No announcement yet.

Paste Design on Package Layout

This topic has been answered.
  • Filter
  • Time
  • Show
Clear All
new posts

  • Paste Design on Package Layout

    Packages that have a thermal pad, for example qfn packages, have the paste broken into smaller blocks, some datasheets give a guideline, but some
    does not have a guideline, Is there a paste calculator in the industry that we can use?, Thank You.
  • Answer selected by Lakshamana Balakrishnan at 04-15-2022, 08:50 PM.

    JohnsonMiller It is not only a question on how easy it could be for Altium. Also consider the possible downsides to this.

    As I mentioned previously, paste mask is fabrication type output, even though it is used for the assembly. It is coupled with the layout.
    If you create 2 variants, with varying (not) fitted components, you would need two stencils. As WhoKnewKnows mentions, solder paste costs money. A stencil also costs money. And using the wrong stencil for a production cycle is the most expensive. When you do not produce that many products <= 10k/year, I do not think that saving on solder paste is worth it.
    People may export wrongly, expecting the single paste mask export works for both variants.

    And finally, if Altium make the paste mask expansion in the variant, then why also not the solder mask, oh and track and pads, footprints. Can you imagine how complex Altium would get?
    For a recent session I did for production data, I created a document containing almost 70 bugs and ideas. Most of these are just for the basics - schematic, layout and data export. Sure there are many advanced things I would like to see, but I would much more like the basic tasks to work correct, smooth and consistent.


    • #2
      Hi Anlau ,
      A general guideline is to have the paste layer at about 70% of pad size.
      I have been using this for a while now and it is working fine for me.

      Thank you..


      • #3
        The paste shape(s) is an opening in a stencil that a squeegee passes over. It fills the opening with solder paste. If the opening is too big, the squeegee flops down into the opening as it passes by and starves the opening of paste. If a rigid squeegee is used it doesn't starve the opening, but over a certain size, too much paste is deposited. Dividing a large opening into smaller opening reduces overall opening size and gets you the best deposition performance no matter what squeegee type is used. If lots of fine pitch features are used in the design, then a thinner stencil may be needed. Thinner stencils reduce deposition amounts, so you may have to increase opening sizes on your windowed parts.


        • #4
          Anlau Hope this calculator helps!!


          • #5
            This video will help you, we talk there about it:
            How to create perfect PCB Footprint - What you really need to know


            • #6
              I was hoping someone would point to a nice document or IPC standard, but so far I am unlucky.

              Let me first comment on some of the other reactions:
              chitransh92 I do know that fabricators tend to modify the design without notifying the designer. Perhaps it is more often that they split larger shapes into smaller ones. However, a coverage of 60...80% is mentioned sometimes by others as well.
              WhoKnewKnows Exactly, but do you know of any guidelines or standards for the shapes, maximum sizes, coverage, etc.?
              Lakshamana Balakrishnan I do not see how that calculator can help...
              robertferanec Perfect footprint, but unfortunately Library Expert does not create smaller paste mask 'pads' for big pads.

              Now my own set of ideas.
              The shape and size of the paste mask opening depends on many parameters:
              1) Thickness of the stencil
              2) Type of solder used
              3) PCB finish used
              4) SMD or NSMD (Solder Mask Defined)
              5) Production method of the stencil

              For thermal pads there are also the via's which may or may not be filled. Size of the hole, solder mask, etc.
              Some manufacturers spend more time on how to produce there products then others, but at the same time also limiting the options of stencil thickness and solder type.

              One of the interesting documents I have found on the paste mask is:
              Unfortunately, no mentioning of dividing large pads into smaller sections.


              • #7
                qdrives TBH, I don't remember where I came to know how, but I've always targeted about 70 to 75% of the full pad area. Another thing for folks to keep in mind is if the design isn't already a dedicated via-in-pad design where the vias will be filled and plated over, the designer can have vias in the power patch of a QFN or similar, but they need to line up things so the "windows" fall where the vias ain't. Or, the window frame needs to cover up the vias so the paste gets deposited on the pad away from the vias. In this case, I usually increase the amount of solder deposited, because there's still going to be some lost to the vias, but at least you're not starting off by covering the vias with solder paste and inviting the loss.


                • #8
                  qdrives your document is wonderful. By the way, that calculator helps us to determine the Area Ratio of the Solder Paste. Please refer the below picture

                  Click image for larger version

Name:	Capture.png
Views:	181
Size:	21.9 KB
ID:	19013

                  From the above picture Orignal Gerber is COPPER PAD and Recomendations are Stencil Dimensions, If both satisfies area ratio as like above. We can go with choosen value for Manufacturing Stencil film capability.


                  • #9
                    robertferanec actually I watch the video today, again after the initial release. So much information in it.
                    Lakshamana Balakrishnan It is not my document ;-) I looked at the calculator but could not determine how it works. The report seems to have more details.

                    I asked Tom Hausherr about breaking the pads into small parts for big components like inductors. His answer is no, it is only needed when there is no way for the solder to go as is the case with the exposed pad. Link


                    • #10
                      What happens when we set variant and some parts are not fit, can I expect no opening for those parts in the stencile?


                      • #11
                        Fitted/not-fitted status typically affects schematic appearance and component count on the BOM, and doesn't affect solder stencil openings. That would be a cool option, though.


                        • #12
                          But this was all parts either fitted or not fitted will receive the paste, I have seen boards that not-fitted parts do not receive paste, and pads of those parts are clean with original surface finish.
                          In my opinion, variant change should affect the stencil.


                          • #13
                            JohnsonMiller Paste mask is in the fabrication. At the moment variants are only on the BOM. There is an option for variants in fabrication, but I do not know if this is only for text elements.

                            Another solution is to put all the optional components in a special component class. Use that class (or classes) to select the components and, by using a filter, adjust the paste mask opening.
                            This is a manual operation, but if you really need the pads to remain clear, it may the easiest way to do this.


                            • #14
                              Originally posted by JohnsonMiller View Post
                              But this was all parts either fitted or not fitted will receive the paste, I have seen boards that not-fitted parts do not receive paste, and pads of those parts are clean with original surface finish.
                              In my opinion, variant change should affect the stencil.
                              Did you see this in an Altium project, or are you referring to some PCBAs that you've seen manufactured?

                              To clarify, I'm just not aware of how to make Altium automatically change the paste mask status on parts when they change status to not-fitted. It may be possible. Meanwhile, if you're referring to PCBAs that you've seen like this, in some cases the CM will block off sections of the solder stencil to reserve paste from going onto a section of the PCB that's not getting populated. Solder paste isn't cheap and it isn't usually a tangible invoiced item, so CMs save it where they can.


                              • #15
                                I think some assembly houses may only have 1 stencil with all openings and cover some of the openings with some sticky tape. But normally they don't do that unless there is a really important reason to do it. However, I am not sure why we would like to do that, is there any special reason?