disapearing pads

[Dan]

Good morning,

I have this AMP connector that has 38 SMT pads, and 5 thru hole pads in the center (connecting to ground). Now when I post process the board, and then view my artwork the pads for the bottom side soldermask are not there????? Any help would be greatly appreciated seeing as I've got to get this board done today and I'm running out if time.

GOD I hate my job....

Dan

[Tom]

Dan,

Could you take that Amp Connector and put it in a blank database all by itself and attach it to this thread? I need to verify the construction of the decal. I would also need to know some information. What version are you using V3.6 or V4.0. If you're using V3.6 I can't help you because we do not have any installations of V3.6 running anymore. Once Innoveda released V4.0.1 we dumped V3.6. Let's get your problem resolved. I'm sure it's just a simple oversite.

[Dan]

Tom,

I'm using 3.6, so I shouldn't bother sending you the component. I've looked the decal over and it appears that there is copper associated to the pad????? Could this have anything to do with it?

Thanks,

Dan

[Tom]

Dan,

Yes, Associated Copper has an effect on your Soldermask output process. Whenever you have a pad, PowerPCB uses it to process Soldermask data. Whenever you associate copper with a pad, the associated copper takes the place of the pad. I.E.: Postprocessing no longer looks for the pad when it produces Gerber data it looks at the associated copper.

In PowerPCB V4.0 there is an updated "Layers Menu" in the CAM routine that has this new feature:

Pins with associated Copper:
O Advanced Selection
O Pads
O Open Copper
O Filled Copper

If you can, I would upgrade to V4.0.1. there are many new great features and has minimal bugs.

[randychase]

See this:

http://www.innoveda.com/support/kb/powerpcb/ApplicationNote/Applications_of_Associated_Copper.htm

You need to define the soldermask shape on those pads on layer 28 and then add Layer 28 pads to the CAM output.

[Tom]

The solution that Randy has provided is something that we built into all 8,000 PowerPCB decals in the pcbstandards library. Every part has full padstacks so the user is in complete control of your output. Then you will begin to like your job. :-)

[Dan]

I don't really understand why associating copper to a pad would change it's purpose? Guess that's just another thing I don't understand about PADS. I defined copper in the post processing of the soldermask layer, does it see it as copper or a pad? Should I never associate copper with a pin?

Tom,

Are you saying that you define every layer in the pad stack? Do you define it by saying layer one is .050, layer 2 is .050, layer 3 is .050, etc, or do you define inner layers as all inner layers. Do you also define soldermask top and bottom, solderpaste top and bottom? Why don't you just oversize in CAM?

Just want to get it clear.

Dan

[Tom]

Dan,

On Surface Mount decals we define the following padstack layers:
Mounted Side
Solder Mask Top
Paste Mask Top
Assembly Drawing Top (only on large parts)

On Through Hole decals we define the following padstack layers:
Mounted Side
Inner Layers
Opposite Side
Solder Mask Top
Solder Mask Bottom
Assembly Top
Assembly Bottom
Layer_25 (for CAM Plane Technology)

That's it. We only define what we need, not every available layer.

[Dan]

Thanks Tom,

But what about the associated copper? Should I not use it on pads, does it just cause too much confusion when I try to process in CAM?

I guess I should do what Randy suggested, and add that associated copper to all layers that loose the pads. Kinda a major pain in the ass, but if it's the only way to make it work........ I better get back to work, the pressure is mounting to get this board out.

Thanks for all your help today.

Dan

[randychase]

Originally posted by Dan
I don't really understand why associating copper to a pad would change it's purpose? Guess that's just another thing I don't understand about PADS. I defined copper in the post processing of the soldermask layer, does it see it as copper or a pad? Should I never associate copper with a pin?

The link I provided goes into the history of why this is the way it is. In the old days, they made surface mount parts with breakouts built in. The associated copper was the real pad. The round drilled pad was a via that most people would not want open from the soldermask so it was suppressed.

The question now is why it stays that way. I think doing it this way would be rare.

Like Tom mentioned, our libraries have full pads on mask layers and paste and assy layers too. That way you have 100% control when you CAM out. You will find that a lot easier to use when you use BGAs.

I still associate copper to pads. It's easy to fix.

For a quick fix (since you are under the gun), just revise the padstack of that one part to add pads on Layer 28 (Soldermask Bottom) and revise your CAM output to include pads on L28. It's just that one layer and only the parts with associated copper connected to a thru hole pin.

Or more crudely, draw some copper pads on Layer 28 on those pins. Been there, done that. It works.

But, let me ask you this. I am curious. Why do you have these associated coppers connected to these pins? I find there are not that many times I need to do this that I can't do it outside the decal itself. In other words, create a copper shape on the board for current or thermal or connectivity reasons and assign it the proper net.

[Dan]

Randy,

The decal has through hole pins in the center of the component. If you add additional solder to the paste in the shape of a rectangle (per AMP's spec sheet), you can run this part through reflow and not have to wave the through hole pins. Saves an assembly process, or additional solder touching of that component.

I don't know who built this decal, so I just found this issue. Maybe this was how it had to be done in prior releases of PADS???? Still very new to the SMT world.

Thanks for your help, I have my work around for now to keep me going.

One more thing.... now that I'm doing SMT, should I change from using RS-274D to RS-274X?

Dan

[Tom]

Dan,

Yes, you should be using RS-274X. And I would highly recommend that you "Regenerate Apertures" prior to postprocessing Gerber data. Regenerating converts your SMT drawn pads to Flashes. Saves data space by making smaller Gerber files and speeds up the fabrication front end process.

[gerald gutowski]

Randy or Tom

while on this subject, why do you have the solder mask and
assembly pads the same size or smaller as pads on electrical
layers

[Tom]

Gerald,

We are working very closely with some PCB manufacturers. So close that you form a trusting relationship. The pcbstandards library has full padstacks that contain Solder Mask, Paste Mask and Assembly Layer. The library is used for a diverse realm of PCB design layout trace width and spacings.

Here are some of the popular trace width / spacing:
0.1mm (.004")
0.125mm (.005")
0.15mm (.006")
0.2mm (.008")
0.25mm (.010")

The routing grid for all these trace widths is the same 0.05mm.

The reason why all the Solder Mask sizes are exactly the same as the pad sizes is that we let the manufacturer perform a global "Oversize" on the 1:1 scale Solder Mask to whatever they feel is the best manufacturing practice for whatever trace / space was used for that particular design.

Our manufacturers pleaded with us to make the Solder Mask 1:1 scale to allow them to perform their global oversizeing from a known starting point. They said that they wish that every customer would provide 1:1 scale soldermasks so that they could get the highest yeild from the batch. Hallmark Circuits said "Please do not try to do our job for us. We know what we are doing and we will give back to you the best results. We know our equipment and our tolerance factors. Let us determine what is the best Solder Mask oversize."

You can't argue with that and we're not about to. Letting the PCB designer perform the Solder Mask oversize has a potential for screwing up the manufacturing process. They obviously know their equipment and their capabilities better than I do.