Group Actions
Engagement
  • Author Author: fmilburn
  • Date Created: Date Created
  • Views 2028 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.

  • in reply to Fred27

    Very interesting conversation.  I have an order in on the board photographed above which will meet OSH Park specs and has soldermask between pins.  It is a small sample from one manufacturer so I won’t learn anything about variability but I will be checking from now on.  I also want to see how much difference it makes in reducing rework. 

  • in reply to rachaelp

    Just to add to that, from the proto services in China, I believe (not sure) that the 4-layer boards could be made to slightly better specs than they mention.

    Also another point is that if the rules are slightly exceeded, some boards may be better quality than others, i.e. since they tend to supply ten PCBs instead of just (say) three, then there is a chance that some of the boards in that set of 10 will be better than others. For instance perhaps around 3 mil width may be possible, but not if there is too much misalignment.

    I used that to my advantage when working with a 0.4mm pitch connector. A few of the boards had solder mask between the pads. Others had it damaged slightly due to misalignment of the solder mask to the copper, causing the very narrow width solder mask to have broken. Since I only needed a few prototypes, I selected the best boards out of the ten.

     

    With 0.5mm pitch components or higher, I've never had an issue with solder mask between pads, all the low-cost PCB services I have tried (PCBway, Elecrow and iTead) have managed it.

     

    The more expensive Europe PCB prototype services almost precisely align the masks as I understand. I've only used PCBtrain in the UK, and they aligned extremely well (to be expected, it is a factory that does super-high-end boards). But the cost is a huge difference to the China PCB prototype services.

  • 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?

  • 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 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.