extract technical drawing from pdf into altium
I solved this problem using inkscape with the following procedure.


Import the pdf page into inkscape.
Use object-ungroup and path->split path to break the diagram down into individual lines (Otherwise totally unrelated lines can be part of the same path)
Copy and paste the diagram of interest into a new inkscape document.
Use the toolbar to measure the locations in mm of two objects (e.g. the pick lines of a dimension marker) that will establish the scale and subtract to find the distance between them.
Calculate the scale factor needed to convert the diagram to 1:1 scale by dividing the expected distance between the objects by the distance measured on the diagram. Multiply this scale factor by 100 to convert it to a percentage.
Select the whole diagram, set the toolbar units to percent and turn on the aspect ratio lock.
Enter your percentage scale factor using the toolbar and press enter to rescale.
Save the file from inkscape as a dxf with mm units.
Use file-import to import the dxf into your Altium PCB, again remember to set the units to mm. Also it's a good idea to set a reasonable line width, the default is unreasonablly small and will make the lines difficult to select.
Finally use edit-move selection by x,y to move the imported diagram into the correct place on the PCB.