Group Actions
Engagement
  • Author Author: fmilburn
  • Date Created: Date Created
  • Views 2400 views
  • Likes 11 likes
  • Comments 22 comments
Related
Recommended

Microscopes and Solder Masks

fmilburn

Now that the TI-RSLK robot RoadTest is finished I have turned my attention back to a problem spotted in the last round of PCBs ordered for the AIS alarm project.  But first, I have a new toy.

image

I have been looking for the right used Nikon microscope in budget but finally could not stand it any longer and bought this Chinese model after my friend bought one.  I am amazed at how much better this is than peering through a magnifying glass or loupe.  At low magnification stereoscopic details pops and there is good depth of field.  I bought a version that takes a C-mount camera but don't have a camera yet.  Good value for the money I think but this was a "want" rather than "need" purchase.

 

I went back and put some of my old PCB designs under the microscope and discovered several had a problem I reported in a previous blog - that is, the solder mask did not extend between the pins of smaller SMD packages.  This of course makes solder bridging and the resultant need for rework more likely.

 

I have had the problem occur for two reasons:

  1. The PCB manufactures had a minimum guaranteed spacing specification between the pad and the solder mask.  Check the specification especially with low cost prototyping services.
  2. I use KiCad and the default pad mask clearance is pretty high - so high that there is no mask between some SMD pins.  For KiCad the fix is to go into Dimensions -> Pad Mask Clearance while in pcbnew and change the default to the desired value.  OSHPark has a discussion on the topic and recommends 2 mil (0.05 mm) clearance for 2 layer boards.

 

The MSP430FR2xxx protoboard I put together a while back had the second problem and I did not realize it until I looked under the microscope.  They were made by OSH Park and it is hard to see the problem with the naked eye on that purple background.  Pesky default values....  I have reordered the board with the fix since they are inexpensive and I have another project in mind for that particular microcontroller.

Parents

  • Getting back to your original question, I think it's normal not to try putting soldermask between SMD pins of such a small pitch. That board looks fairly normal to me.

     

    I can't remember where I read it, but I'm fairly sure the recommendation is not to try mask between the pins as it tends to flake off. Any misalignment may also mean you could get soldermask on the pads. (I'm thinking of 0.5mm or 0.4mm pitch LQFP and QFN packages here)

     

    I'm now going to go search and see if I can find more info. If anyone else beats me to it feel free to correct me.

  • in reply to Fred27

    I think it's also very dependant on your PCB manufacturer. High end manufacturers are able to align the mask much more accurately and give a much finer minimum mask width. I took a look at a couple I use, Eurocircuits and Wurth. Here are links to their respective capabilities:

     

    https://www.eurocircuits.com/pcb-design-guidelines/

    https://www.we-online.com/web/en/index.php/show/media/04_leiterplatte/2011_2/relaunch/produkte_5/012012_Basic_Design_Guide.pdf

     

    So a couple of interesting things from these:

     

    Eurocircuits recommend you make your solder mask opening match exactly your pad size and then they will adjust the solder mask aperture as part of their processing to match the PCB pattern class. The thinnest solder mask segment they can create is 3.15mil which is pretty small. If your footprint pitch is such that the solder mask will end up less than this then they will automatically remove all the solder mask between these pads.

     

    Wurth's capabilities for solder mask are slightly better, they can do down to 2.75mil solder mask segments which would allow for extremely fine pitch parts to still have solder mask between the pads.

     

    I also had a quick look at PCB Way and Seeed Studio. PCB Way say they can do down to 4 mil for green and 6 mil for all other colours with their solder mask process and Seeed Studio say they can do down to 3 mil with their solder mask process.

     

    It would be interesting to get some small test boards with some fine pitch footprints built from some of these manufacturers (except Wurth as they only do whole panels, they are not a rapid prototyping PCB manufacturer) and see how they compare.

  • in reply to rachaelp

    With Seeed it is a bit hit or miss. They use different fabs, and these interpret the mask differently.

    In my case when the mask (defined within their limits) was running over copper fills, it was missing in one order, and correct in another order.

  • in reply to Jan Cumps

    That's a bit disappointing. They should either be consistent across their various fabs, assign designs to fabs which can actually build them as specified in their rules and depending on the difficulty of the board, or their rules should be such that they can be catered for at the fab of lowest capability. Did you raise this with them?

Comment
  • in reply to Jan Cumps

    That's a bit disappointing. They should either be consistent across their various fabs, assign designs to fabs which can actually build them as specified in their rules and depending on the difficulty of the board, or their rules should be such that they can be catered for at the fab of lowest capability. Did you raise this with them?

Children
No Data