Re: PCB / fabrication print



On 13 Oct 2006 07:07:33 -0700, J.Wankenhorst@xxxxxxx wrote:

Hello NG,

i want send my PCB design to a manufacturer; i am new to pcb
prototyping and that is why i have a question: How can i make a
frabrication print?
The manufacturer's website (www.pcbfabexpress.com) says the following:
- Make sure Fabrication Print is provided and it is not missing any of
the following:
» Material type and finished thickness of the board
For general purpose work, you can use FR4. They don't actually use FR4
anymore, but the description will tell them to use the "standard"
grade board material. 0.0625" (1.6mm) is a common thickness. Other
less common board thicknesses are 0.031" and 0.093".

» Finished copper weight
This is the thickness of the copper given in ounces/square foot. 1
ounce, or about 0.0012 to 0.0014", is common. For lots of small traces
(smaller than 5 mil wide, 5 mil spacing) closely spaced, 0.5 ounce.
For power circuitry, 1.5 to 4 oz.

» Board dimensions and outline
This is the outline of your board edge. I put this info on the drill
drawing. If the outline is complicated or I need the board put into a
panel, I'll make a separate drawing with all useful dimensions in a 2D
CAD program like AutoCad and include that drawing as a PDF. Of course,
if you have a complicated board outline, I usually do the board
outline in a 2D CAD program and export the board outline to the PCB
layout program.

» Cut outs or slots information (if cutouts & slots are allowed in
the product you are buying; check
the product specs)
Some boards have material removed from the center portion. This can be
shown in the drawing showing board outline

» Board Construction information
You need to tell the board house the order of the layers, what
material to use, copper thickness, buried and blind via layer
associations, board material type, and anything else that is
pertinent.

Do you know what software i an use for that? For the design of my board
i used EAGLE from Cadsoft.
You should be able to put all information about your board using
Eagle. If you need to supply an additional 2D drawing, use any 2D
drafting package and include that drawing as a PDF.

Also, how can i find out my copper weight and do you know what exactly
is meant by outline?
Or can somebody point me to an example?

Best regards and thanks in advance, Juergen

It is customary to only have an even number of layers as this reduces
manufacturing costs for the board house. If you have an odd number of
layers, think about duplicating a ground layer to make it even.

A simple board submission will include the following files:
1. Gerber files (files with trace and pad info for each layer)

2. Excellon drill file(s) (drill hole file)

3. Readme file with your contact info, descriptions of each file in
your submission to the board house, board details (copper thickness,
board thickness, board material, layer order, number of layers, number
of drill holes, number of different hole sizes, special instructions,
etc).

Pack everything up in a ZIP file.

You may find this web site of interest:
http://www.pcbpro.com/pcb-glossary.php

---
Mark

.