Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Is solder mask metal?

Status
Not open for further replies.

liletian

Full Member level 6
Joined
Mar 5, 2008
Messages
337
Helped
2
Reputation
4
Reaction score
2
Trophy points
1,298
Activity points
3,790
I have a question. Is solder mask metal?
In this link

for the chip package, it looks like the solder mask is really close(figure solder_mask(.stc).png in the attached file. I am pretty sure the distance between top mental is enough (topmetal(.cmp).png) in the attached file. I am not sure if solder mask means metal or not. If it is metal, it might cause problem when I solder down the chip. I believe the solder mask layer comes from the tstop layer (29) in my design.
Can anyone help on this?
Thank you
 

Attachments

  • solder_mask(.stc).png
    solder_mask(.stc).png
    3.1 KB · Views: 90
  • top_metal(.cmp).png
    top_metal(.cmp).png
    11.6 KB · Views: 86
Last edited:

Solder mask is not metal. It is a 'solder resist'. I prevents short circuits due to solder bridging from one pad to another.

Keith
 

Solder mask is not metal. It is a 'solder resist'. I prevents short circuits due to solder bridging from one pad to another.

Keith

SO what will be the real pad size in the attached files.
the real metal size or the solder mask size?
In other words, the black pad at solder_mask(.stc).png or the real metal size at top_metal(.cmp).png in the attached file.
 

Attachments

  • solder_mask(.stc).png
    solder_mask(.stc).png
    3.1 KB · Views: 94
  • top_metal(.cmp).png
    top_metal(.cmp).png
    11.6 KB · Views: 75

The pad size is always the meal size. The solder mask is showing the holes in the solder resist to allow soldering - usually slightly larger than the actual pad.

Keith
 
Thanks Keith
You are awesome.:)
 

I probably didn't make it clear that the solder mask is a negative layer - where something is drawn there is no solder mask.

I haven't commented on your pictures as they don't show up too well on my phone. That is also why I haven't replied to your private message - I haven't been able to look at the attachments yet.

Keith
 

I probably didn't make it clear that the solder mask is a negative layer - where something is drawn there is no solder mask.

I haven't commented on your pictures as they don't show up too well on my phone. That is also why I haven't replied to your private message - I haven't been able to look at the attachments yet.

Keith

Hi Keith
I got it from your previous post before this one.
Thank you very much and have a great weekend.
Bests
 

The solder mask illustrated above will cause problems when soldering. There isn't enough space between the pads solder mask to allow for a dam of solder resist between the component pins, this could cause soldering problems during manufacturing.
It is standard practice these days to supply solder resist data as a 1:1 with the corresponding pad size, then let the manufacturer open up the iopening to work with his processes with the caveat below, from my PCB manufacturing notes:
Solder resist (solder mask) is required on both external faces of the printed board, it shall meet the qualification/conformance IPC-SM-840 class H. Coverage, cure and adhesion shall be as defined in paragraphs 3.8.1 to 3.8.3 of IPC-6012, except that no encroachment of solder resist is allowed on any surface mount or ball grid lands, and that ALL pad patterns have solder resist slivers between individual pads. The height of the solder resist should not cause any mounting problems for surface mount components.
Solder resist data is provided as per IPC-7351 standard, 1:1 with the land size, the manufacturer is to oversize these solder resist openings commensurate with their manufacturing procedures ensuring that ALL the above requirements are met, the amount of oversize to take into account the minimum track and gap dimensions as shown on the Printed Boards Master Drawing. Solder resist not related to a component pad is not to be enlarged.
 
Can anyone else comment on this ? Kind get confused from previous post.
Thanks a lot
If there does have a problem ,how can I fix it ?
Thanks a lot
 

If you look at the solder mask artwork, the pads are almost touching, you cannot get a solder mask sliver between two pads that thin, the PCB manufacturer will more than likely make a block so the mask clears all pads, thus you may get solder bridges during soldering. They are callewd solder mask dams bec ause they stop the solder flooding to the next pad.
Some pretty pictures.
**broken link removed**
 

So what will be an enough distant and how I can solve the problem ?
Thanks


The solder mask illustrated above will cause problems when soldering. There isn't enough space between the pads solder mask to allow for a dam of solder resist between the component pins, this could cause soldering problems during manufacturing.
It is standard practice these days to supply solder resist data as a 1:1 with the corresponding pad size, then let the manufacturer open up the iopening to work with his processes with the caveat below, from my PCB manufacturing notes:
Solder resist (solder mask) is required on both external faces of the printed board, it shall meet the qualification/conformance IPC-SM-840 class H. Coverage, cure and adhesion shall be as defined in paragraphs 3.8.1 to 3.8.3 of IPC-6012, except that no encroachment of solder resist is allowed on any surface mount or ball grid lands, and that ALL pad patterns have solder resist slivers between individual pads. The height of the solder resist should not cause any mounting problems for surface mount components.
Solder resist data is provided as per IPC-7351 standard, 1:1 with the land size, the manufacturer is to oversize these solder resist openings commensurate with their manufacturing procedures ensuring that ALL the above requirements are met, the amount of oversize to take into account the minimum track and gap dimensions as shown on the Printed Boards Master Drawing. Solder resist not related to a component pad is not to be enlarged.
 

Provide the soldermask openeing as a 1:1, same size as the component pad and use the blue text as a manufacturing instruction.
Also look at page 13.1 below
**broken link removed**
 

I believe you use Eagle? If so go to the DRC and find the MASKS tab. Change the STOP min & max to zero. They are probably set to something 0.1mm oversize at the moment. That is OK for large components but not for things like fine pitch TQFP devices.

Keith.
 

should be the soldermask opening a little bigger than actual pad size?
what is a blue text?
thank you very much for pointing this out, I really appreciate it.
Provide the soldermask openeing as a 1:1, same size as the component pad and use the blue text as a manufacturing instruction.
Also look at page 13.1 below
**broken link removed**
 

yes, it is 0.1 mm right now. after I set them to 0 mm, the mask in QFN does go to zero. However, in other place, the tstop layer seems to be crazy as attached. They generate some weird overlaps.
Thanks,

I believe you use Eagle? If so go to the DRC and find the MASKS tab. Change the STOP min & max to zero. They are probably set to something 0.1mm oversize at the moment. That is OK for large components but not for things like fine pitch TQFP devices.

Keith.
 

Attachments

  • tstop.png
    tstop.png
    42.8 KB · Views: 79

Are you sure they are all tStop layer? Turn off all layers except tStop.

Keith.
 

yes, there are.
the attched document are after I turn off all the layer except tstop.
the DRC reports a lot of tstop error, that is how I found out the overlap.
Thanks
Are you sure they are all tStop layer? Turn off all layers except tStop.

Keith.
 

Attachments

  • tstop2.png
    tstop2.png
    19.2 KB · Views: 78
  • tstop.png
    tstop.png
    24.7 KB · Views: 74

Hi Marce
Thank you very much for pointing this problem out. I really appreciate it.
Bests,
Bo
The solder mask illustrated above will cause problems when soldering. There isn't enough space between the pads solder mask to allow for a dam of solder resist between the component pins, this could cause soldering problems during manufacturing.
It is standard practice these days to supply solder resist data as a 1:1 with the corresponding pad size, then let the manufacturer open up the iopening to work with his processes with the caveat below, from my PCB manufacturing notes:
Solder resist (solder mask) is required on both external faces of the printed board, it shall meet the qualification/conformance IPC-SM-840 class H. Coverage, cure and adhesion shall be as defined in paragraphs 3.8.1 to 3.8.3 of IPC-6012, except that no encroachment of solder resist is allowed on any surface mount or ball grid lands, and that ALL pad patterns have solder resist slivers between individual pads. The height of the solder resist should not cause any mounting problems for surface mount components.
Solder resist data is provided as per IPC-7351 standard, 1:1 with the land size, the manufacturer is to oversize these solder resist openings commensurate with their manufacturing procedures ensuring that ALL the above requirements are met, the amount of oversize to take into account the minimum track and gap dimensions as shown on the Printed Boards Master Drawing. Solder resist not related to a component pad is not to be enlarged.
 

Thanks all of you's help. Especially Keith and Marce. I really appreciate it. FInally my solder mask looks like this:

It should be ok.
Thank you for all helps and comments.
 

Attachments

  • soldermask.bmp
    299.8 KB · Views: 74

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top