How to get gerbers from Eagle - Page 1
Forum section: electronics / general

author: Simon
author_rank: Unknown
timestamp: February 28, 2014, 09:13:48 am
content: I have been sent the project files by our subcontractor and they are in eagle, so I have downloaded and installed the basic version. It's a bit cranky (there's a surprise) but all i need to be able to do is get gerbers from the project. How do I do that, does the free version allow it ? I assume he used a paid version of eagle.

author: Kjelt
author_rank: Super Contributor
timestamp: February 28, 2014, 09:55:27 am
content: The free version only allows:•EAGLE Light (1 schematic sheet, 2 signal layers, 100x80mm routing area)Is the design within these parameters?

author: Simon
author_rank: Unknown
timestamp: February 28, 2014, 09:56:27 am
content: no, it's 3 sheet and 100x100mm so I'm bugered and need to ask him to generate the gerbers for me.

author: Kjelt
author_rank: Super Contributor
timestamp: February 28, 2014, 09:57:51 am
content: Maybe you can do it, you can try. The viewer may let you generate an already made design but you can not alter it, you have to try.Here are the simple guidelines how to generate a gerber from eagle:http://www.eurocircuits.com/index.php/technology-guidelines/pcb-layout-data/117-cadsoft-eagle-brd-to-gerber-conversion-guidelines

author: Simon
author_rank: Unknown
timestamp: February 28, 2014, 10:01:03 am
content: I think I will ask for the subcontractor to sort it out, that's what they are paid for, we just need all of the manufacturing information should they go bust.

author: baljemmett
author_rank: Unknown
timestamp: February 28, 2014, 12:34:17 pm
content: Quote from: Kjelt on February 28, 2014, 09:57:51 amI believe that's correct - and in fact using a free license as a .brd- > gerber exporter seems to be explicitly allowed - from the license, schedule 3, "conditions applicable to the Freeware edition only":QuoteIn terms of how the board size restrictions are implemented, it lets you open (and in fact create your own) boards that are larger than the maximum size, but you can't place any components outside of the specified bounds. So as long as you're not editing the board, or you only need to re-route traces or add text or suchlike without moving any components, it won't stop you.Generating gerbers is done with the CAM Processor which I believes comes with some pre-configured Job files to set it up with a sane starting point - but since there seem to be plenty of tutorials that come up when Googling the obvious sort of phrases, I'm sure I'd only be making a pills of things if I tried explaining the process from memory!

author: FrankBuss
author_rank: Unknown
timestamp: February 28, 2014, 12:55:39 pm
content: Usually you use a CAM file, which some PCB manufacturers provide, see for example athttp://imall.iteadstudio.com/im120418001.htmland click at the bottom of the page "download". Then you can open the BRD file in Eagle and run the CAM job, as explained here:http://support.oshpark.com/support/articles/134816-generating-custom-gerbers-from

author: LukeW
author_rank: Frequent Contributor
timestamp: April 11, 2014, 12:32:16 am
content: You should be able to do it, generally the free Eagle license will let you open and view Eagle files that exceed the "free rules", eg. big dimensions or >2 Cu layers. But you just can't modify those files on the internal copper layers or outside the "free dimensions". But I think the CAM processor should still work.Basically, in Eagle you've got a plethora of different layers, like a couple of hundred different types of layers.When you physically make a board, you've got maybe 6-10 layers, or so. For example you've got top and bottom copper, top and bottom soldermask, top and bottom silkscreen, internal copper layers if it is a >2 layer board, top and bottom paste stencils, and the drill file.What you do in the Eagle CAM Processor, to give you a really basic short explanation, is to go through each of the half-dozen or so "physical layers" of your board each of which will correspond to a Gerber file, and create a "map" which specifies which layer(s) of the hundreds of "Eagle internal" layers will "map" onto that physical layer.For example you might have the "Top", "Pads". and "Vias" layers mapped onto the top copper layer, and the "Bottom", "Pads" and "Vias" layers mapped onto the bottom copper layer, and the "tPlace" layer mapped onto the top silkscreen, although you may add other layers such as tNames or tValues to the top silkscreen layer if you like.I actually use a makefile to do it for me. But you can do it in the GUI in Eagle's CAM Processor setup.Code:.PHONY: gerbersgerbers :mkdir -p gerbersmkdir -p tempfor f in `ls *.s#* *.b#* 2> /dev/null`; do mv $$f ./temp/; doneecho "Generating Gerber files..."eagle -X -d GERBER_RS274X -o ./gerbers/$(PROJECT_NAME).GTL $(PROJECT_NAME).brd Top Pads Vias Dimension > /dev/nulleagle -X -d GERBER_RS274X -o ./gerbers/$(PROJECT_NAME).GBL $(PROJECT_NAME).brd Bottom Pads Vias > /dev/nulleagle -X -d GERBER_RS274X -o ./gerbers/$(PROJECT_NAME).GTO $(PROJECT_NAME).brd tPlace > /dev/nulleagle -X -d GERBER_RS274X -o ./gerbers/$(PROJECT_NAME).GTP $(PROJECT_NAME).brd tCream > /dev/nulleagle -X -d GERBER_RS274X -o ./gerbers/$(PROJECT_NAME).GBO $(PROJECT_NAME).brd bPlace > /dev/nulleagle -X -d GERBER_RS274X -o ./gerbers/$(PROJECT_NAME).GTS $(PROJECT_NAME).brd tStop > /dev/nulleagle -X -d GERBER_RS274X -o ./gerbers/$(PROJECT_NAME).GBS $(PROJECT_NAME).brd bStop > /dev/nulleagle -X -d GERBER_RS274X -o ./gerbers/$(PROJECT_NAME).GML $(PROJECT_NAME).brd Milling > /dev/nulleagle -X -d GERBER_RS274X -o ./gerbers/$(PROJECT_NAME).GKO $(PROJECT_NAME).brd Dimension > /dev/nulleagle -X -d EXCELLON -o ./gerbers/$(PROJECT_NAME).TXT $(PROJECT_NAME).brd Drills Holes > /dev/nullzip $(PROJECT_NAME)-gerbers ./gerbers/*.*image :`gerbv --export=png --output=$(PROJECT_NAME)-pcb.png --dpi=$(GERBER_IMAGE_RESOLUTION) --background=#$(BACKGROUND_COLOUR) --f=#$(HOLES_COLOUR) \gerbers/$(PROJECT_NAME).TXT --f=#$(SILKSCREEN_COLOUR) gerbers/$(PROJECT_NAME).GTO --f=#$(PADS_COLOUR) gerbers/$(PROJECT_NAME).GTS --f=#$(TOP_SOLDERMASK_COLOUR) \gerbers/$(PROJECT_NAME).GTL --f=#$(BOTTOM_SOLDERMASK_COLOUR) gerbers/$(PROJECT_NAME).GBL &`echo "Gerber photoplotter files and board preview rendering generated."