Can anyone tell me how to create a pad on a PCB decal that can be tied to the GND net but which has no soldermask or pastemask openings? Much appreciated.
FYI, this came from SupportNet, a very good source for answers to questions like yours:
Or go to the Listserver, an almost better resource (you can interface with some very experienced designers there):
It is useful to know the function. Furthurmore, could only several pads in a components is suppressed?
Yes, but you would need to have built your Decals with padstacks (aka define soldermask pad(s) and/or solderpaste pad(s) for the surface pad(s)).
If you do pad stacks, I would say not to use the default oversize function. Based on conversations I've had with some fabricators, I would reccommend that the default soldermask opening should be 6 mils (~0.15mm) over the pad size (for example, a 0.060" RD pad would get a 0.066" mask opening).There are exceptions to this of course, but they will normally be defined by the engineer or by the MFR data sheet. Some examples of exceptions would be ganged openings for QFPs, a reduced opening (like 4 mils or less) on high-density BGAs, reduced or removed mask openings for vias, oversize openings on fiducials or mounting holes, things like that
Unless you always use the same shop, or are captive to a company that does its own assembly and know exactly what the shop wants, I would make the solderpaste pad 1:1 to the SMT pad, and allow your assembler to redefine those as they see fit.
You can then edit the Decal at the board level to selectively remove or modify soldermask and/or solderpaste for specific pads on specific parts (much like how you can modify specific anti-pads and/or thermal connections now).
Otherwise, you would need to edit the Gerbers using CAM350 or a similar program. Do-able, but, IMHO, not really a good idea.
It is lovely to learn your introduction, every functions work very well. which bring more flexibility for PCB design.
However, the selection of "pins with associated copper" didn't work, please refer to attached picture. That means, even I select the tick marked box. Only pads but not including associated copper is display in past mask layer of gerber file.
My Pads version is "Pads 2007". Could you please answers it is my wrong operation or a bug in the software.
I don't know why did you do that? Is it the sme to no PCB Dcal ?
On one particular tiny quad package I am using the only way to connect all of the ground pads is from the center of the part by using a via in the center and pouring copper over the inside. But this part also has a square pad in the center of the part. (usually connected to copper for heat transfer but not in the case of this part) I do not want to change the decal to remove the center pad. The manufacturer indicates that the center square pad is not to be connected to ground. So I have a decal with a center pin pad that I don't want solder or paste mask openings. Thanks for all of the advise.
That is good method to deal with this issue! Thanks for your explanation,
Retrieving data ...