PCB / fabrication print

[[email protected]]

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
» Finished copper weight
» Board dimensions and outline
» Cut outs or slots information (if cutouts & slots are allowed in
the product you are buying; check
the product specs)
» Board Construction information
Do you know what software i an use for that? For the design of my board
i used EAGLE from Cadsoft.
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

 

[Peter Bennett]

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:

Sounds like the "readme" text file that I send with my board orders.

» Material type and finished thickness of the board

Usually FR-4, 1/16" nominal thickness

» Finished copper weight Usually 1 ounce
» Board dimensions and outline

I put the board outline (the actual shape of the finished board) on
all layers as a .005" track

» Cut outs or slots information (if cutouts & slots are allowed in
the product you are buying; check
the product specs)
» Board Construction information
Do you know what software i an use for that? For the design of my board
i used EAGLE from Cadsoft.
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

My usual "readme" files look something like this:
===============================

<my name and company info>
<purchase order number>

Job: 0929-3 Modular Motor Driver
PC Board P-13162

The following files are required for this job:
p13162.GTL Component side copper photoplot file
p13162.GBL Solder side copper photoplot file
p13162.GTO Component layout silkscreen
p13162.GTS Top Solder Mask
p13162.TXT Drill file
readme.txt This file


Note: the Gerber files include embedded aperture data.

Drill Information
Tool Hole Size Hole Count Plated Tool Travel
---------------------------------------------------------------------------
T1 28mil (0.7112mm) 57 45.83 Inch
T2 35mil (0.889mm) 234 59.37 Inch
T3 55mil (1.397mm) 10 12.06 Inch
T4 63mil (1.6002mm) 15 15.61 Inch
T5 110mil (2.794mm) 4 21.67 Inch
T6 125mil (3.175mm) 8 14.71 Inch
---------------------------------------------------------------------------
Totals 328 169.25 Inch
(4298.82 mm)


The board is approximately 8.8 x 3.94 inches, double-side,
..0625" nominal thickness, FR-4 material
1 oz or greater copper
Standard through-hole plating, standard tin-lead plating on exposed
copper.

Solder mask both sides
Component Ident silkscreen on component side


Trim boards to outline on component side artwork

Please make at least 20 boards.

=============================

 

[JeffM]

How can i make a [fabrication] print?
i used EAGLE from Cadsoft.
Juergen

All the data required is embedded in the various layers of the Layout
file.
This is translated into Gerber and Excellon by the CAM Processor.

how can i find out my copper weight
and do you know what exactly is meant by outline?

If you haven't read David L. Jones' 25-page PDF yet,
now would be a good time:
http://groups.google.com/group/sci....-package-*-*-included-it-in-their-Help-system

A previous thread related to this:
http://groups.google.com/group/sci....abrication-Information+Warp-*-twist+checklist

 

[qrk]

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