> >I try to find out how many SMD-pad I have in my design.
> [snip]
> >I need the Paste Mask cout for an offer for an Laser Stencil
> >(www.schablone.de).
> >
> >Edi
>
> Some PCB manufacturers ask for the smt pad count for
> their quotes. To accommodate them, I do the following:
>
> First, do a Reports/Board Information. Now the tricky part,
> subtract the number of vias from the Pad/Via Hole count.
> This will give you the number of pads with holes. Then
> subtract this number from the number of pads. What is left
> over should be the number of pads without holes (i.e. smt pads).
> I've verified that this works by manually counting smt pads. Although
> I haven't actually done this exercise since P98.
>
> Jeff Stout
Bear in mind that there *might* be pads on layers *other* than the Top
copper, Bottom copper, and MultiLayer layers. Additionally, some of the pads
on the outside copper layers might be masked on the Paste Mask layers (with
fiducial pads being one such typical example).
So I would suggest that you generate Gerber files from the Top Paste Mask
and Bottom Paste Mask layers, then *import* these into a blank/new PCB file.
After so importing these, do a Reports/Board Information to get a pad count.
(If you want a count of the number of pads on *each* side, do a
Reports/Board Information, *before* importing the *second* such file, to get
a pad count for the *first* file imported. Note/save that number, then
subtract it from the number reported after importing the second file, in
order to get a pad count for the second file.)
(This previously blank/new PCB file can then be discarded, unless you have
some other reason for retaining this.)
I was going to suggest using the "Edit/Export to Spread" command (to acquire
details of all pads within the PCB file), but that would incorrectly count
pads on the copper layers which were masked on the Paste Mask layers. OTOH,
the above approach correctly caters for such masked pads (as they are not
incorporated in the Gerber files, so will not be counted), along with any
pads which might have been specifically placed on the Paste Mask layers (as
opposed to being placed on the outside copper layers).
How much user interest would there be in having a Process provided which
counts the number of pads on each Paste Mask layer (to avoid the requirement
to import Gerber files produced from these layers into a previously
blank/new PCB file in order to acquire such a count)? I am still working
(with assistance from Ian Wilson) on a PCB inverting server, but this is
something that I could do at some stage, *if* there was sufficient user
interest.
Regards,
Geoff Harland.
-----------------------------
E-Mail Disclaimer
The Information in this e-mail is confidential and may be legally
privileged. It is intended solely for the addressee. Access to this
e-mail by anyone else is unauthorised. If you are not the intended
recipient, any disclosure, copying, distribution or any action taken
or omitted to be taken in reliance on it, is prohibited and may be
unlawful. Any opinions or advice contained in this e-mail are
confidential and not for public display.
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/subscrib.html
* - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/[email protected]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
