Soldermask between component pads

[Henrik Olesen]

Hi

Our production asks us to remove soldermask between component pads
especially on fine pitch components.
Does any of you have any experiences, good or bad, with this?
The engineers in my department are especially concerned about migration if
we remove the mask.

Regards
Henrik Olesen
Kamstrup A/S
Denmark

-END-
SupportNet: http://www.mentor.com/supportnet
To unsubscribe send a blank email to: leave-ta...@listserver.pads.com
For assistance please send mail to talkli...@mentor.com

[Denis Lefebvre]

Your engineers concern is a valid one. When we considered this issue we
decided, for 0.5mm pitch devices, that we'd provide a min solder mask
web of 0.1mm between the lands. This meant doing some tweeking in our
'standard' pad & oversize to accomplish it, but it seems to be working.
So the numbers look like this:
Solder Mask pad = 0.4mm wide. (normally would be 0.45)
Solder Land = 0.28mm (normally would be 0.30)

Denis Lefebvre, CID+
Sr. PCB Designer
Finisar Corporation
(408)542-3832

-----Original Message-----
From: Henrik Olesen" <h...@kamstrup.dk> [mailto:ta...@listserver.pads.com]

Sent: Thursday, October 16, 2008 6:29 AM
To: Talk Mailing List
Subject: Soldermask between component pads

[mkennedy]

If the web is going to be less than 3-4mils then yes it makes sense to remove the masking in that pin area, other wise the webbing can migrate into the pad area and cause soldering issues, and possible carry solder over to adjacement pins, causing shorts and bridges. That's why there is a copper wieght limit on fine fine pitch devices. So the pads are nice and tight, and you hope your CM or in-house, have good manufacturing processes.

 

Matthew Kennedy

Sr. PCB Designer C.I.D.

Sedona Pads

Work: 603.546.0106 x218

Cell:   781.307.1030

 

---

From: Denis Lefebvre [mailto:ta...@listserver.pads.com]
Sent: Thursday, October 16, 2008 9:38 AM
To: Talk Mailing List
Subject: RE: Soldermask between component pads

No virus found in this incoming message.
Checked by AVG - http://www.avg.com
Version: 8.0.173 / Virus Database: 270.8.1/1728 - Release Date: 10/16/2008 7:38 AM

[Klaus Bak]

Hi Henrik

We have removed soldermask between SMT pads on fine pitch components for many years now.
I haven't heard of any problems.
But I guess the reflow soldering process becomes more critical.

Anyway - you won't be able to have soldermask between SMT pads on the smallest packages.

Regards
Klaus Bak
Grundfos A/S. -END- SupportNet: http://www.mentor.com/supportnet To unsubscribe send a blank email to: leave-ta...@listserver.pads.com For assistance please send mail to talkli...@mentor.com

[Robert Kondner]

Hi,

I would think production would WANT solder mask between fine pitch leads
though that can be difficult. Even at .5mm pitch a .2mm wide pad only leaves
.3 for mask plus alignment. If you allow .1mm for alignment you have only
.1mm left for mask. A .2mm wide pad is very thin, paste release will be
difficult. All these numbers are very tight.

If you really want to eliminate mask you could increase the pad oversize
some.

Can anyone tell me:

If you put solder mask copper into the top mask layer of a DECAL does that
mask copper get swapped to the correct layer when the decal is flipped to
the bottom side?

Bob Kondner

-----Original Message-----
From: "Henrik Olesen" <h...@kamstrup.dk> [mailto:ta...@listserver.pads.com]
Sent: Thursday, October 16, 2008 9:29 AM
To: Talk Mailing List
Subject: Soldermask between component pads

Hi

Our production asks us to remove soldermask between component pads
especially on fine pitch components.
Does any of you have any experiences, good or bad, with this?
The engineers in my department are especially concerned about migration if
we remove the mask.

Regards
Henrik Olesen
Kamstrup A/S
Denmark

-END-

[George Defond]

Yes, it flips to the bottom mask when the part is flipped.

George Defond, PCB Designer
David Clark Co. Inc.
PO Box 15054
Worcester MA 01615
(508) 751-5800 x333
gdefond at davidclark dot com

-----Original Message-----
From: Robert Kondner [mailto:ta...@listserver.pads.com]
Sent: Thursday, October 16, 2008 9:58 AM
To: Talk Mailing List

Subject: RE: Soldermask between component pads

[Les Embrey]

I have done some fine pitched and even bgas with no solder mask on the parts between the pads.
It is really up to your Fab house wither or not  you can put it down.
My concern is ROHS as I have not much experience with it and solder masks.
Again Talk to your Fab house if they will not talk to you about what they can or can not do
Find a better house

--
Electrical Designer
Smithsonian Astrophysical Observatory
Central Engineering
100 Acorn Park Drive
Cambridge Ma. 02140
PH 617-384-9332
lem...@cfa.harvard.edu
http://www.cfa.harvard.edu

[Hawker <hawker@ashevillecommunity.org>]

This is one of the areas I have issues with the new IPC decal spec (over
the old one). If you follow IPC for .5mm pitch TQFPs there isn't enough
room for solder mask between pins or the mask is so thin it comes up
into the pads and causes connectivity issues.
If you remove it we have had yield issues with pin to pin shorts.
So we do what someone else said. We tweak the pin width down so that we
can still get some solder mask between pins. I forget the numbers off
the top of my head. Would have to re-visit decals.

Hawker

[John Matthews]

There are cases where the manufacturing process simply can't give you a soldermask dam between pads. This is, as someone said, usually on very fine pitch devices (pretty much limited to some connectors and ICs). It has gotten better than it used to be, but can still be a problem, especially if you go "cheap" for fab. I can't find my process engineer to verify this, but I think the minimum line size for mask is about 3 mils...

We have done ganged opening with pretty good success in the past. The main thing is to have an assembler with a good quality process in place.

And yes, the associated copper should flip sides...

JM

Robert Kondner wrote:

Hi,

  I would think production would WANT solder mask between fine pitch leads
though that can be difficult. Even at .5mm pitch a .2mm wide pad only leaves
.3 for mask plus alignment. If you allow .1mm for alignment you have only
.1mm left for mask. A .2mm wide pad is very thin, paste release will be
difficult. All these numbers are very tight.

  If you really want to eliminate mask you could increase the pad oversize
some. 

  Can anyone tell me:

 If you put solder mask copper into the top mask layer of a DECAL does that
mask copper get swapped to the correct layer when the decal is flipped to
the bottom side?

Bob Kondner


-----Original Message-----
From: "Henrik Olesen" <h...@kamstrup.dk> [mailto:ta...@listserver.pads.com

] 
Sent: Thursday, October 16, 2008 9:29 AM
To: Talk Mailing List
Subject: Soldermask between component pads

Hi

Our production asks us to remove soldermask between component pads 
especially on fine pitch components.
Does any of you have any experiences, good or bad, with this?
The engineers in my department are especially concerned about migration if 
we remove the mask.

Regards
Henrik Olesen
Kamstrup A/S
Denmark 



-END-
SupportNet:  http://www.mentor.com/supportnet

To unsubscribe send a blank email to: leave-ta...@listserver.pads.com
For assistance please send mail to talkli...@mentor.com


-END-
SupportNet:  http://www.mentor.com/supportnet
To unsubscribe send a blank email to: leave-ta...@listserver.pads.com
For assistance please send mail to talkli...@mentor.com

  

-- 
John Matthews
Silicon Hills Design
8504 Cross Park Drive
Austin, Texas 78754

512.836.1088 x1108

[John Matthews]

Actually I should have said "with VERY good results in the past".

You do need to maximize the spacing between pads on the device. We normally will make the pad width the nominal width of the lead, concentrating on getting a good solder joint at the heel and toe of the leads.

JM

John Matthews wrote:

We have done ganged opening with pretty good success in the past. The main thing is to have an assembler with a good quality process in place.

[John Matthews]

Found my process engineer, soldermask needs 3-5 mils width, depending on the quality of the fab house, to adhere properly. Below that, you can get smearing, or the little pieces of mask can come loose from the board, possibly falling completely or partially onto a solder pad, which is bad.

JM

[ta...@listserver.pads.com]

Hi Henrik,
We are starting to run into this problem here. The boards we use here
are all IPC-6012 class 3 which means the fabrication tolerances are
fairly tight. Our board house has to hold a .038 mm to .051 mm clearance
between the edge of the pad and the edge of the Soldermask opening. This
allows us to go down to a .076-.10 mm wide solder mask web between
adjacent pins. I would say that you should check with your PWB supplier
and see what he says.
Like someone else said, "It might be complicated, but at least it's
expensive".
Dave Connitt CID+
Printed Circuit Designer
KDI Precision Products, Inc.
A Wholly Owned Subsidiary of:
L3 Communications
3975 McMann Road
Cincinnati, Ohio 45245
Ph. 513- 943-2010 Fax 513-943-2288

-----Original Message-----
From: Henrik Olesen" <h...@kamstrup.dk> [mailto:ta...@listserver.pads.com]

Sent: Thursday, October 16, 2008 9:29 AM
To: Talk Mailing List
Subject: Soldermask between component pads

Hi

Our production asks us to remove soldermask between component pads
especially on fine pitch components.
Does any of you have any experiences, good or bad, with this?
The engineers in my department are especially concerned about migration
if we remove the mask.

Regards
Henrik Olesen
Kamstrup A/S
Denmark

-END-