Subject: | |
From: | |
Date: | Tue, 04 Jun 96 15:23:14 CST |
Content-Type: | text/plain |
Parts/Attachments: |
|
|
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.
|
|
|