[sdiy] KiCad, was Re: RS Designspark PCB tool

[Veronica Merryfield]

On 2012-06-22, at 5:09 AM, Harry Bissell wrote:

> So far I'm finding KiKad slow but not ~too~ painful

It gets much quicker on the second full board. I've lost count of how many I have done with it now. 

Placing mounting holes is best done by creating a schematic pad first. I call mine 'pad' - a single pin part that has a connection with no line to the pin and no package, so it shows as a pad in the schematic. I use M as the designator, as in mount. Some get connected but most don't. I have a number of different sized mounting pad parts in my module library now and usually pick one to suit the project. 

Some PCB stuffers want optical marks on the board and I have a few of those now as well. Usually they are circles of copper only. 

It is worth maintaining your own parts and module library in a separate directory from the install. This ensures your libraries exist across an upgrade. When I ship the files to a client, I tell them which version of the tools I used and I export the library parts and modules that aren't in the install. Way back I picked up up a project from someone else who did not export their custom parts and I had to recreate them - I think that was an OrCad project. The practise learnt then has stuck. However, with KiCad, if you get a project with the custom stuff missing, a little hunting with a text editor can dig it out of the project files and the libraries can be recreated with a text editor.

It is worth taking a look at the files with a text editor and get to know them. I have done a number of larger pin parts with a text editor. Create the first pin in the app, then use a text editor to do the rest of the pins. Go back to the app to check and tidy up. 

Vias have to get placed as part of laying down traces but you can delete the trace later and leave the vias. The only time I have needed to do this is to place vias to connect flood fill areas. The vias need to be laid with traces to give the vias a net to be part of then they will get connected with the flood fill of the same net.

There are some great people of the KiCad mailing lists and worth lurking on the developers list to see what is being planned etc.