I am trying to PCB using a schematic I made
As you have said PCB designing is not your strong point, so let's give you some pointers:

Here are some general guidelines of PCB design in no specific order:


Know your mechanical constraints. These can be anything from board dimensions, connector position, height limitations, and mounting holes, yes, don't forget those, if unsure, always add 3mm holes 5mm from each edge at each corner.
Try to keep all polarised components facing the same direction. For example all the cathodes of the diodes pointing towards the top edge of the board. This makes assembly easier and reduces mistakes. The advice is valid for ICs as well. It makes the board aesthetically more pleasing. Please note that if the layout gets too complicated or puts the signal integrity at risk, then you can ignore this rule. 
Avoid via holes as much as possible. Vias can be the weakpoint in a design, especially if you are etching the boards yourself. If you cannot avoid them, try to make them exposed so that they can be worked on if needed.
Make tracks as wide as you can, giving priority to the power supplies. As a general rule, calculate that a track 1mm wide can tollerate 2 Amps increasing in temperature by roughly 25 degrees Celsius. Keep that as a rule of thumb, but always exceed this for currents above 500mA. I don't know what the currents involved on your board are, but as a rough estimate I would suggest 1mm for the signal traces and 3mm for the powers. I know that they are oversized, but they are also much more forgiving.
Avoid passing tracks between the pins of an IC. Components can be moved, for example in your layout, just moving R7 and R8 between IC2 and IC3, will take away that nasty  track under IC3
Make the placement first, the routing later. If the ratsnet looks good, the layout will be easy. Spending time on carefully placing the components will save you a lot of time on the layout
Try to align the components so that they are spaced equally and aligned. If a board looks good, it is more likely to work. (it shows that you have taken the time required)
The tracks should be always routed at 90 degrees to each other, with only bends routed at 45 degrees. Intersections must be at 90 degrees, and make routes as short as possible, unless there is a good reason.
keep your clearances to other tracks, but most importantly to the pads. If a board like this, the minimum clearance should not be less than 1mm. IF you have the space, keeps as far as you can from pads.
If you intend to solder wires directly to the board, make sure that the holes are big enough for the wire to go through, and I recommend that you over size the pads, so that you have more mechanical strength. As a rule of thumb, these kind of pads, should be 3 times the diameter of the hole where the wire comes through.
Don't forget to tidy up the layout. Once you have finished the routing you are only half way there.


Spending 5 minutes in MS paint you can see how much more compact the board can be without pushing the boundaries. 


Don't forget to put some copper under the bodies of those TO220, so that they can dissipate a little bit more heat.

I will not go into the merits of your schematic, as you have already stated that the board works flawlessly.