4 Replies Latest reply on Nov 10, 2015 9:08 AM by carl.triglia

    Selective solder mask for parts


      Looking for input into the following dilemma that we are facing.


      I have a pwb with several areas that need to have solder mask and several areas that do not need solder mask. This is easy.

      Here's the problem, I want to place a 0.006" piece of solder mask around each pad in the area that does not need solder mask.

      This is needed because some of the pads are flooded over with ground plane and we use the solder mask as a way to stop the part from floating to one side.

      We have placed a note on our fabrication drawing and placed notes on the solder mask gerber trying to explain this.

      Some board houses got and some just didn't.

      We would like to incorporate this into the PADS file so there would be no confusion at the board fabricator.

      We have experiment with copper on the Solder Mask layer and works for a simple opening but not too well when there are a lot of components and via's.

      See attachment for clarification.

        • 1. Re: Selective solder mask for parts
          David Ricketts

          This can be done, but you need to use a different way of creating the soldermask, so it takes a little while to set it up, but once that's done, it's reusable for editing and new designs. The term to describe the lines being created is solder dams. This technique might take some experimenting and practice to get it to where it's easy to use, but it works.


          As it's implemented in PADS, soldermask is a negative space. So wherever you draw something solid, there's no soldermask, and where there's a void or opening, there is soldermask.


          The trick is to create the soldermask opening for the RF areas using a copper pour on the soldermask layer. The smaller the line and grid used for the pour, the sharper the corners.


          To define the soldermask dams on the parts, add copper cutouts placed on the soldermask layer to the decals. You can draw lines to define where you want the dams, then use those as guides to draw the cutouts, then delete the lines. This has to be done for every decal type used in the RF area defined by the copper pour on the soldermask layer. Update your parts on the board with the new decals. The weird part is the cutouts aren't visible on the board level unless you move the part, but you'll see their effect once you flood the soldermask pour. You can probably use one decal for both RF and non RF, or you can use separate decals, but how you implement this is your choice.


          Vias can be covered if you want by adding an antipad on the soldermask layers. Give these vias a new name to avoid mixing them up in the non RF areas.


          Anytime you move or edit a part, the soldermask will need to be re-poured, but if you write this into your post-processing check list, you'll be OK. You do have one of those, right?


          There may be some more details I'm forgetting, so good luck.

          • 2. Re: Selective solder mask for parts

            Thanks David for the response.

            I will give it a try and see what happens.

            • 3. Re: Selective solder mask for parts

              Are you using PADS layout? How do you flood a pour on the soldermask layer?

              • 4. Re: Selective solder mask for parts

                I figured it out!  I had to change the layer definition for the soldermask to "General".


                Thanks for the input!