Stats

  • Locked Locked
  • Replies 3
  • Subscribers 166
  • Views 18514
  • Members are here 0
More Content
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

SOLDER-MASK OPENING

GIRISH KUMAR

As per the IPC-7351B standard we will give Solder mask opening 1:1 , but there will be some special cases like fine pitch BGA or Mask bridge must between pads

 

where the pad of the type NSMD (SM is bigger than pad) or SMD type (SM is smaller than pad).When we have different type of mask opening requirement in Gerber will

 

it cause any issue for fabricator ? Will they do component level mask requirement check ? What is the general design consideration we should take care while sending Gerber

 

(Because I knew that few fabricator usually slightly increase the mask opening of all pads to control the SM registration tolerance.)

Any suggestions on this in generic not specific to particular fab. house ?

  • SevenFortyOneB

    You could make all of your solder mask clearances larger than the pads for NSMD pads and 1:1 for SMD pads and then add a note in your drawing that restricts the PCB fabricator from editing anything on the solder mask layers without permission.  This will probably result in the fabricator stopping the job and calling to ask permission to modify something unless you have a very good understanding of their solder mask process limits.

    Another option might be to make all clearances 1:1 and then add notes to your drawing forbidding edits to certain areas, components, or clearance sizes where you have SMD pads or otherwise want a specific solder mask clearance size.  Another note stating that bridging is not allowed in certain areas may also be appropriate.

    In my experience, PCB fabricators don't check for the type of component before adjusting solder masks.  They base their decisions on DFM/DRC checks that deal with manufacturability issues like overlap, bridging, and clearance annular ring. 

    PCB fabricators may not realize (or care) that making slight changes to the solder mask to improve manufacturability of the PCB could cause problems at the assembly stage.  Sometimes a drawing note is the best way to convey this type of information / requirement to them.   

     

     

     

     

     

  • GIRISH KUMAR
    Thanks for the detailed explanation. Regards,GK
  • ScottCad
    I think putting your gerber soldermask layer out as 1:1 does not give you much margin with the board house to control your design. I never ever do that because at the board level you also need to consider DFM, I have found some board houses will cut corners if they can. In particular with the soldermask on fine pitch land patterns. Best thing is to ask the board house what is the minimum web width they can achieve between lands so as to get an idea of how capable they are. You also want to specify the actual Soldermask type and color on your fab drawing, add a a couple of notes like. Soldermask should not bleed onto any exposed pad. Soldermask must be concentric with lands to +/- 4 mils etc. Soldermask modification is not permitted without contacting us first. Scott
Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.