Advice For Solder Mask & Paste Mask Layers

Message Topic Search Topic Options Post Reply Create New Topic Printable Version Translate Topic

Dear Tom Hausherr or maybe another expert,

I’m not exactly sure if I’m at the right place to ask a question I’m wondering about for a long time! It is about your definite advice for the specification of solder mask and solder paste layers. In several publications you recommend a 1:1 clone of the pads. I know about several board manufacturers who recommend this approach as well. I don’t know about PCB assembly facilities (for recommendations on the solder paste layer). But I guess they are making the necessary adjustments for reliable results just like the board manufacturers do with the solder mask layer.

However, and now comes the hard part. On several locations on all the published material you give specific instructions to deviate from the baseline 1:1 recommendation. These are for example:

1.    Solder mask defined pads under fine pitch BGA packages.
2.    Multiple separated squares on the paste mask layer to create 50% area reduction in the thermal pad of a QFN package.
3.    Maybe it is not directly your advice but somewhere I red about putting solder mask on these thermal via to avoid solder paste wicking.
4.    The solderdam (stroke of solder mask) approach to avoid solder paste wicking in via-in-pad technology.
5.    Etcetera

Questions

1.    What is your final advice to me regarding defining solder and paste mask layers to me as a PCB layout engineer.
2.    It would be totally awesome if you can find to time to sum up every situation when a PCB designer needs deviate from the baseline 1:1 advice, or could you point me to a recourse that provide this information.

Regarding point 1 (not question 1) , you wrote in your original blog: “When you use solder mask defined lands you must indicate which parts deviate from the 1:1 scale solder mask rule in the fabrication drawing notes to notify the CAM operator not to swell these solder mask features.”

3.    I’m pretty new to my role as PCB layout engineer, but this seems error-prone to me. Isn’t there a more automated process to clearly indicate which features deviate from the 1:1 rule. Also the mixed influence (by me and the CAM operator) of the final definition of these masks layers seems very unreliable to me. Moving from vendor to vendor might require heavy adjustments of the mechanical layers because every vendor have a different approach on this. What could you recommend me regarding these concerns?
4.    In my eyes it would be best to provide the vendor a separate mechanical layer for each type of tool they are using. For example a separate mech layer for: milling, via-fills, gold plating, V-scoring, cutouts or whatever additional process have to be performed on the board. Ideally they only need to feed the right Gerber layer to the right machine maximizing the automation. Or am I missing something?

You are improving me strongly in my understanding of the whole PCB manufacturing process if you can provide answers to these questions!

Thank you very much for your attention and time!

Best regards,
Maarten Verhage

Author	Message Topic Search Topic Options Post Reply Create New Topic Printable Version Translate Topic
Maarten Verhage Members Profile Send Private Message Find Members Posts Add to Buddy List Active User Joined: 27 Jul 2012 Location: Netherlands Status: Offline Points: 27	Post Options Post Reply Quote Maarten Verhage Report Post Thanks(0) Quote Reply Topic: Advice For Solder Mask & Paste Mask Layers Posted: 27 Jul 2012 at 7:32am
	Dear Tom Hausherr or maybe another expert, I’m not exactly sure if I’m at the right place to ask a question I’m wondering about for a long time! It is about your definite advice for the specification of solder mask and solder paste layers. In several publications you recommend a 1:1 clone of the pads. I know about several board manufacturers who recommend this approach as well. I don’t know about PCB assembly facilities (for recommendations on the solder paste layer). But I guess they are making the necessary adjustments for reliable results just like the board manufacturers do with the solder mask layer. However, and now comes the hard part. On several locations on all the published material you give specific instructions to deviate from the baseline 1:1 recommendation. These are for example: 1. Solder mask defined pads under fine pitch BGA packages. 2. Multiple separated squares on the paste mask layer to create 50% area reduction in the thermal pad of a QFN package. 3. Maybe it is not directly your advice but somewhere I red about putting solder mask on these thermal via to avoid solder paste wicking. 4. The solderdam (stroke of solder mask) approach to avoid solder paste wicking in via-in-pad technology. 5. Etcetera Questions 1. What is your final advice to me regarding defining solder and paste mask layers to me as a PCB layout engineer. 2. It would be totally awesome if you can find to time to sum up every situation when a PCB designer needs deviate from the baseline 1:1 advice, or could you point me to a recourse that provide this information. Regarding point 1 (not question 1) , you wrote in your original blog: “When you use solder mask defined lands you must indicate which parts deviate from the 1:1 scale solder mask rule in the fabrication drawing notes to notify the CAM operator not to swell these solder mask features.” 3. I’m pretty new to my role as PCB layout engineer, but this seems error-prone to me. Isn’t there a more automated process to clearly indicate which features deviate from the 1:1 rule. Also the mixed influence (by me and the CAM operator) of the final definition of these masks layers seems very unreliable to me. Moving from vendor to vendor might require heavy adjustments of the mechanical layers because every vendor have a different approach on this. What could you recommend me regarding these concerns? 4. In my eyes it would be best to provide the vendor a separate mechanical layer for each type of tool they are using. For example a separate mech layer for: milling, via-fills, gold plating, V-scoring, cutouts or whatever additional process have to be performed on the board. Ideally they only need to feed the right Gerber layer to the right machine maximizing the automation. Or am I missing something? You are improving me strongly in my understanding of the whole PCB manufacturing process if you can provide answers to these questions! Thank you very much for your attention and time! Best regards, Maarten Verhage



Tom H Members Profile Send Private Message Find Members Posts Add to Buddy List Admin Group Joined: 05 Jan 2012 Location: San Diego, CA Status: Offline Points: 5718	Post Options Post Reply Quote Tom H Report Post Thanks(1) Quote Reply Posted: 27 Jul 2012 at 8:23am
	It's IPC that has long recommended the 1:1 scale solder mask & paste mask. However, the new PCB Footprint Expert has the unique ability to generate complete libraries that adhere to the User Preference Rules. This means the user can create a rule file for a specific PCB layout, put all the parts for that layout in a unique FPX file and one click create the library. This may be the future for PCB layout because of its accuracy and simplicity. Maybe having a master library that's used on every design is not the solution. But being able to quickly customize a PCB library for a specific application is the solution. Years ago we used to do this and we told PCB fabrication not to touch the Gerber data because we designed a perfect board with a perfect library. Now, if the solder mask and paste mask are 1:1 scale we must have special notes on the fabrication and assembly drawings with instructions for mask adjustments or otherwise we won't get what we want. A real good example of this is Flexible Circuit Boards where it is best practice to solder mask define the Toe and Heel but not the side for the purpose of improving the pad adhesion to the Flex surface. Then the paste mask stencil also needs to be customized so that the paste is deposited on the exposed pad and not the solder mask covering the pad Toe and Heel. Another example is fine pitch BGA part pads need to be solder mask defined to secure the pad to the board to pass drop tests. It has been proven that during drop tests a BGA solder joint will survive better than the pad ripping off the PCB surface because the pad size is so small. So solder mask defined BGA pads for fine pitch BGA's help adhere the pad to the PCB surface resulting in drop test success. So all PCB designers are left with 2 choices. Use a stock library with 1:1 scale masks and create fabrication and assembly note instructions for solder mask and paste mask adjustments Create a custom library for a PCB layout and tell the manufacturer's not to touch (adjust) the Gerber data.