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.