kicad-developers team mailing list archive

[Wayne Stambaugh <stambaughw@xxxxxxxxxxx>]

On 6/9/2014 2:01 PM, jp charras wrote:
> Le 09/06/2014 19:23, Lorenzo Marcantonio a écrit :
>> On Mon, Jun 09, 2014 at 06:56:25PM +0200, jp charras wrote:
>>> For guys who are interested by theses extensions (I am thinking a change
>>> in Gerber Format should have a major interest for everybody), see:
>>
>> The extension in themselves are quite interesting. If only to say 'this
>> is the top layer' inside the file (and not using some other method).
>> Could nearly replace D356, too.
>>
>> The only problem will be acceptance by the tool manufacturers (i.e. will
>> my fabricator accept X2 gerbers?)
> 
> The best way is to ask them for that.
> 
>>
>> I think that *maybe* in a few years we will know the answer.
> 
> 
> Gerber X2 fixes a *major issue*: the stack order.
> Therefore IMHO, accepting X2 gerbers is not a matter of years.

JP,

I'm sure you already thought of this but making X2 gerbers a plot option
solves both problems and it shouldn't be too difficult to implement.
It's probably safer this way just in case someone has a board vendor
that cannot handle the X2 gerbers.

Wayne

> 
>>
>> I skimmed the specs and, knowing the tools out there, X2 is *not*
>> backward compatible. Most of the tools out there will probably choke
>> horribly on the first %TF or %TA they encounter. The 'short header
>> option' IIRC is there just to make the gerber readable anywere... It
>> would be a truly backward compatible specification if they used some
>> structured form of G04 (something like the structuring in postscript).
>> IIRC it's not written anyway that 'any unknown mass parameter should be
>> ignored'
> 
> After loading a GERBER X2 file:
> Gerbview does not choke (run fine).
> Gerb does not choke ( has only some warnings)
> GC-Prevue does not choke ( has only one warning)
> 
>>
>> Drill files as plots are cute but nothing extraordinary; they could have
>> their use but I don't see them replacing excellon or s&m tapes...
> 
> Excellon works fine, no need to replace this format.
> 
>>
>> I think a good way to implement attributes would be to make them
>> optional (maybe putting them in a G04 block as a debug/documentation
>> aid).
>>
>> PS: somewhere in there they say that kicad does planes in the wrong way (who
>> cares... I've seen worse things:D)
> 
> What do you mean? currently, Kicad does not know planes.
> If you are talking about negative objects in Gerber files examples, I do
> not see any reason to use negative objects in gerber files (at least for
> copper layers): this is known as a bad practice.
> 
>>
>> PPS: in the list of the standard attributes there is a list of layer
>> types; that could be very useful for the other thread!
> 
> I agree.
> In examples, there is also an idea for gerber file names.
> 
>