kicad-developers team mailing list archive

[Jeff Young <jeff@xxxxxxxxx>]

Here’s a really dumb test file just so you can get an idea of what it looks like:

(version 1)
(selector (match_netclass "Default") (rule "Big Gap"))
(selector (match_type track) (rule "Big Gap"))
(rule "Big Gap" (clearance 1.5))
(selector (match_type blind_via) (rule "Big Hole"))
(rule "Big Hole" (hole 2))
(rule "Small Edge" (clearance 2))
(rule "Big Edge" (clearance 3))
(selector (match_type board_edge) (rule "Small Edge"))
(selector (match_layer "In1.Cu") (match_type board_edge) (rule "Big Edge") (priority 2))


> On 16 May 2020, at 16:43, Jeff Young <jeff@xxxxxxxxx> wrote:
> 
> I’ve just merged a possible implementation of the DRC rules.  I’d like to get some feedback on it, and also some testing.  (Because the rules support such a wide range of possibilities it’s going to need a good deal of testing.)
> 
> For now, it picks up DRC rules from a file named “drc-rules” in the project directory.
> 
> There’s no GUI editor at present: use a text editor.
> 
> Grammar is s-expr.  It generally follows the ideas set down here:
> 
> https://docs.google.com/document/d/1qvCH9aHwCzp5qtKTna4jJXuloNU0b96gAxAHSKPuXpU <https://docs.google.com/document/d/1qvCH9aHwCzp5qtKTna4jJXuloNU0b96gAxAHSKPuXpU>
> 
> with one major exception: I found the select-a-single-rule didn’t pan out.  You have to duplicate too much stuff in each rule for that.
> 
> Also, because the DRC engine (and zone filler) don’t currently support min/opt/max the prototype implements min with Seth’s “relaxed” option.
> 
> Top level is a list; first expression must be (version x) followed by any number of (selector…) and (rule…) expressions.
> /*
>  * Match tokens:
>  *     match_netclass
>  *     match_type
>  *     match_layer
>  *     match_all
>  *     match_area  (not yet implemented with the exception of “$board”, which matches everything)
>  *
>  *     (selector (match_area "$board") (rule "OSHParkClass3") (priority 100))
>  *
>  *     (selector (match_netclass "HV") (rule "HV_internal"))
>  *     (selector (match_netclass "HV") (match_layer "F_Cu") (rule "HV_external"))
>  *     (selector (match_netclass "HV") (match_layer "B_Cu") (rule "HV_external"))
>  *
>  *     (selector (match_netclass "HV") (match_netclass "HV") (rule "HV2HV"))
>  *     (selector (match_netclass "HV") (match_netclass "HV") (match_layer "F_Cu") (rule "HV2HV_external"))
>  *     (selector (match_netclass "HV") (match_netclass "HV") (match_layer "B_Cu") (rule "HV2HV_external"))
>  *
>  *   TODO: pads for connector pins or wire pads have even larger required creepage clearances.  How to encode?
>  *   User attributes on parent footprint?
>  *
>  *     (selector (match_netclass "HV") (match_type "pad") (match_netclass "HV") (match_type "pad") (rule "pad2PadHV"))
>  *
>  *     (selector (match_netclass "signal") (match_area "BGA") (rule "neckdown"))
>  *
>  * Type tokens:
>  *     track
>  *     via
>  *     micro_via
>  *     blind_via
>  *     pad
>  *     zone
>  *     text
>  *     graphic
>  *     board_edge
>  *     hole
>  *     npth
>  *     pth
>  *
>  * Rule tokens:
>  *     allow  (not yet implemented)
>  *     clearance
>  *     annulus_width
>  *     track_width
>  *     hole
>  *
>  * Rule modifiers:
>  *     relaxed
>  *
>  *     (rule "HV" (clearance 200) (priority 200))
>  *     (rule "HV_external" (clearance 400) (priority 200))
>  *     (rule "HV2HV" (clearance 200) (priority 200))
>  *     (rule "HV2HV_external" (clearance 500) (priority 200))
>  *     (rule "pad2padHV" (clearance 500) (priority 200))
>  *
>  *     (rule "signal" (clearance 20))                       // implied priority of 1
>  *     (rule "neckdown" (clearance relaxed 15) (priority 2))
>  *
>  *     (rule "allowMicrovias" (allow microvia))
>  */
> 
> 
> _______________________________________________
> Mailing list: https://launchpad.net/~kicad-developers
> Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
> Unsubscribe : https://launchpad.net/~kicad-developers
> More help   : https://help.launchpad.net/ListHelp