kicad-developers team mailing list archive

[jp charras <jp.charras@xxxxxxxxxx>]

Le 01/05/2017 à 10:37, Nick Østergaard a écrit :
> 2017-05-01 8:25 GMT+02:00 jp charras <jp.charras@xxxxxxxxxx>:
>>> Hi,
>>>
>>> Lachlan sent me a complex board in Eagle that has several copper zones,
>>> each with different clearances, which filled incorrectly or didn't fill
>>> at all. There were some trivial issues (e.g. inverted filling priority),
>>> but there is one that needs discussion:
>>>
>>> In pcbnew, each zone must have manually assignned clearance (in the
>>> property window). In Eagle or Altium, if there's no clearance specified,
>>> the program takes the clearance set in the Design Rules for the net the
>>> zone belongs to.
>>>
>>> I propose to add a similar feature to Kicad, that is:
>>> - add a checkbox "use custom clearance" in the zone properties window
>>> - if not checked, take the netclass clearance.
>>>
>>> This unfortunately requires a small file format change. Would you agree
>>> with that?
>>>
>>> Also, many thanks to Lachlan for spotting this problem!
>>>
>>> Cheers,
>>> Tom
>>
>> About zones clearances:
>> the actual clearance is the min between the zone clearance and the netclass clearance.
>> Therefore to use the netclass clearance, just set the zone clearance to 0
>> (or to any value smaller than the netclass clearance).
>> No need to change the file format.
>>
>> About clearance between board edges, or any obstacle, the Margin layer was intended to control this
>> clearance, but not yet in used.
>>
> 
> I have been wondering for a long time how this layer is supposed to be
> used. I there any functionality associated with the layet at the time
> of writing? If not, how is one supposed to use it when it is
> implemented?
> 
> In my mind it makes sense to specify a pull back property to the edge
> cuts lines.  AFIK the spec is usually to have a minimum pullback for
> some reason, and if one needs more in some section of the board, then
> it is not really a pull back in that sense anyway and should be
> handled "manually" by adding a cutout or keepout zone. This is my
> immediate thoughts on this, there may be use cases I have missed here.

Currently, no functionality is associated with the Margin layer.
There is no code attached to this file.

What I had in mind when providing this layer is:
- having a common layer (any graphic item on the Margin layer is also seen on other copper layers)
mainly to define obstacles. This is similar to edge cuts, but with an easy control of clearances.
- this layer is not intended to be plotted (at least to create Gerber files for manufacturing)
- A graphic item define a clearance area (the that is the shape and size of the item)

It is similar to a cutout zone, with a few differences:
- it is common to all copper layers
- a single line defines a clearance on all layers (much more easy than a zone cutout to define a
clearance around the board edges).
- it is clearly displayed on board, and can be plotted for testing.
- this clearance can differ from edge cuts, for instance for castellated holes or keepout areas in
footprints.

-- 
Jean-Pierre CHARRAS