Frequently Asked Questions
How can I create a pad shape that isn't provided by the application?
[ General / Libraries ]
Some components require pads with strange shapes that don't match any of the inbuilt shapes provided by the application but the range of available shapes is quite comprehensive so it's worth checking whether any would be suitable by creating or editing a pad style under design technology..
If no standard pad is suitable, you can add the shapes required for these pads by adding copper in the PCB symbol.
You will still need to start with a 'real' pad in the symbol, so you should first add a pad using one of the provided shapes. Then you can 'extend' the shape of the pad by drawing shape(s) on the appropriate layer(s) (top and/or bottom copper, not forgetting the solder and/or paste mask layers if you need them). Resist shapes can be created most easily by copying the relevant shape to the resist layer then increasing the line width by twice the edge clearance required (which also adds an appropriate radius on corners). Unfortunately this rarely works for paste as negative line widths aren't possible!
Before finishing with the symbol, you also need to mark each of the electrical (copper) shapes to specify to which pad they belong. This is done using the Pad Number field on the Properties dialog for the shape. If you don't do this, you will find that Design Rule Check flags an error between your pad and the copper because it doesn't know they are supposed to be treated as part of the same item.
Once a shape is linked to a pad, you can also enable the Auto Mask checkbox to tell the application to treat the shapes as part of the pad when generating paste and resist masks automatically from the electrical layer.