If you're trying to control impedances and PCB thickness across multiple layers, the best solution is to describe your constraints to any good fab house and ask them what they recommend. Note that fab houses can usually adjust trace widths fairly easily but adjusting center-to-center spacing is not something they do easily, if at all. Therefore, on differential traces you need to use a distinct trace width. For example, you can tell the board house which layers contain differential pairs, that you want to run them on 0.25mm, or 0.3mm center-to-center spacing with a minimum line-to-line clearance of .15mm, and that the differential impedance needs to be 62 Ohms. Then ask them what layer stackup, trace width, and center-to-center spacing they recommend. They will come back to you with a good approach. Then in the documentation give them the flexibility to adjust differential trace widths, identify the differential traces by a distinct width, tell them that width, and give them the responsibility of matching the differential impedance spec.

If you are not matching any impedances, you are still better off asking them what stackup they would recommend, because you may not know what brands of material they use or regularly stock.

Jeff Condit

----- Original Message ----- From: "H. Selfridge" <[EMAIL PROTECTED]>
To: "Protel EDA Forum" <[EMAIL PROTECTED]>
Sent: Sunday, October 03, 2004 1:04 PM

The standard thickness of core material depends on who makes the laminates used by your fab.

If your fab can't make the board to your required dimensions, you need to call around and see what other fabs can get/do.

An example of available material from one laminate manufacturer can be seen at:
A table of available laminates can be seen in design guidelines from a fab at:

Finished thickness for prepreg and some cores can be different from the raw thickness as supplied. When heated and pressed in the laminating press, some reduction in thickness of the individual layers tends to occur. The data sheet from the laminate manufacturer gives the raw and finished thicknesses. Again, the best source of information is from the fab. If you're controlling impedance, the finished thickness data is essential for modeling stripline and microstrip characteristics.

At 11:56 AM 10/3/04, you wrote:

is there a table of standard core thicknesses somewhere?

i have a 6 layer stackup


and am trying to hit 062" overall thickness within +-005

what are all the material thickness possibilities out there?
(well maybe not ALL of them :) )

given 007 prepreg and 021 cores
my vendor tells me that once you add the copper thickness at 1oz
the overall is about 071" thick

sounds like 017 cores would do it, but that also sounds like a wierd number

thanks for any help

Dennis Saputelli

-- _______________________________________________________________________ Integrated Controls, Inc. Tel: 415-647-0480 EXT 107 2851 21st Street Fax: 415-647-3003 San Francisco, CA 94110 www.integratedcontrolsinc.com

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to