Re: gEDA-user: Composite/negative layers in gerbers

[DJ Delorie <dj@xxxxxxxxxxx>]

> My board house[1] has complained about my gerbers having "negative
> plots" and "composite layers".

Can you send us examples?  Which PCB are you using (hid or pre-hid)?

> 1) (Main question) How can I tell if my gerbers are negative and/or
> composite so I can check?

In the gerber file itself, look for the strings IPPOS and IPNEG,
and/or LPC and LPD.  For pre-hid PCB, also search for LNCUTS.

A generic trace layer will have IPPOS (positive polarity) and LPD
(draw the "dark" parts).  IPNEG is a negative polarity layer,
sometimes used for ground/power planes if certain conditions are met.
LPC means we're drawing "cuts" or "clears" to erase previously drawn
stuff, such as when we make clearances for traces through polygons.

> 2) What can I do to affect whether pcb uses negative and/or composite
> outputs?  Is that what the "Invert positive/negative" tick box on the
> printing page does, at least for the negative stuff?

There's not a lot you can do, because there's not much else we can do
to make clearances.  The Gerber spec itself says to use LPC to make
clearances.  The gerber HID doesn't use IPNEG yet, so that might be an
option for you at the moment.