of the assembly. The other example is the cut feature for the holes in the back of the vanity cabinet. The vanity
cabinet is an existing part that you edit in the context of the assembly. These examples are discussed in the next two sections. As you create an in-context part, the software includes notations and options with information about the relationships in the features. For more information on creating in-context components, see Creating a Part in an Assembly in the Help.
Create an Assembly Component In-Context
The diameter of the supply pipe component depends on the diameter of the faucet stem. It is a good idea to create the supply pipe component in the assembly so you can reference the geometry of the faucet stem. You use the Convert Entities and Offset Entities sketch tools to reference the geometry of the faucet stem for a sketch in the supply pipe component. This reference ensures that the size of the supply pipe changes if you change the size of the faucet stem. You can use the same method to create the waste pipe component, which depends on the diameter of the exit stem at the bottom of the basin.
Use Convert Entities and Offset Entities Extrude the sketch to create the sleeve between the faucet stem and the supply to create the sleeve between the faucet pipe. stem and the supply pipe.
Modify a Part In-Context of an Assembly
The positions of the holes in the back of the vanity cabinet depend on the length of the supply pipe and the waste pipe components. It is a good idea to edit the vanity cabinet component in the assembly so you can reference the geometry of the supply pipes and waste pipe. You use the Offset Entities sketch tool to reference the geometry of the pipes for a sketch of the cut in the vanity cabinet component. This reference ensures that the position and size of the holes changes if you change the position and size of the supply pipes or waste pipe.
Supply and waste piping before in-context Supply and waste piping after in-context cut cut
Load an Assembly
You can improve performance of large assemblies significantly by using lightweight components. After you create an assembly, you can load it with its active components fully resolved or lightweight. • When a component is fully resolved, all of its model data is loaded in memory. • When a component is lightweight, only a subset of its model data is loaded in memory. The remaining model data is loaded on an as-needed basis. Loading an assembly with lightweight components is faster than loading the same assembly with fully resolved components. Lightweight components are efficient because the full model data for the components is loaded only as it is needed. Assemblies with lightweight components rebuild faster because fewer details are evaluated. However, mates on a lightweight component are solved, and you can edit existing mates. The vanity cabinet is a relatively simple assembly, so any performance gains using lightweight components are minimal.
Examine the Assembly
The SolidWorks software includes various assembly tools that can display, test, and measure your assembly components once you apply the mates. Some of the assembly tools include:
Hide and Show Components
You can hide or show components in the graphics area. Hiding components often facilitates component selection when you add mates or when you create in-context parts. For example, to select the inner and outer diameters of the faucet stems, you can hide all
Hide all components except the one you need Zoom. 67 . rotate. They affect only the display. rotate. and change the view if necessary to select the feature Hide Components and Show Components do not affect the mates between the components. and then zoom. or change the view as needed.Assemblies components except the faucet subassembly.
what distances to use. and in which direction to display the exploded components. The exploded view is saved with a configuration of the assembly or subassembly. Exploded views include many options such as which components to include. In the faucet subassembly. The SolidWorks software can detect collisions with the entire assembly or a selected group of components that move as a result of mates. You can set the Stop at collision option to determine where the components collide. note how the faucet handles collide with the faucet.Assemblies Explode the Assembly An exploded view separates the components in an assembly to facilitate viewing. 68 . Detect Collisions Between Components You can detect collisions with other components when you move or rotate a component.
Notice the handle moves inside the faucet. Collision Detection with Stop at collision active. Notice the handle cannot move inside the faucet. 69 .Assemblies Normal position of handles Collision Detection without Stop at collision active.
4 Drawings Drawings are 2D documents that convey a design to manufacturing. This chapter includes the following topics: • • • • Drawing Documents Vanity Cabinet Drawing Sheet Faucet Assembly Drawing Sheet Vanity Assembly Drawing Sheet Drawing Documents You create drawings from drawing templates. The drawing sheets have underlying formats. Within a drawing document are drawing sheets that contain drawing views. 70 .
You can create custom drawing templates with any of the following characteristics: • • • • Drawing sheet size (for example. you open a drawing template. The standard drawing sheet formats contain borders and title blocks for the C-size landscape format: 71 . Drawing templates contain basic document information. author's name. B. millimeters and inches) Company name and logo. and C) Drawing standard (for example. A. You choose from templates supplied with the SolidWorks software containing default drawing sheets or templates you customize. The sheet format controls: • • • • Size of the drawing sheet Drawing borders Title block Sheet scale Drawing Templates To start the drawing document. the size of the drawing is undefined. ISO and ANSI) Units (for example.Drawings Drawing templates and sheet formats are two distinct entities. When you begin a new drawing using the default drawing template. The software prompts you to select a sheet format. and other information Drawing Sheets For the vanity drawings. The software comes with one drawing template and a set of sheet formats (in English and metric). a drawing template with a C-size drawing sheet in landscape orientation is appropriate.
and editing and adding notes. like a set of drawings. You can link the notes to system properties and custom properties. 72 . The sheet format underlies the drawing sheet and is separate from the drawing sheet. You edit the sheet format separately from the drawing sheet. After changing the sheet scale. You can add sheets at any time using any format. and the bill of materials anchor point. Sheet Formats The bottom right corner of the default sheet format contains a title block. Drawing Views Drawing views are placed on drawing sheets and contain the images of the models. plus dimensions and annotations. the title block appears as shown. adding two sheets. note text.Drawings The drawing document for the vanity contains three sheets. regardless of the format of other sheets in the document. You can have any number of drawing sheets in a drawing document. The scale and page numbers are linked to system variables and updated automatically. Sheet formats can contain items such as lines. Tabs with sheet names appear at the bottom of the graphics area. bitmaps.
In first angle projection. top. The example in this section uses third angle projection. and left (first angle projection). comprise three views: front. see the Lesson 3 . You can insert these views from an open part or assembly document. you can derive other types of views. and adding dimensions to drawings. top. For a lesson on drawing documents. from a file. In third angle projection. top. For more information on document templates. see the Help. drawing sheets. inserting standard views. the default front view is displayed at the lower left. such as projected. Standard 3 Views Standard 3 views.Drawings tutorial. 73 . front. or from other views in the same drawing document. and drawing views. Standard Views Drawings generally start with a standard 3 view or some type of named view.Drawings Drawings begin with standard views. section. The views are displayed in different modes and contain dimensions and annotations. Third angle projection is typically used in the United States. and detail. and right (third angle projection) or front. Vanity Cabinet Drawing Sheet The vanity cabinet sheet contains standard 3 views and named views that are generated from the part. First angle projection is typically used in Europe. as the name implies. for example. the front view is displayed at the upper left. From those views. or exploded. isometric.
you add an isometric view of the cabinet (a named view) to the drawing sheet.Drawings For more information on first and third angle projection. top. The standard 3 views of the vanity cabinet are the first views that are placed on this sheet. 74 . and isometric • Current model view • Custom named views Next. for example. see First Angle and Third Angle Projection in the Help. front. Named views include: • Standard orientations. Named Views Views are named in the model documents.
but not vertically.Drawings You select the view orientation as you bring the view into the drawing. Standard 3 views are aligned so that if you drag the front view. Projected Views Projected views are orthographic projections of existing views. The top view moves independently in the vertical direction. 75 . The standard 3 views are displayed with Hidden Lines Visible. View Display and Alignment You can choose various display modes for drawing views.) The isometric view is displayed with Shaded With Edges. the back view is displayed with Hidden Lines Removed. The vanity has details in the back that are important to show. (Hidden lines appear gray on screen. project the right view and place it to the right. To create a back view. but as dashed lines when printed. but not horizontally. On the Vanity Cabinet sheet. but you can break the alignments. Some views are aligned automatically. The right view moves independently in the horizontal direction. both the top and right views move with it.
You can set the units (for example. and are driven. and changing a model dimension in a drawing changes the model. see Drawing View Alignment and Display in the Help. Typically. and vice versa. For example. and aligning views. The values of reference dimensions change when the model dimensions change. then insert those dimensions into the drawing views. For more information about dimensions in drawings. The vanity is in millimeters in the ISO standard. Changes in the model are reflected in the drawing. but these are reference dimensions. which is aligned with the front view by default. millimeters or inches) and the drawing standard (for example. hiding. and auxiliary views automatically align in the direction of the view arrows. the back view of the cabinet is aligned horizontally with the right view. you cannot edit the value of reference dimensions to change the model. you create dimensions as you create each feature in a part. Dimensions Dimensions in a SolidWorks drawing are associated with the model. You can also add dimensions in the drawing document. Detail views are not aligned by default. ISO or ANSI) in the detailing options. see Dimensions Overview in the Help. For more information on displaying.Drawings Section views. 76 . Changing a dimension in the model updates the drawing. You can align views that are not automatically aligned. projected views.
Insert Model Items
You use the Insert Model Items tool as a convenient way to insert existing model dimensions into the cabinet drawing. Insert items for a selected feature, an assembly component, a drawing view, or all views. When inserted into all views (as in the example), dimensions and annotations appear in the most appropriate view. Features that appear in partial views, such as detail or section views, are dimensioned in those views first. Once you insert the dimensions, you can manipulate them. For example, you can drag them into position, drag them to other views, hide them, or edit properties. If the model contains annotations, you can also insert the annotations into drawings by the same procedure.
Reference Dimensions
The back view on the Vanity Cabinet sheet is included to show the dimensions of the holes in the cabinet for the supply and waste pipes. Reference dimensions help you to locate the holes. You can choose whether to enclose reference dimensions in parentheses automatically.
Other types of reference dimensions include baseline dimensions and ordinate dimensions. For example, you might add ordinate dimensions to the front view of the cabinet as shown. You can dimension to edges, vertices, and arcs. The dimensions jog automatically to avoid overlapping. You can display ordinate dimensions without the chain (the arrows between the dimension extension lines).
Hole Callouts
You can specify hole callouts when creating holes in models with the Hole Wizard. The Hole Wizard creates and positions holes you define for fasteners such as counterbore and countersunk screws and tap holes. Hole Wizard design data, such as diameter, depth, and counterbore, becomes part of the hole callout automatically. Hole callouts help you to specify the size and depth of the holes in the cabinet. Hole callouts are annotations that are also dimensions. These hole callouts are in the back view.
In addition to dimensions, you can add other types of annotations to your models and drawings to convey manufacturing information: • • • • • • • • • • • • Notes Geometric tolerance symbols Datum feature symbol Center marks Surface finish symbols Datum target symbols Weld symbols Balloons and stacked balloons Blocks Multi-jog leaders Area hatches Dowel pin symbols
Most annotations can be added in part and assembly documents and inserted automatically into drawings in the same way that dimensions are inserted into drawings. Some annotations (center marks, multi-jog leaders, hole callouts, area hatch, and dowel pin symbols) are available in drawings only. For more information on annotations, see Annotations Overview in the Help.
Geometric Tolerance and Datum Feature Symbols
Geometric tolerance symbols display various manufacturing specifications, often in conjunction with datum feature symbols as shown in the example. You can insert these symbols in sketches and in part, assembly, and drawing documents. In the right view of the cabinet, the back edge is specified with a geometric tolerance symbol as parallel to the front edge within 10mm.
For a lesson on adding derived views. You can rotate center marks. see the Advanced Drawings tutorial. Faucet Assembly Drawing Sheet The faucet assembly drawing sheet displays several derived views and annotations. Here is the completed vanity cabinet drawing sheet.Drawings Center Marks Center marks are annotations that mark circle or arc centers and describe the geometry size on the drawing. and exploded views to drawings. center marks are added to the holes in the back view of the cabinet. specify their sizes. Center marks can be used as reference points for dimensioning. In this example. You can place center marks on circles or arcs. and choose whether or not to display extended axis lines. annotations. 80 .
81 . With standard 3 views or a named view in a drawing. Explode lines show the relationships between assembly components. Section Views You can create a section view in a drawing by cutting the parent view with a section line. Derived Views Derived views are created from the standard views. The sectioned components automatically display crosshatching. such as aligned section views and broken-out section views.Drawings Explode Lines The faucet assembly is shown in an isometric named view in its exploded configuration. The lines are displayed in phantom line font. and angle). you can create other views without going back to the model. You can edit the properties of the crosshatching (pattern. scale. A section view of the faucet in the faucet assembly drawing shows the faucet pipe walls and connections. You add the explode lines to the assembly document in an explode line sketch. In this example. You can also jog the lines as needed. you insert a top view of the faucet assembly as the basis for the section view. There are other types of section views.
usually at an enlarged scale. The parent view is the section view. The overlay views are displayed in the drawing in phantom lines. 3D. Other drawing views include: Auxiliary view Crop view Broken-out section A projection normal to a reference edge Everything outside a sketched profile removed Material inside a profile removed to expose inner details Broken view Portion of a long part with a uniform cross-section removed 82 . often to show range of motion of an assembly component. The faucet handles are shown on the faucet assembly sheet in an alternate position view to display the range of motion of the handles. The connection of the faucet is shown in a detail view. or section view. Additional Drawing Views Alternate position views display overlays of two or more positions on the same view.Drawings Detail Views Detail views show a portion of an orthographic.
see Derived Drawing Views in the Help. as in the second example. edge. 83 .Drawings For more information about drawing views. as in the first example. Notes and Other Annotations Notes and Multi-Jog Leaders The alternate position view has a note with a degree symbol. In the exploded faucet view. or vertex) in the document. A note can be free floating. the note uses a multi-jog leader. or pointing to an item (face.
and balloons. unexploded. The surface finish symbol attached to the faucet handle specifies a circular finish and the maximum roughness of the surface. material removal. and rotation. The drawing also contains an isometric named view of the complete assembly. production method. You can insert multiple symbols and multiple copies of a symbol. a bill of materials. This drawing contains an exploded view of the vanity assembly. Some of the characteristics that you can specify for a surface finish symbol include type of symbol. Exploded Views Exploded views are versions of named views defined in configurations in the assembly document. Vanity Assembly Drawing Sheet This drawing sheet contains an exploded view. 84 . assembly. roughness. at the lower left.Drawings Surface Finish Symbols You can add surface finish symbols to part. or drawing documents. direction of lay. Here is the completed faucet assembly drawing sheet.
quantity. The item numbers reflect the sequence in which the model was assembled.Drawings Bill of Materials A bill of materials (BOM) is a table that lists the components of an assembly along with information needed in the manufacturing process. description. and weight. For more information. the BOM updates to reflect the changes. part number. The SolidWorks software populates the item number. You can also edit and save a custom BOM template. see Bill of Materials . material. 85 . You set the anchor point for the BOM in the drawing sheet format. and part number columns automatically. When you insert a BOM. vendor number. stock size. If the assembly or its components change.Overview in the Help. you have a choice of BOM templates with various columns for data such as item number. quantity.
Stacked balloons have one leader for a series of balloons. In the example. You can stack the balloons vertically or horizontally. The exploded vanity assembly includes balloons and stacked balloons for each component. You can set the style. and type of information for balloons. 86 . Here is the completed vanity assembly drawing sheet. The item numbers appear in the balloons automatically. see the Advanced Drawings tutorial. the balloons display the item number corresponding to the BOM in a circle. For a lesson on bills of materials and balloons. size.Drawings Balloons and Stacked Balloons You can insert balloons in assembly and drawing documents.
For more information on which tools are available with the different packages. and SolidWorks Premium. In the SolidWorks software. see the Product Matrix (http://www. not every customer wants the same handle style. you saw how configurations could be used to build two different lengths of the molding in one part file. you may want to create multiple configurations of the faucet handle. This chapter includes the following topics: • • • • • • • • • • • Building Multiple Configurations of Parts Updating Models Automatically Importing and Exporting Files Performing Stress Analysis Customizing SolidWorks Sharing Models Creating Photo-Realistic Images of Models Animating Assemblies Managing SolidWorks Files Accessing a Library of Standard Parts Examining and Editing Model Geometry Building Multiple Configurations of Parts Design tables let you build several configurations of a part by applying the values in the table to the dimensions of the part. SolidWorks Professional. The SolidWorks software is available in SolidWorks Standard.com/sw/mechanical-design-software-matrix. This design table shows the parameters used to create variations of the faucet handle: 87 . In Parts on page 36.5 Engineering Tasks The SolidWorks software contains several tools to help you complete engineering tasks such as creating variations of parts and importing files from legacy CAD systems to your SolidWorks models. The following example illustrates how design tables help organize several configurations. After all.htm). For example.solidworks. you can create different handle styles within one part file using a design table.
the configuration updates with the specified value. 88 .Engineering Tasks The first column lists the different configuration names. In addition to changing dimension values. Give a meaningful name for each configuration to reduce confusion in complex parts and assemblies and to help others who use the models. The final column shows the suppression state of a fillet feature. The values and suppression states define each configuration: Configuration name standard_handle Model view wide_handle tall_handle For a lesson on design tables. When you change a dimension value in a design table. you can also change the suppression state of a feature in design tables. The next four columns show the dimension names and values. see the Design Tables tutorial. These configuration names describe the type of handle generated from the design table. A feature can be suppressed (S) or unsuppressed (U).
your customer needs a longer faucet to accommodate a utility sink. and the associated assembly and drawing also update. any SolidWorks document that references that model also updates. Original faucet Revised faucet Revised assembly Revised drawing Loading the Latest Models You can refresh shared documents to load the latest version. You can modify the dimension of the faucet to make it any length. However. the associated assembly and drawing also change. For example.Engineering Tasks Updating Models Automatically When you change a model dimension. including any changes made by one of your colleagues. you designed the faucet to be 100mm in length for a vanity countertop. if you change the length of an extrude in a part. 89 . More specifically.
mates used in the original part are applied to the replacement part wherever possible. With the SolidWorks import and export functions. and a coworker just updated one of the assembly components. You can reload the revised component. Current subassembly New handle New subassembly When you replace a component.Engineering Tasks Suppose that you are working on a SolidWorks assembly document. For example. another engineer in your group designs a more cost-effective faucet handle. To ensure that the mates are preserved. Reloading is easier than closing and reopening the assembly with the revised part. allowing you more flexibility in the design process. consider that you are working on the faucet subassembly. without having to delete and replace each handle. Replacing Referenced Models You can replace a referenced document with another document from anywhere on a network. and the SolidWorks software automatically updates the assembly. see the Import/Export tutorial. Meanwhile. You can globally replace the current handles with the new ones. rename the corresponding edges and faces on a replacement part to match the edge and face names on the original part. Importing and Exporting Files You can import and export several different file formats to and from the SolidWorks software so you can share files amongst a broad user base. Consider that your company works with a vendor that uses another CAD system. For a lesson on importing and exporting files. you can share files between companies. 90 .
For example. see the SolidWorks SimulationXpress tutorial. For a lesson on SimulationXpress. you can edit the sketches to change the geometry of the features. you do not have to remodel the same part in the SolidWorks application. ® Performing Stress Analysis SolidWorks SimulationXpress provides an easy-to-use first pass stress analysis tool for SolidWorks parts. 91 . It also shows critical areas and safety levels at various regions in the faucet.Engineering Tasks Recognizing Features in Non-SolidWorks Parts FeatureWorks is an application that recognizes features on an imported solid body in a SolidWorks part document. For features that are based on sketches. SimulationXpress simulates the effect of the force and provides displacement and stress results. You can edit the definition of recognized features to change their parameters. you can examine the effects of a force applied to the faucet. Recognized features are treated the same as features that you create in the SolidWorks software. and you want to use them in the SolidWorks software. You can use the FeatureWorks software to recognize each feature as a SolidWorks feature. The FeatureWorks software is intended primarily for machined and sheet metal parts. Based on these results. you can strengthen unsafe regions and remove material from overdesigned areas. For a lesson on the FeatureWorks software. This way. Suppose you have legacy . see the FeatureWorks Overview tutorial.step files at your company. SimulationXpress helps you reduce cost and time-to-market by testing your designs on the computer instead of expensive and time-consuming field tests.
if you save your SolidWorks model as an eDrawings file. The API contains thousands ® functions that can be called from C#. if you work with a client in a remote location. you can customize the SolidWorks application to help reduce design time. For instance. With the API. You view eDrawings files with the eDrawings Viewer that you can download from the SolidWorks Web site for free. you can set the system options without setting each one individually.NET. C++. use the API to automatically set all of your options. Substantially smaller in size than the original files. eDrawings makes it practical to send files via email. you save time by programming the settings only once. With the API. This way.htm). ® 92 . you can perform batch operations. default templates. No additional CAD software is required. you can send a much smaller version of the file to your client. eDrawings files have the following features: Ultra Compact Files Built-in Viewer Send eDrawings files through email. You can embed the eDrawings Viewer when you email an eDrawings file. VB. For more information. For example. even over slow connections. However. assembly. and create your own PropertyManagers. Sharing Models SolidWorks eDrawings eliminates the communication barriers that designers and engineers deal with daily. then email these eDrawings files to others for instant viewing. View eDrawings files immediately. For lessons on the API.Engineering Tasks Customizing SolidWorks The SolidWorks Application Programming Interface (API) is an OLE programming interface to the SolidWorks software. these options include system colors. You can create eDrawings files from part. automatically populate drawing documents with model views or dimensions. and performance settings. or the API Support page on the SolidWorks Web site (www. you probably set system options to customize your working environment. see the API Help. Oftentimes. These functions provide you with direct access to SolidWorks functionality. see the SolidWorks API Tutorials. Anyone with a Windows-based or Macintosh computer can view eDrawings. or drawing documents.com/sw/support/apisupport. when you use any software application. In the SolidWorks software. you might need to send a model for their approval. Microsoft Access and Microsoft Excel ) or SolidWorks macro files. Instead. and of ® ® VBA (for example.solidworks. the file size is too big to send through email. or you can embed the eDrawings Viewer in the eDrawings file. For example.
text. Navigate through views automatically. Save SolidWorks configuration data and see the configurations in the eDrawings Viewer. Hyperlinking 3D Pointer Animation SolidWorks Simulation Data The optional eDrawings Professional version provides the following additional capabilities: Cross Sections Markup Measure Move Components SolidWorks Animator Output Configurations Exploded Views Create cross-section views with a variety of planes to fully examine a model. Display SolidWorks Simulation and SolidWorks SimulationXpress data. Move components in an assembly or drawing file. The 3D Pointer helps orient you when you check features in multiple views. assembly. and drawing documents. View animations created with SolidWorks Animator and observe in real time how moving parts interact as true solids. Measure the distance between entities or measure dimensions in part. The following features help you overcome common barriers for effective 2D drawing communication: Layouts Open individual views in a drawing and arrange them in any way you desire. Layouts enable the eDrawings recipient to print and export any subset of a drawing. Click the view annotation. The markup elements are inserted as comments in the file. and the section view or detail is immediately added to your layout. when available. Save SolidWorks exploded view information and see the exploded views in the eDrawings Viewer. Identify and match geometry in multiple views. eliminating searches for views or details. ® Cross-section view of the vanity with dimensions and comments 93 .Engineering Tasks eDrawings files are also significantly easier to understand than standard 2D drawings. or geometric elements. Create animation sequences of eDrawings views. in eDrawings part or assembly files. regardless of how the views were arranged in the original drawing. Mark up files using clouds.
Engineering Tasks For a lesson on the eDrawings software. you specify model appearances.avi files. see the SolidWorks eDrawings tutorial. You can create rotated animations. Animation helps your customers visualize models in a real-world situation. you can create . You can also import assembly motion from other types of motion studies. By incorporating Appearances and RealView Graphics. Examples of models rendered in PhotoView 360: For more information on PhotoView 360. or faucet handles move. see the Animation tutorial. your customers can see a vanity door open and close.avi files that animate your products. and lighting. In the SolidWorks software. For a lesson on animated motion studies. 94 . exploded view animations. To stand out from the competition. Creating Photo-Realistic Images of Models PhotoView 360 lets you create photo-realistic rendered images directly from SolidWorks models. or collapsed view animations. Then use PhotoView 360 to render the model. you can produce photo-realistic animations. Suppose that your company is at a convention with competing companies. see Rendering with PhotoView 360 in the Help. This way. Animating Assemblies You can create animated motion studies to capture the motion of SolidWorks assemblies in . scenes.
This way. in a tree structure. Therefore. You have the option to find and update references to documents.sldprt to countertop_with_sink.sldprt (such as the vanity assembly) does not recognize that the part name changed. when you attach the hinge to the vanity cabinet or when you fasten the waste pipe to the sink. SolidWorks Toolbox has several engineering tools: 95 . then drag the component into your assembly. and JIS. DIN. according to the active function. consider that you want to rename the countertop part from countertop. you do not have to make additional parts to complete the vanity assembly. and it does not appear in the assembly.sldprt. • Copy. Select the standard and the type of part you want to insert. or replace referenced documents. then edit them as needed. SolidWorks Explorer lets you: • View document dependencies for drawings. SolidWorks Explorer The SolidWorks software recognizes that you renamed the part. For example. Any document that references the part updates accordingly with the new name. Accessing a Library of Standard Parts SolidWorks Toolbox includes a library of standard parts that are integrated with the SolidWorks software. For example. parts. replacing. BSI. the SolidWorks software cannot find the renamed part. Additionally. You can customize the SolidWorks Toolbox library of parts to include your company's standards or to include those parts that you refer to most frequently. you can use standard screws and washers included in SolidWorks Toolbox. • View data and previews or input data.Engineering Tasks Managing SolidWorks Files SolidWorks Explorer is a file management tool designed to help you accomplish tasks such as renaming. rename. and assemblies. ISO. If you rename the part in: Windows Explorer Any SolidWorks document that references countertop. CISC. and copying SolidWorks documents. Solidworks Toolbox supports several international standards including ANSI. You can also make a copy of SolidWorks Toolbox parts.
You can extrude the sketch in the SolidWorks software to create the beam. Creates industry standard O-ring and retaining ring grooves to your cylindrical model. Then. see the Toolbox tutorial. Examining and Editing Model Geometry SolidWorks Utilities is a set of tools that lets you examine and edit individual parts. The cam can be either circular or linear with 14 motion types from which to choose.Engineering Tasks Beam Performs deflection and stress Calculator calculations on structural steel cross sections. Bearing Performs bearing calculations to Calculator determine capacity ratings and basic life values. and compare the features and solid geometry of pairs of parts. For a lesson on SolidWorks Toolbox. Cams Creates cams with fully-defined motion paths and follower types. you can use the Compare Features utility to compare the parts. This utility identifies the unique features of each part so you can collaborate and decide on the best design methods. if you and a coworker design two similar types of faucet handles. Grooves Structural Brings the cross-section sketch of a structural steel beam into a part. either as a blind cut or a cut through the entire cam. The Steel sketch is fully-dimensioned to match industry standard sizes. you can identify the most efficient designs and combine them in one model. You can also set how the track for the follower is cut. SolidWorks Utilities includes the following tools: 96 . For example.
loops.Engineering Tasks Compare • Compare Documents. Compare Features. Compares bill of material (BOM) tables from two SolidWorks assembly or drawing documents. feature type. assembly. Power Select Report Manager Simplify Symmetry Check Thickness Analysis For a lesson on SolidWorks Utilities. this utility identifies differences in file and document properties. feature name. For example. Finds a set of features in a part that satisfies specified parameter conditions so you can edit them in batch mode. Symmetry Check. Creates simplified configurations of a part or assembly for analysis. face color. Feature Paint Find and Replace Annotations Find/Modify Geometry Analysis Copies feature parameters (such as depth and size) from one feature to others that you select. 97 . Compares the properties of two SolidWorks documents (including two configurations of the same model). • Compare Features. and unique features. Compares two parts to find their geometric differences. It also computes the common volume of the two parts (or assemblies) and the volume of material added and removed. modified. and Thickness Analysis utilities. and failed rows. small faces. and surface type. feature color. Manages reports generated from the Geometry Analysis. Compares features of two parts and finds identical. You can compare two documents of the same or different types. • Compare BOMs. Checks parts for geometrically symmetric faces. faces. Selects all the entities (edges. You can specify criteria for edge convexity. This utility identifies unique and modified faces in both parts. Compare Documents. Determines thin and thick regions of a part. Finds and replaces text in a variety of annotations for part. • Compare Geometry. short edges. edge angle. and discontinuous edges and faces. see the SolidWorks Utilities tutorial. Compare Geometry. knife (sharp) edges and vertices. extra columns and rows. It also determines the thickness of a part within a specified range of values. This utility identifies the following categories of geometric entities: sliver faces. Identifies geometric entities in a part that could cause a problem in other applications such as finite element modeling or computer-aided machining. and drawing documents. The results list missing columns and rows. Compare BOMs. or features) in a part that meet the criteria that you define.
A Step-by-Step Lesson This chapter includes the following topics: • • • • • Getting Ready for the Lesson Creating a Box Creating a Lid for the Box Putting the Box and Lid Together Creating a Drawing Getting Ready for the Lesson Before you begin this lesson. which means that menu items are grayed out if the tools are not available for your current task. see Menus in the Help. Many of the tools you use are accessible in three ways: • Menus • Toolbars • CommandManager These tools are context sensitive. it is helpful to know how to access the SolidWorks software's tools. and the CommandManager. toolbars. The following table lists the tools you use in the lesson and their locations on menus. so it is helpful to know which toolbar you use to access them. the tools do not appear at all. 98 . Sometimes. For more information.
99 .Tool New Save Options Sketch Smart Dimension Rectangle Icon Menu File > New File > Save Tools > Options Insert > Sketch Tools > Dimensions > Smart Toolbar Standard Standard Standard Sketch Sketch CommandManager Menu Bar Menu Bar Menu Bar Sketch Sketch Tools > Sketch Sketch Entities > Rectangle Insert > Boss/Base > Extrude Insert > Features > Shell Features Sketch Extruded Boss/Base Shell Features Features Features Insert Components Insert > Assembly Component > Existing Part/Assembly Insert > Mate Assembly Assembly Mate Assembly Creating a Box The first part you create is a box.
second. select MMGS to set the unit of measurement to millimeter. it becomes a 3D model. In Overall drafting standard. select ISO. you open a new part document where you will build a model. Later. when you extrude the sketch. 2. In the New SolidWorks Document dialog box. A new part document opens. On the left pane. • The PropertyManager opens at the left and prompts you to select a plane on which to sketch the rectangle. Top. Click Options In the System Options . 6. (Sketch toolbar) or Tools > Sketch Entities > • The software enters sketch mode. Under Unit system. Setting the Drafting Standard and Units Before you begin modeling. 3. 1. In this procedure. click Units. 1. Click Corner Rectangle Rectangle.Opening a New Part A part is the basic building block in the SolidWorks software. The sketch is in 2D. 4. 5. 2. 1. (Standard Toolbar) or Tools > Options. 100 . select the Document Properties tab. Click New (Standard toolbar) or File > New. click Part and click OK. • The Front. Sketching a Rectangle You use a sketch to construct the basic outline of the part. Click OK. and Right planes are visible.General dialog box. you set the drafting standard and unit of measurement for the part. gram.
press the spacebar. You may see four symbols: . It does not matter what size you make the rectangle. 101 . To see the rectangle normal to (straight on). which makes the rectangle appear skewed. they indicate where lines are vertical and horizontal . click. 2. 4. Click the Front plane. 3.• The pointer changes to to indicate that you can select a plane. These symbols are called sketch relations. In the Orientation dialog box. The pointer changes to to indicate that you can now draw the rectangle. then drag the pointer to create a rectangle. Click to complete the rectangle. you can dimension it later. Starting anywhere. The current view is isometric. double-click Normal To. In the rectangular sketch.
Instead of exiting sketch mode, you keep the sketch open so you can dimension the rectangle in the next set of steps.
Dimensioning the Sketch
Now that you have a sketched rectangle, you need to dimension it by adding measurements. You can use the Smart Dimension tool to dimension the rectangle. If you had exited sketch mode in the previous procedure, you would have to re-enter sketch mode to dimension the sketch. 1. Click Smart Dimension (Dimensions/Relations toolbar) or Tools > Dimensions > Smart. The pointer changes to .
2. Select the top horizontal line in the rectangle. A dimension appears. 3. Drag the dimension up and click to place it. 4. In the Modify dialog box, type 100 and click .
5. Repeat steps 2 through 4 for the right vertical line in the rectangle.
6. In the upper right corner of the window in the Confirmation Corner, click the sketch icon exit sketch mode.
Extruding the Sketch
After dimensioning the 2D sketch, you can extrude it to make a 3D solid model.
1. Click Extruded Boss/Base
(Features toolbar) or Insert > Boss/Base > Extrude.
• If the sketch is selected, the Boss-Extrude PropertyManager appears and a preview of the extrude appears. • If the sketch is not selected, the Extrude PropertyManager appears and indicates that you need to select a sketch. 2. If the Extrude PropertyManager appears, select the sketch by clicking any line in the square. Otherwise, go to the next step. A preview of the extrude appears.
3. In the PropertyManager: a) Set Depth to 100.
b) Click . The 2D sketch changes to a 3D model.
Creating a Hollow Model
In this procedure, you use the Shell tool to create a hollow box. 1. Click Shell (Features toolbar) or Insert > Features > Shell. 2. In the Shell PropertyManager, under Parameters, set Thickness to 5.
3. In the graphics area, select the face as shown:
Face<1> appears in the PropertyManager under Faces to Remove 4. Click . The box is hollow with walls that are 5mm thick.
The box is complete.
Saving the Part
1. Click Save (Standard toolbar) or File > Save. 2. In the Save As dialog box: a) Browse to the location where you want to save the document. b) For File name, type box. c) Click Save. The part is saved as box.sldprt. 3. Keep the part open.
Creating a Lid for the Box
You created the first part, a box. Now you need to create a second part to make a lid for the box.
2. Click New (Standard toolbar) or File > New. select the Document Properties tab. 4. click Part and click OK. click Units. Click Corner Rectangle Rectangle. 3. (Sketch toolbar) or Tools > Sketch Entities > 1. Click the Front plane. Setting the Drafting Standard and Units Before you begin modeling. select ISO. In this procedure. In the New SolidWorks Document dialog box. select MMGS to set the unit of measurement to millimeter. you set the drafting standard and unit of measurement for the part. Under Unit system. A new part document opens. second. gram. Sketching a Rectangle The lid for the box is shaped like a square. Click Options In the System Options . In Overall drafting standard. 5. then drag the pointer to create a rectangle. you sketch a rectangle.General dialog box. 6. Later you can dimension it to fit the box. 3. 1. 105 . Click OK.Opening a New Part 1. Click. 2. On the left pane. (Standard Toolbar) or Tools > Options. The PropertyManager prompts you to select a plane on which to sketch the rectangle. 2.
Select the top horizontal line in the rectangle. 4. Click to complete the rectangle. you need to dimension it so it has the proper measurements. Dimensioning the Sketch Now that you have a sketched rectangle. In the Modify dialog box. type 100 and click . Click Smart Dimension (Dimensions/Relations toolbar) or Tools > Dimensions > Smart. 3. 5. 106 . The pointer changes to 2. 1.4. Drag the dimension upwards and click to place it. Repeat steps 2 through 4 for the right vertical line in the rectangle. A dimension appears.
The 2D sketch changes to a 3D model. In the upper right corner of the window in the Confirmation Corner. 107 . Extruding the Sketch After dimensioning the 2D sketch. (Features toolbar) or Insert > Boss/Base > Extrude. Sketch mode is turned off. 3. click the handle (arrow) and drag it until you reach 10 on the scale. If the Extrude PropertyManager appears. 2. • If the sketch is not selected. A preview of the extrude appears. the Extrude PropertyManager appears and indicates that you need to select a sketch. 1. the following occurs: • If the sketch is selected. then click in the PropertyManager. you can extrude it to make a 3D solid model. Otherwise. go to the next step. select the sketch by clicking any line in the square. In the graphics area. Click Extruded Boss/Base Depending on what is selected in the graphics area. the Boss-Extrude PropertyManager appears and a preview of the extrude appears.6. click the sketch icon .
1. In the Orientation dialog box. select the face as shown: 108 . Press the spacebar or click View > Modify > Orientation. 3. you create a lip on the cover using another extrude. The cover is rotated so the front is visible. Click Corner Rectangle (Sketch toolbar) or Tools > Sketch Entities > Rectangle. double-click *Front. 2. 4. In the graphics area.Creating a Lip on the Cover To ensure that the cover fits tightly on the box.
A dimension appears. 1. Click Smart Dimension (Dimensions/Relations toolbar) or Tools > Dimensions > Smart. 109 . Dimensioning the Sketch You need to dimension the rectangle so it has the proper measurements. In the graphics area: a) Select the top horizontal line in the rectangle. It does not matter what size you make the rectangle.5. b) Select the top edge of the extrude. Sketch a rectangle on the face. The pointer changes to . you can dimension it later. 2.
1. 2. Repeat steps 2 through 4 for the rest of the sketch: 6. Sketch mode is turned off. you can extrude it to make a lip for the lid. In the Orientation dialog box. 4. Extruding the Sketch After dimensioning the 2D sketch. In the upper right corner of the window in the Confirmation Corner. double-click *Isometric. Drag the dimension upwards and click to place it.3. 110 . click the sketch icon . In the Modify dialog box. type 2 and click . Press the spacebar or click View > Modify > Orientation. The cover is rotated. 5.
The 2D sketch changes to 3D. click the handle (arrow) and drag it until you reach 5 on the scale. 111 . select the sketch by clicking any line in the square. 4.3. In the graphics area. Click Extruded Boss/Base (Features toolbar) or Insert > Boss/Base > Extrude. then click in the PropertyManager. 5. In the graphics area.
c) Click Save. 2. type lid.sldprt. A new assembly document opens. Click Save 2. 1. Click New (Standard toolbar) or File > New. The part documents become "components" in the assembly. b) For File name. Opening a New Assembly In this procedure. In the Save As dialog box: a) Browse to the location where you want to save the document. In the New SolidWorks Document dialog box. you open a new assembly document where you will insert the box and lid models. click Assembly and click OK. in this case. 1.The lid is complete. the box and lid. 112 . 3. Putting the Box and Lid Together An assembly is a collection of part documents. The part is saved as lid. Keep the part open. and the Begin Assembly PropertyManager appears. Saving the Part (Standard toolbar) or File > Save.
under Part/Assembly to Insert. It is OK if the parts overlap. 3. click to place the part in the assembly.Inserting Parts into the Assembly An assembly is a collection of parts. . In the Begin Assembly PropertyManager. where they become components in the assembly. The part appears in the graphics area. select box. click to place the part in the assembly. 5. you insert the box and lid into the assembly. 113 . In this procedure. The part moves to the center of the graphics area. In the graphics area. 1. select lid. In the Insert Component PropertyManager. under Part/Assembly to Insert. In the graphics area. The part appears in the graphics area and the pointer changes to 2. Click Insert Components (Assembly toolbar) or Insert > Component > Existing Part/Assembly. 4.
you may want to move them so they do not overlap. you are warned that the component is fixed and cannot be moved. 1. Click the Move Component Component arrow (Assembly toolbar) and click Rotate or click Tools > Component > Rotate. it is easier for you to select faces during the mate process. the first part in an assembly is fixed in position. 1. Rotating a Component To align the components before you mate them. .Moving a Component When you insert components into an assembly. 3. If you try to drag the box component. it is easier to select them when you mate the components. The Rotate Component PropertyManager appears and the pointer changes to 114 . Click . Click Move Component (Assembly toolbar) or Tools > Component > Move. By default. . The Move Component PropertyManager appears and the pointer changes to 2. By aligning the components. By moving the components. you can rotate them so they are in the proper orientation. Drag the lid component to the right of the box.
Click The assembly appears as shown: Mating the Components Mates create geometric relationships between components. The lip should be in the back. The Mate PropertyManager appears. Before rotating After rotating . 3. Click the lid and rotate it approximately as shown.2. As you add mates. you define the allowable movement of the components. Click Mate (Assembly toolbar) or Insert > Mate. 1. 115 .
• In the PropertyManager. 116 . Coincident • The Mate pop-up toolbar appears with Coincident selected. In this case. Click Zoom In/Out (Heads-up View toolbar) or View > Modify > Zoom In/Out to help you select the faces if necessary. the software makes the faces coincident. Before mating After mating 3. under Standard Mates. Click . but the PropertyManager remains open so you can add more mates. is selected. Select the highlighted faces on each component.2. The mate is applied. When you select the second face: • The most logical mate is applied to the faces.
sldprt: Front face of box. Select the highlighted faces on each component.4. Click . Select the highlighted faces on each component: A coincident mate is applied to the faces. and the lid fits into the box.sldprt Back face of lip on lid. Use Rotate View by clicking View > Modify > Rotate to help you select the back face of the lip on lid. 6. Before mating After mating 5.sldprt A coincident mate is applied to the faces. 117 .
In the dialog box: a) Browse to the location where you want to save the document. In the list. A new drawing document opens. Opening a New Drawing 1. Keep the assembly open. 118 . Saving the Assembly 1. select A3 (ISO) and click OK. Creating a Drawing You can create 2D drawings of the 3D solid parts and assemblies you design. 2. and drawings are linked documents. The assembly is saved as box_with_lid. Parts. type box_with_lid. In the New SolidWorks Document dialog box. c) Click Save. Click Save (Standard toolbar) or File > Save. Click New (Standard toolbar) or File > New. b) For File name. click Drawing and click OK. 3. assemblies. Click twice. any changes that you make to the part or assembly change the drawing document. 3.sldasm.7. The Sheet Format/Size dialog box appears where you can set the drawing sheet parameters. 2.
119 . Click Standard 3 View 3 View.sldprt appear in the drawing. select the Document Properties tab. In the dialog box. 3.4. second. Setting the Drafting Standard and Units Before you begin the drawing. 2. In the Standard 3 View PropertyManager.Drafting Standard dialog box. Inserting Standard 3 Views The Standard 3 View tool creates three related orthographic views of a part or assembly. click Units. and left orientations.Units dialog box. The standard 3 views of box. In the Document Properties . On the left pane. If the Model View PropertyManager appears. under Unit system. 6. click to close it. Click OK. 2. select MMGS to set the unit of measurement to millimeter. Click Options (Standard Toolbar) or Tools > Options. under Part/Assembly to Insert. select box. (Drawing toolbar) or Insert > Drawing View > Standard 1. select ISO. In the Document Properties . in Overall drafting standard. you set the drafting standard and unit of measurement for the document. top. Click . gram. The views use the front. 3. 4. 5. 1.
click in the lower right corner of the sheet to place the drawing view. 120 . In the Model View PropertyManager. 2. Click Smart Dimension (Dimensions/Relations toolbar). click Shaded With Edges 5. 1. (Drawing toolbar) or Insert > Drawing View > Model. or Tools > Dimensions > Smart. Click Model View 2. 1. click *Isometric . 3. . you can choose the view orientation that you want to display. . you insert an isometric model view of the assembly. 4. under Part/Assembly to Insert. Click The drawing view is attached to the pointer. Dimensioning the Drawing In this procedure. In this procedure. but do not place it yet. In the PropertyManager: a) Under Orientation. Click . you use autodimensioning to add dimensions to a drawing view. 6. select box_with_lid. b) Under Display Style. In the Dimension PropertyManager: a) Select the Autodimension tab. In the graphics area.Inserting an Isometric Model View When you insert a model view.
c) Under Horizontal Dimensions. select Above view. The drawing view is dimensioned. the leftmost vertical edge turns pink and the bottom edge turns purple. in the front view. click . Drag a dimension to move it. d) Under Vertical Dimensions. These colors correspond to the colors in the PropertyManager under Horizontal Dimensions and Vertical Dimensions: 4. In the PropertyManager. click in the space between the drawing view border (dotted line) and the drawing view as shown: In the drawing view. select Left of view. In the graphics area.b) Under Entities to Dimension. The drawing appears as: 121 . 3. click Selected entities.
122 .
and drawing. you can access the finished parts. Washer. This chapter includes the following topics: • • Covered Can Bolt. However. Create the parts. 123 . lid. and drawing using the given information. and drawings at install_dir\samples\introsw. assembly. and Nut Covered Can This exercise helps you to use basic tools and concepts by creating a can.B Exercises There are no step-by-step procedures for these exercises. assemblies.
Can: R5 is the fillet radius. Lid: Assembly: 124 .
Create the parts. 125 .Drawing: • Two model views of the lid • One model view of the cylinder Bolt. and drawing using the given information. nut. and drawing. and Nut This exercise helps you to use basic tools and concepts by creating a bolt. washer. assembly. Washer.
Bolt: Washer: Nut: 126 .
Assembly: Drawing: 127 .
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