kicad-developers team mailing list archive

[Tomasz Wlostowski <tomasz.wlostowski@xxxxxxx>]

On 04/26/2013 04:08 PM, Simon Huwyler wrote:
> One more thing: I agree that the additional numbers may confuse a bit.
> So, why not just insert a check box named: "Use layer based constraints"?

Hi Simon,

I agree that such constraints are very useful, I use them frequently in 
Altium, but this is only a small piece of the whole DRC machinery that 
needs to be rewritten. A makeshift patch to the current DRC code will 
only make it more difficult to fix properly in the future, for instance 
by keeping these extra rules hardcoded in PCB files (that any newer 
release will have to parse to keep compatibility).

For example, what about area-bound clearance/width constraints (i.e. 
different clearance values for different parts of the PCB?). Why not 
just insert another checkbox named "Use area based constraints" next to 
yours and store a few more parameters in the .kicad_pcb file? Then 
someone else comes up with yet another specialized constraint, and we'll 
end up with bloated GUI and mess in code.

What about simply letting users specify a set of boolean expressions 
that return the clearance for a pair of objects to be checked. For example:

1. both.GetLayer() in ['Top', 'Bottom']: 10 mil
2. not both.GetLayer() in ['Top', 'Bottom']: 14 mil
3. first.InArea ('My area'): 20 mil else: 10 mil
4. any.InComponent ('Some BGA that needs smaller clearance'): 5 mil
5. default: 10 mil

.... and so on, and so forth, for any DRC check.

These can be python expressions, evaluated through the scripting engine 
for each item before starting the DRC.

The advantages are:
- no need to change DRC's C++ code and/or GUI whenever somebody requests 
a fancy constraint configuration
- rule expressions can be stored in .kicad_pcb files without risk of 
being deprecated (unless somebody changes the API of the scripting engine).
- P&S must follow design rules as well. I would prefer get the clearance 
value for any pair of objects directly via scripting engine  instead of 
parsing and analyzing all specialized constraints again in P&S code.
- automatic trace impedance calculation via python expressions:

both.IsDiffPair() && both.GetLayer() == 'Top'  : 
DifferentialMicrostrip(first, second).Gap

Regards,
Tom