9 Replies Latest reply on Sep 15, 2011 12:50 PM by jmatthews

    Creating custom solder mask and paste mask openings for a large thermal pad on QFN

    Red5

      QFN packages have a large thermal pad in addition to the signal pins.  I have read a number of application notes that indicate a good strategy is to do the following:

      1) Create the PCB land pad 1:1 with respect to the pad on the part

      2) Use vias distributed on the pad to connect it to copper on other layers for better thermal performance

      3) Use tented vias to avoid having the solder wick down into them

      4) Create a number of small evenly spaced apertures in the paste mask to achieve 50% solder paste coverage on the pad.

       

      Up to this point, I have been using the following solution:

      1) Create the part footprint, but leave off the terminal for the thermal pad.

      2) In the decal editor, arrange "copper" on the solder mask layer to create an opening for the pad that has the "tents" where I plan to place vias

      3) In the decal editor, arrange "copper" dots on the paste mask layer to create the openings for the solder paste

      4) Once the part is placed on the board, I create a copper pour under the part and associate it with the appropriate net to make the connection for the large thermal pad.

       

      Here is an example:

      footprint1sa.bmp

      The green is the solder mask opening, and the blue is the paste mask opening (not 50% coverage on this part).

       

      This method requires some vigilance, because the copper for the pad is not built into the part, and neither is the connection/net.  I can solve the connection/net problem by adding a terminal that is the same size as one of the paste mask dots and locating it in place of one of them.

       

      So here is my question.  Is there a way to create a pad in the decal editor and create custom openings for the solder and paste mask for that pad instead of just having the masks shaped like the pad?  This would be ideal, since all the design information would be included in the part.

        • 1. Re: Creating custom solder mask and paste mask openings for a large thermal pad on QFN
          jduquette

          Answer to your questioin - Yes, you can define 'copper pour' shapes on the solder mask.  Think of them as solder mask pours.

           

          When I've done this in the past I don't place vias under the part.  I define additional pads (and pins on the schematic) so that they are defined with the part.  I define a copper shape for the thermal pad and associate it to an appropriate pad.  Once the pins are connected together on the schematic there are no design errors because the thermal shape lays over all the other pads.  An example (without tenting) is attached.

           

          I believe you'll have to update your Gerber generation to include shapes on the soldermask layer.  There may have been a few other steps in there too.

           

          How did you get an image to show up in the middle of your post?!?  I like that!

          1 of 1 people found this helpful
          • 2. Re: Creating custom solder mask and paste mask openings for a large thermal pad on QFN
            Red5

            Thanks for the response.  I had seen your technique with the vias in my hunting.  Your comment about the associated copper got me headed in a direction toward a good result.

             

            I chose to add a terminal in place of one of the dots I created on the paste mask layer (stencil).  Then, instead of associating copper to it, I just added copper in the shape of the actual thermal pad(not associated).  This pad only contributes a small dot right where I want it to be on both the solder mask and paste mask layers.  On the solder mask layer, I use the same pattern shown in my original post (green area), and it swallows the dot from the terminal.  On the paste mask layer, I also use the same pattern shown in my original post (blue dots), and the dot from the terminal just shows up in the same spot as the dot on the paste mask layer.

             

            I am not going to include the vias on the decal, since there may be cases where they are not wanted.

             

            So the process looks like this:

            1) Create the part footprint, but make the terminal for the thermal pad a small dot (or other shape) where one of the stencil openings is going to be.

            2) In the decal editor, arrange "copper" on the solder mask layer to create an opening for the pad that has the "tents" where I plan to place vias

            3) In the decal editor, arrange "copper" dots on the paste mask layer to create the openings for the solder paste

            4) Once the part is placed on the board, decide whether or not to add vias to the other planes for heat sinking

            5) Use the cam tool to show the copper shapes on the solder mask and paste mask output

             

            In getting to this point, I first used the method of associating the copper with the terminal.  In that case, I had to use the advanced setting for "pads with associated copper" in the cam tool to keep the associated copper from showing up on my silkscreen and paste mask layers.  Unfortunately, turning off the associated copper affects other parts that have associated copper (makes it so the associated copper does not open in the mask for parts that you would want it to).

             

            When we create our cam output for solder mask and paste mask, we use the pads on the top or bottom layer as the starting point.  The bottom line is that it appears the only way to have full control of the solder mask layer would be to create a copy of each pad on the solder mask and paste mask layer for each component decal when it is created.  This way you can customize what it looks like without relying on the copper shapes on the top/bottom layers.

             

            BTW, I just used the little camera icon to add the image in-line.  They may have a file size limit for this feature that prevented your image from being shown in-line.

            • 3. Re: Creating custom solder mask and paste mask openings for a large thermal pad on QFN
              jduquette

              "I am not going to include the vias on the decal, since there may be cases where they are not wanted."

               

              That sounds error prone.  Another designer may see the tents and assume that the vias are already in place.  I recommend adding the vias (component pads) to your standard part.  if someone needs to delete them for a specific board they can make those changes on the PCB.  If they later update the footprint from the library they'll have issues but that will be easy to clean up.

               

              Thanks for the tip on the camera!

              delme.JPG

              • 4. Re: Creating custom solder mask and paste mask openings for a large thermal pad on QFN
                markl

                all your hard work may be for naught

                paste masks are seldom used as they come from CAM output without being modified

                one reason many simply give a 1:1 of the smd

                and let the manf eng and stencil maker tweak it to to what their experience tells them.

                even then they often go thru 2-3 iterations before they get it right

                 

                adding the vias to the decal is a good idea if you seldom have comps on both sides of the board

                but if you often do, it may be better to leave them out and add manually since you don't want to tie your hands of available real estate on the back side of the board for placement

                • 5. Re: Creating custom solder mask and paste mask openings for a large thermal pad on QFN
                  jduquette

                  I used to think that too until I had an assembly house put my job on hold because they didn't like my solder paste layer.  This was a low volume house so they wanted all the 'engineering' done before they got the job.  i agree that almost all higher volume houses will tweak it to their process.

                  • 6. Re: Creating custom solder mask and paste mask openings for a large thermal pad on QFN
                    jmatthews

                    Yup, unless you're dealing with a low-volume "we want everything done up front" shop, let the assembler worry about the paste. I used to work for a  company that does assembly, they liked 80% coverage for the solderpaste.

                     

                    And they liked the vias untented under the part. Actually, they liked the soldermask opening to be 1:1 (or slightly oversized) to the GND slug pad.

                     

                    The nice thing about those "we want everything done up front" shops, they usually have very specific guidelines for how they want past and mask handled.

                    Yup, let the assembler worry about the paste. I used to work for a  company that does assembly, they liked 80% coverage for the solderpaste.

                     

                    And if they liked the vias untented. Actually, they liked the soldermask opening to be 1:1 (or slightly oversized) to the GND slug pad.
                    • 7. Re: Creating custom solder mask and paste mask openings for a large thermal pad on QFN
                      Red5

                      Good to know.

                       

                      In my case, I am dealing with low volume and a local CM.  All the heavy lifting is done by us .

                      • 8. Re: Creating custom solder mask and paste mask openings for a large thermal pad on QFN
                        Red5

                        <off_topic>

                        My wife wants to figure out a way to do Lego mini-figure costumes for our boys this Halloween.  Is that a picture of a costume you made?  If so, would you mind sharing some construction tips?

                        • 9. Re: Creating custom solder mask and paste mask openings for a large thermal pad on QFN
                          jmatthews

                          I should have said: "They liked 1:1 soldermask openings, then we would modify as specified by our component engineer. They liked about an 80% coverage for the solderpaste."