JoAnn A., Scott D. and John S.,
     
     Scott is on the right track; the hole needs to be drilled oversize to 
     allow for reduction after copper plating and solder coating.  One 
     exception, in my "guideline" the "drill size adder" is applied (added) 
     to the NOMINAL finished plated through hole size, not the MAXIMUM as 
     IPC-D-275 implies.  
     
     In my original "guideline" posting response, I defined "D" as "Drill 
     size, typically 0.004-0.006" larger than NOMINAL finished hole size; 
     accounts for the reduction in hole size after plating...".  

     I'll add two other "guideline" comments:
     1) Typical hole size tolerance for component holes (copper plated and 
        solder coated) is usually +/-.0.003", once in awhile we'll see 
        +0.003/-0.002" or +0.002/-0.003"tolerance; and,
     2) Via hole size tolerance that most board fabricators typically request is
        "nominal +0.003"/-nominal.  Thus, if the print specifies the nominal 
        finished via hole size to be .012", the requested tolerance would be 
        +0.003/-0.012". The reason for the low end tolerance of "- nominal" is 
        that the hot air solder leveling (HASL) process can't assure all holes 
        below 0.015" dia. will be cleared of solder 100% of the time.     

     As fundamental as it may seem, the #1 deviation request that board  
     fabricators ask for is an increase in the pad sizes associated with 
     component and via holes.   

     Regards, Dave Wolf
______________________________ Reply Separator _________________________________
Subject: Re: [DC] Hole size calculations
Author:  Scott Decker <[log in to unmask]> at SMTPLink-Hadco
Date:    4/24/98 6:10 AM

JoAnn Amerson wrote:
     
> > From:          [log in to unmask]
> >
> >      Example:  Assume finished plated through hole size of 0.034+/-0.003"; 
> >                minimum annular ring requirement of 0.002"; and, FA = 0.014" 
> >
> >      Therefore:  P = (0.034 + 0.005) + 0.014 + 2(0.002) = 0.057" 
> >
> >
> >      Using the information from the above example, I would answer your 
> >      questions as follows:
> >
> >      #1  Maximum finished hole size = 0.034 + 0.003 = 0.037 
> >
> >      #2  Value to add to nominal hole size = 0.005 + 0.014 + 0.004 = 0.023 
>
> This thread is of interest to me.  We don't use a standard formula here  
> but I would like to try to have one.  One of my responsibilities is to   
> develop a "guideline" (the word "standard" isn't allowed) on creating 
> component footprints.  Right now I can't justify the pad sizes we are 
> using.  If I had a formula I could start using that and feel beter about 
> the numbers I come up with.
>
> I was doing fine with Mr. Wolf's explanation until he popped in real 
> numbers.  He started with .034±.003".  Then he states P = (0.034 +
> 0.005) Where did that .005 come from?  Or was that a typo? 
>
> Anyone care to help me?  I know it's early, and it's Friday, but
> surely someone has a few brains cells they can show off this morning. 
>
> TIA,
> Jo
>
     --------------------------------------------
 JoAnn,
  The drill hole size number that was mentioned, (.005") is what most board
manufactures use as an oversize amount. You have to drill the hole larger than 
the finished size to account for plating. This .005" is .0025 on each side and 
when they plate .001" or so in the hole, presto a finished hole size of
what you specified... One thing you do have to take into consideration is that 
this .005" should be from the plus side of your tolerance. If the hole is .035 
+/- .003 the drilled hole at the board shop will be .038 + .005 = .0043. Your 
pad size needs to be able to handle this oversize for the annular ring.
Dang.... I was trying to post this to the group but I hate Netscape 4.XXX..... I
hope this helps in you quest for a stand..... I mean GUIDELINE at your place..
     
         Scott Decker

################################################################
DesignerCouncil E-Mail Forum provided as a free service by IPC using LISTSERV 1.8c
################################################################
To subscribe/unsubscribe, send a message to [log in to unmask] with following text in the body:
To subscribe:   SUBSCRIBE DesignerCouncil <your full name>
To unsubscribe:   SIGNOFF DesignerCouncil
################################################################
Please visit IPC web site (http://jefry.ipc.org/forum.htm) for additional information.
For the technical support contact Dmitriy Sklyar at [log in to unmask] or 847-509-9700 ext.311
################################################################