Unlike other EDA software tools, which have one type of library that contains both the schematic symbol and the footprint variations, kicad .lib files contain schematic symbols and .mod files contain footprints, or modules. Cvpcb is used to successfully map footprints to symbols.
As for .lib files, .mod library files are text files that can contain anything from one to several parts.
There is an extensive footprint library with kicad, however on occasion you might find that the footprint you need is not in the kicad library. Here are the steps for creating a new PCB footprint in kicad:
- From the kicad project manager start the PCBnew tool. Click on the 'Open Module Editor' icon on the top toolbar. This will open the 'Module Editor'.
- We are going to save the new footprint in the footprint library 'connect'. Click on the 'Select working library' icon on the top toolbar. Select the 'connect' library, though you can choose a different location if you want.
- Click on the 'New Module' icon on the top toolbar. Type 'MYCONN3' as the 'module reference'. In the middle of the screen the 'MYCONN3' label will appear. Under the label you can can see the 'VAL*' label. Right click on 'MYCONN3' and move it above 'VAL'. Right click on 'VAL*', select 'Edit Text Mod' and rename it to 'SMD'. Set the 'Display' value to 'Invisible'.
- Select the 'Add Pads' icon on the right toolbar. Click on the working sheet to place the pad. Right click on the new pad and click 'Edit Pad'. You can otherwise use the e key shortcut.
- Set the 'Pad Num' to '1', 'Pad Shape' to 'Rect', 'Pad Type' to 'SMD', 'Shape Size X' to '0.4', and 'Shape Size Y' to '0.8'. Click OK. Click on 'Add Pads' again and place two more pads.
- If you want to change the grid size, Right click → Grid Select. Be sure to select the appropriate grid size before laying down the components.
- Considering, for instance, that a 0.8mm BGA component has a pin to pin distance of about 30 mil (0.8mm), it is generally commendable to set a grid size of 5 mil when you route.
- Move the 'MYCONN3' label and the 'SMD' label out of the way so that it looks like the image shown above.
- When placing pads it is often necessary to measure relative distances. Place the cursor where you want the relative coordinate point (0,0) to be and press the space bar. While moving the cursor around, you will see a relative indication of the position of the cursor at the bottom of the page. Press the space bar at any time to set the new origin.
- Now add a footprint contour. Click on the 'Add graphic line or polygon' button in the right toolbar. Draw an outline of the connector around the component.
- Click on the 'Save Module in working directory' icon on the top toolbar, using the default name MYCONN3.