1) We typically process with .002/side soldermask clearances. We will 
     go to .0015/side if the design requires it, and the Customer will not 
     let us change to block clearances.
     
     2) We can only maintain webs of .005 and greater. 
     
     And yes we will modify the soldermask clearance to .0015/side to 
     achieve the .005 webs.
     
     
     Ray


______________________________ Reply Separator _________________________________
Subject: FAB: Soldermask Clearance and Web Width requirements 
Author:  [log in to unmask] at SMTPLINK-HADCO
Date:    5/13/96 1:42 PM


     Designing soldermask webs is always a pain in the neck, particularly 
     for fine pitch.  
     
     I'd like to conduct an informal survey, supplementing Doug's excellent 
     questions below regarding soldermask:
     
        1.  Using LPI type masks what is the minimum nominal clearance 
     (Copper to soldermask) that PCB fabricators need to prevent soldermask 
     from encroaching onto the copper?  I've got answers in the past 
     ranging from 2 mils to 5 mils.
     
        2.  What is the minium nominal soldermask design web width that can 
     maintained in production?   I.E. a minimum width that I can expect to 
     still have a soldermask web remaining after processing.  I've got 
     answers here in the past also from 2 - 5 mils.
     
     Need both answers from as many fabricators as possible.
     
     I am looking for a number suitable for volume production (i.e. >10K  
     panels per month).
     
     Does a table exist in any IPC design guidelines indicating these 
     geometries?
     
     Is it typical practice for PCB fabricators to modify soldermask 
     artwork to get the necessary clearance?
     
     Thanks,
     
     [log in to unmask]
______________________________ Reply Separator _________________________________
Subject: FAB: Soldermask Webs.
Author:  [log in to unmask] at Dell_UNIX 
Date:    5/11/96 7:50 AM
     
     
-- [ From: Doug Jeffery * EMC.Ver #2.10P ] --
     
Friends,
     
We have seen many designs that have smaller webs between SMP's than they 
have circuits.  Imagin creating a .003" line in Soldermask yet the board 
has .006" traces.  We have found that any Soldermask web design that is 
.005" of web by design is reproducable and  can be placed reliably, but 
below .005" the LPI masks do no hold on.  
The key reason is undercut. The  LPI between SMP's is thicker than 
anywhere else on the board.  This requires that the exposure be set up 
to accomadate the thicker material, however overexposure can cause 
other feature problems.  After you have optimised the exposure you play 
with the developing until you keep a good dam between pads, Bingo you 
are leaving ink in the holes.   So,  you crank up the developer and get 
that ink out of the holes....Catch 22...
     
AT .005" feature size (dams) you are able to optimize the process, 
below .005" dams the undercut takes the foot of the LPI down to .003" 
or .002" which makes the adhesion a problem, hense the peelers and 
redoposit problems that you expressed.  
     
?What is the answer for .020" pitch devices that require .014" pad 
widths?
     
?what is the answer for .006" lands on .012" centers?
     
I don't know but certainly we have to get to one.  We have tried double 
coating, Unpigmented material, reduced pigmented material..No 
significant result differences.  We try to get customers to leave use 
.009" min space between SMP's to keep a dam (2/5/2 by design.  This 
makes LPI exposing a tighter regitration than our outerlayer 
requirements.