PCB Manufacturing Process with Eagle PCB
I'm using Eagle PCB for most of my PCB making. One user ask for one of my PCB design but the PCB manufacturer didn't accept native Eagle PCB files. Protel is the standard format in this industry.
Most if not all PCB manufacturers should accept Gerber file. Since Eagle PCB documentation is not complete on the subject of PCB manufacturing, or I didn't find it ;), I'll will list here my own findings on what you need to provide to have your PCB made using Eagle PCB. These steps should also apply to other PCB programs since the manufacturing process is the same.
This is a quick step by step guide. I hope you find it usefull.
Eagle PCB Making Process Files creation:
The complete process will create these Gerber layer files:
1) Top/Bottom/Silk Layers
2) Create Drill Rack Table file
3) NCDrill file (layer drill)
4) Solder Mask layers
Here each steps in more details:
1) Top/Bottom/Silk Layers___________________________
Create the Gerber files using the Cam Processor (see the Eagle menu /File/Cam Processor) using the output device <GERBER_RS274X> for the following layers:
Top & Bottom (Layers that include the via, pads & traces)
tPlace, bPlace (Top/Bottom Silk Screen layers)
2) Create Drill Rack Table file_________________________
For the holes, more steps are needed, you need to generate the NCDRILL file. A separate script program (see the /eagle/dru directory), called drillcfg.ulp, will generate a Rack Drills File. This text file will be used by the CNC machine to select automatically the needed drills during the PCB drilling process.
First with the PCB openned, execute the script /File/Run/drillcfg.ulp, to generate the file Drill_Rack.drl file
This text format file will contain a list of max 10 drills. The next step may generate a "Missing drill size" error if the pcb has more holes sizes, such as the mounting holes. To correct this fault, you may need to edit this file manually and add the missing drills.
T03 0.036in, etc...
3) Create the NCDrill file (layer drill)_____________________
Then using the Cam Processor, create the NCDRILL file, select:
-Layers: Drills (& Holes if you have mounting holes)
-Rack: Drill Rack.drl file created previously
This will create the NCDRILL.dri file.
Don't forget to include the rack file with this file. It may be needed.
The NCDRILL.dri file is a normal text file. You can look at it using Notepad. It is an interesting reading containing all the needed CNC programmation informations.
The NCDRILL file (no extension) is also a text file containing for each drill size, each X-Y coordinates for each hole to drill.
4) Create the Solder Mask layers___________________________
Solder Masks are created automatically, you don't need to draw them on the pcb.
Use the Cam Processor, Device <GERBER_RS274X>, then select one of these layer tStop or bStop and execute the processor. This will generate the solder mask files. The solder mask layers isolate spacing is defined into the Design Rules/Masks sub-menu. They are
Solder Mask: 4 mil and Cream Mask: 0 mil (see below)
SMD Auto Assembly Only____________________
If you need to have the PCB manufacturer to install automatically smd parts for you you will need to send 2 more layers. They are the cream and glue layers. The cream layer will be use to create a metallic sheet mask used during the cream (solder and flux paste) application. The glue mask is used to apply glue that will hold the smd part during the part auto insertion process, before the soldering. These layers names are:
tCream,bCream Solder cream
tGlue,bGlue Glue mask
Good PCB manufacturing and have fun :cool:
|All times are GMT. The time now is 01:54 AM.|
vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2013 DragonByte Technologies Ltd.
Copyright ©1999-2013 diyAudio