Via-in-Pad Problems

[mdldesign]

Hi All

I had an interesting problem occur when I tried to make a .8mm BGA use both SMD pads and thruhole pads (silver filled). When I output my paste master, it would not place pads on the thruhole pads, just the true SMD pads. I even included pads on the paste layer, but they just wouldn't appear. I added the pads with a gerber editor, but I really hate doing this.

It bothers me that PADS wouldn't do what I was asking it to do, no matter what I tried.

Does anybody know a process that works in this situation?

Mark
MDL Design

[Tom]

Mark,

PowerPCB will post process Layer_23 (Top Paste) if you put Layer_23 in your padstack and process Layer_23 PADS. We do this all the time because the pcbstandards library has full padstacks and it works great. As a matter of fact, when we produce a Paste Mask, we just process Layer_23 (and Layer_19 for the targets and title block). We do not process Layer_1 when creating a "Top Paste Mask" because all 8,000 parts in the pcbstandards library have full padstacks. Please let me know if you still have problems processing the correct data you need. I will be able to help you figure it out.

[mdldesign]

Tom

Thanks for your reply! Yes, as I mentioned (maybe you missed it), I did have/try pads on the paste layer, but they failed to materialize. I think PADS will not put any paste info on a thruhole pad, and there's just no controlling this "added" feature.

I should mention that I haven't upgraded to version 4 yet. Maybe this was addressed there. It may be time to get my feet wet and test the 4.0 water.

Mark

[Tom]

Mark,

I read your post and I didn't know if you were processing "PADS" on Layer_23. Another workaround is to put Copper Circles on Layer_23 and process "Copper" on Layer_23. You can copy and paste Copper Circles pretty fast. Try an experiment with that, but I am positive that PADS on Layer_23 works. At least in V4 it does. We are and have been using PowerPCB V4 since August 2001, so I can't duplicate your problem.

[randychase]

You have to output a Custom Gerber using the pastemask layers, not a standard Pastemask gerber. PowerPCB will not output drill pads to a Pastemask Gerber in CAM, even if you have them built into the padstacks. Just output a Custom Gerber.

[mdldesign]

Tom, Randy

Thanks for your help. I've installed version 4.1 now, and here is what I've found:

Version 4.1 has the same problems as 3.6. It won't put pads or copper on thruhole pins when creating a paste mask, even if these items are added to the paste layer in the stackup.

It will work, with both versions, using custom as Randy suggested, either using a pad or copper on the paste layer.

This brings up an interesting point. I've always shied away from building full padstacks into my footprints. One of the powers (or weaknesses in some cases) in PADS has been it's ability to build the padstacks on it's own.

The one weakness I've found is when I want a smaller pad used on my artwork. I've always just edited the gerber file to make this happen, which is something I don't like to do either.

I would like to see PADS do something about these problems rather then forcing me to build padstacks again. I might as well be designing with Allegro (god forbid).

It's interesting to see that you've made your pcbstandards library in this fashion. At least I'll have a good start in building new libraries, should I decide to incorporate this new "feature". I give you lots of credit and thanks for doing this.

Thanks again
Mark

[randychase]

Mark, I very much agree with you regarding padstacks. I loved the ability to automatically handle soldermasks and pastemasks in PADS. I did not really understand why Tom did the padstacks as he did. But I kept running into boards that required special pads, such as most BGAs.

Then it made sense. Since our libraries had them built in, it became easy to use them that way, and add them to the few existing custom parts I had already made in the typical board.