Announcement

Collapse
No announcement yet.

Solder mask

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts

  • robertferanec
    replied
    I like mairomaster solution!

    Leave a comment:


  • oscargomezf
    commented on 's reply
    Ok thank you. I'm pretty sure you told me that in the course: "Schematic and PCB Design Course". But It has been a long time since I finished it, around two years (I have to review my notes) and I haven't the opportunity to design a real PCB.

  • mairomaster
    replied
    In such situations I often change the shape of the 4 corner pads to round instead of perfect (square) rectangle. That gives more clearance between the corners of the corner pads. I do that in the PCB library, since it will probably be an issue with every board.

    Leave a comment:


  • robertferanec
    commented on 's reply
    In critical places I make the solder mask expansion 1 mil (0.0254mm). That should fix your problem.

  • oscargomezf
    replied
    Hi,

    I've passed the design rules check and I've got this error in the 4 corners of my IC. I've set the MinimumSolderMaskSliver = 0.08mm and Solder Maks Expansion = 0.06mm.

    What do you think it's the better option to solve this issue? I can only modify the Solder Maks Expansion in this 4 pins... but I'm not sure if this is the best option.

    Best regards.
    Attached Files

    Leave a comment:


  • robertferanec
    replied
    I mask the vias too.

    Once we had problems with unmasked VIAs under BGA (it may create short circuits). Also when I had a PCB with unmasked VIAs, I had to be extremely careful when working with PCB - even a little bit of tin could make short circuit on PCB (especially dangerous when re-working stuff and when you place your board on the table where you normally solder)

    Leave a comment:


  • mairomaster
    replied
    I prefer tenting (covering) my vias, since this is better in terms of solder mask violations and also silk screen text over such vias looks a bit better. If you need to use some vias as test points for debugging, it is easy to scrape the solder mask off them. I am not really sure what is the advantage (if any) to have the vias uncovered.

    Leave a comment:


  • oscargomezf
    replied
    Sorry, I've got another concern.

    The parameter solder mask expansion for through hole vias have to be 0.05 too or, Is it better cover it with solder mask?

    Best regards.

    Leave a comment:


  • oscargomezf
    commented on 's reply
    Thank you, I see what you mean.

  • mairomaster
    replied
    Yes, you have to verify with the manufacturer what is the minimum value you can use. Normally is in the range 0.05 - 0.15 mm. If you have those error, probably you have pads too close together (either in different components or the same component) which leave too little solder mask between them. This little solder mask bridge (sliver) might break during production which increases the chance of solder bridges between pads.

    Leave a comment:


  • oscargomezf
    replied
    Hi everyone,

    Now I have a lot of errors related to MinimumSolderMaskSliver [I've got this parameter set to 0.08 mm], But this parameter depends on the manufacturer, doesn't It?

    Best regards.

    Leave a comment:


  • oscargomezf
    commented on 's reply
    Thak you very much, @mariomaster.

  • robertferanec
    replied
    we also leave paste expansion 0

    Leave a comment:


  • mairomaster
    replied
    I always leave the paste mask expansion to 0. The manufacturers can adjust that themselves.

    Leave a comment:


  • oscargomezf
    commented on 's reply
    Thank you robertferanec. I have no reason for considering no use solder mask. I thought it was better, but I don't have any problem to add 0.05mm. I've design all my footprints with soller mask expansion from rules, so it's easy to add solder mask.

    Does paste mask expansion has to be zero?

    Best regards
Working...
X