I'm not sure if I read your sketch correctly, but the problem seems to 
     be that the drawing is giving contradictory requirements.  The spacing 
     specified does not include copper.  When you include the copper 
     thickness and the thickness between layers specified in the drawing 
     then the board is too thick. 
     
     The sketch also does not include any tolerances on copper thickness or 
     the seperations between layers.  The overall thickness and tolerances 
     however seems very clear.  The PCB supplier should have flagged the 
     inconsitancies to you before taking the job.  If I was doing the 
     stackup I'd spec the copper thickness required on each layer and the 
     seperation between layers.  I generally leave the seperation between 
     the centermost layers reference only.  The overall thickness will 
     drive the center thickness.
     
     Typical thickness of 1 oz copper inner layers is 35 um.
     For outer layers suppliers typically start with 1/2 oz copper (18 um) 
     and plate additional copper on top of this.  Final outer layer copper 
     thicknesses is typically in the 55 um range.  Thus for a 4 layer 
     construction you would typcially have:
     
     
     Layer 1 copper:                    .055 mm
     Spacing between layer 1 & 2:       .600 mm
     Layer 2 copper:                    .035 mm
     Spacing between layer 2 & 3:       .400 mm
     Layer 3 copper:                    .035 mm
     Spacing between Layer 3 & 4:       .600 mm
     Layer 4 copper:                    .055 mm
     
     Total Nominal:                    1.780 mm 
     
     Obviously this is not what you desire overall.  
     
     The tolerance on overall thickness is usually +/- 10% of nominal.  For 
     example:
     
     1.55 +/- 0.15mm  is a typical overall thickness tolerance for your 
     nominal you desire.
     
     Tighter tolerances such as 1.55 +/- .05mm (or +/- 3% overall 
     thickness) is not practical for production, and will be very expensive 
     if possible at all.
     
     Making a stackup for a PCB isn't straightforward.  You need inputs 
     from  your mechanical designers as to what thickness works to plug the 
     board in a system. You need inputs from your electrical people 
     regarding mininum copper thickesses needed to carry current and target 
     impedance (if applicable) for your stackup.  You need your fabricator 
     to tell you what is possible.  There are a lot of variables here, 
     dielectric seperation, copper weight (thickness), trace width, 
     impedance, etc.  A good PCB shop can help you do this. 
     
     Hope this helps.
     
     Regards,
     
     [log in to unmask]
     
______________________________ Reply Separator _________________________________
Subject: Re: FAB: Fab Drawing misinterpretation..
Author:  [log in to unmask] at Dell_UNIX
Date:    6/4/96 2:12 PM


Dear Technet,
     
I am having big interpretation problem on the FAB drawing:-
     
Customer's Requirement :-
     
__________
|        |      preprag 0.6 mm
----------
__________
|        |      C.L.L 0.4mm
----------
__________
|        |      preprag 0.6 mm
----------
     
It stated on the drawing as:
a.      Thickness of copper foil is 35u 
b.      Thickness of PCB thickness is 1.5/1.6 mm
     
     
     
We end up getting an overall thickness of 1.7 to 1.77mm from our PCB supplier.
     
The PCB supplier come back with their side of the story, 
Supplier's interpretation is
     
----------                    -----   
|       |       35 u            ^
---------                       |      
                                |
|-------|                       |
|       |       70 u            |       
|-------|                       |
|       |                     overall thickness = 1.81 mm  
|       |                       |
|-------|                       |
|       |       70 u            |
|-------|                       |
                                |
---------                       |
|       |       35 u            v
---------                     -----
     
     
I would like to know whether the PCB supplier is right ?, and whar is the 
correct way
to interpret the drawing.
     
and also does anyone know of any spec/book that tell one how to interpret a FAB 
drawing ..
     
I'm appreaciate for any comment given .. Thanks.