Eagle to Gerber - Page 1
Forum section: electronics / beginners

author: Kemme
author_rank: Contributor
timestamp: October 09, 2015, 08:22:51 pm
content: Hello allOk, so I wanted my PCB to look more professional. I found Chinese PCB makers but they require PCB layout in gerber format.I converted the layout to gerber using functions built in Eagle and I am not sure if everything is ok.I downloaded Gerbv (free gerber viewer) to visually check what I've got there. Eagle created 8 files (.cmp, .dri, .gpi, .ncd, .plc, .sol, .stc, .sts) but in Gerbv I could open 6 only of them (.plc is empty). How do I know everything is ok and Chinese company will make it as I want it to be?

author: rx8pilot
author_rank: Super Contributor
timestamp: October 09, 2015, 08:55:28 pm
content: This task took me quite a while to sort out. The first thing I learned is that the standard Eagle gerber output was totally unusable. I ended up taking the one from Sunstone as a starting point and modifying from there.The hardest part was getting the drill files output formatted right. Step 1 is figuring out how it is supposed to be formatted. Step 2 is figuring out how to get that format on your output. Gerber files were defined many millions of years ago when it was considered wasteful to put a decimal in a number. The system on the other side just need to know where to place the decimal in the stream of integers it receives. 2.4 format is what I use and that means the file will have 6 integers and the receiving system will add the decimal after the first 2 integers. It's easy to figure out how your drills will be in bad places if you are one decimal place off.I use GrphiCode GC preview and can easily see the problems visually. The first thing to check is scaling, just make sure that geometry at a known point is actually there. visually compare the gerber view with a clean view of that layer in Eagle. Make sure the drill locations line up with the pads.After you get a good feeling about it, use the free gerber DFM services like the one the Sunstone does. If you have bad geometry, it can show up in the reports. Ask your new house to do a verification even if you have to pay a little extra for a review.

author: KL27x
author_rank: Super Contributor
timestamp: October 09, 2015, 09:21:11 pm
content: QuoteOpen CAM processor. Open job that you used. You can click on each tab in the CAM processor to see what layers (in Eagle) are included in that Gerber file, in the big window on the right.I believe .plc is usually reserved for a Top Silkscreen. If you do not have a silkscreen, then this would be empty. (Other than a dimension layer)If you want a silkscreen, check your Eagle file to see what layer(s) you want to be in the silkscreen and include them in the .plc file in the CAM processor.Output to Gerber 274x format, unless otherwise specified. Except for the drill file, which most manufacturers accept Excellon, which I would use by default unless otherwise specified. And include the dimension (board outline) layer in each file, unless otherwise specified.Quoteopen the gerbers and you should see:By convention:cmp = top copper ; include top copper, top pads, and vias + dimensionsol = bottom copper ; include bottom copper, bottom pads, and vias. + dimensionplc = top silkscreen ; include anything you want to be printed on the top of the pcb. + dimensionpmc* = top paste include top cream layer + dimension ; this only matters if you are getting a stencil or buying assembled boards*I don't know if this is standard or if I made this up?stc = top soldermask + dimensionsts = bottom soldermask +dimensiondri = drill filegpi files are just garbage. Historically used to look at the files, but you are using Gerber viewer for that, so these are simply garbage.These extension names are completely arbitrary and are strictly by convention for two layer boards. Some manufacturers request different extensions.** In the CAM viewer you can add actual human information to the name of each layer to avoid confusion for yourself and/or manufacturer.In the CAM processor, on each Gerber layer tab there is a button that says "name" then a window containing, say, "%n.cmp" where the "%n" is the name of your brd file, and the ".xxx" is the extension with which it will tag the Gerber layer. You can alter it to say "%n - TOP COPPER LAYER YOU MORON.cmp" if you like. Then when you are viewing that file in your Gerber viewer, you will know what you are looking at without knowing what the 3 letter extensions mean. Because your PSU1.brd file will create a .cmp layer named "PSU1 - TOP COPPER LAYER YOU MORON.cmp"If you need to provide any additional information, you can create an arbitrary extension name for it, say ".tit" or ".ass". include the layers you wish to be in there, and tell your assembler what these files are for. E.g., could include detailed component placement/orientation information for LEDs, or outlines of the shape and placement of a previously specified pressure sensitive adhesive, or whatnot, which you drew up in one or more of your Eagle layers.You have complete control over what info is included in each Gerber layer and the name of the file and extension. But remember that the viewer/receiver cannot separate out that Gerber layer into the individual Eagle layers that you included. So sending them a Gerber that includes silkscreen + copper is not going to do them any good.**ITEAD, for instance, asks for specific extensions for their standard FR-4 prototyping pcb service, .GTO etc, and for the outline to be included in a separate file, by itself, .TKO. And drill layer in a text file. Oddly, enough, if you send them these same file extensions for a flex proto, they won't have the first clue what they're looking at. Separate divisions and/or subcontractors, of course. But you'd think they'd know what/why. Instead it goes:ITEAD: We require Gerbers.Me: These are Gerber274X, as specified on your website.ITEAD: But we need Gerbers.LOL, after figuring out how to make regular Gerbers, finally figured out they just wanted the conventional extensions.

author: zapta
author_rank: Super Contributor
timestamp: October 10, 2015, 01:44:30 pm
content: If your PCB vendor doesn't provide you with Eagle CAM files, you can use these ones from Elecrow (2 and 4 layers respectively).http://www.elecrow.com/wiki/index.php?title=How_to_export_gerber_files_from_eagle_fileYou want to review the generated files in a gerber viewer, just in case.

author: LukeW
author_rank: Frequent Contributor
timestamp: October 10, 2015, 03:47:30 pm
content: I'm used to seeing extensions like this that describe what each gerber file is:GTO - Gerber Top Overlay (silkscreen)GBO - Gerber Bottom Overlay (silkscreen)GTL - Gerber Top SignalGBL - Gerber Bottom SignalGTS - Gerber Top Solder MaskGBS - Gerber Bottom Solder MaskGTP - Gerber Top Paste MaskGBP - Gerber Bottom Paste MaskI've never heard of .ncd, .plc, .sol, .stc etc before, personally. I'm sure they're perfectly usable, standard Gerber files, it's just another naming convention.There are basically two schools of thought on this.You can either go TOPCOPPER.foo or you can go with WhateverProjectName.gtl. Either the filename identifies it or the extension does.Personally, I prefer to use descriptive extensions for the different layers in one of the recognisable standard sets of file extensions. The "Protel standard" extensions as above are the best way to go, IMO.This requires a little bit of mucking around to get the process right the first time you use a particular fab house - especially if there's a language barrier between you and the fab house.Their employee might just "push the button" on a piece of software where they don't really know what they're doing, so sticking with a certain workflow, certain extensions etc is important. But once you know how they work it's fast and easy to set up how they expect it next time.Try the online tool at gerblook.org or the OSHPark online submission tool - these tools should be able to successfully parse your Gerber files, and the board preview images should look right, so that's a good test.

author: Jeroen3
author_rank: Super Contributor
timestamp: October 10, 2015, 05:12:58 pm
content: Very often the PCB house has Eagle DRC and CAM files to download on their website.Such as: iTeadStudio, Eurocircuit, Smart prototyping and probably many more.http://www.eurocircuits.com/PCB-design-guidelineshttp://www.eurocircuits.com/blog/48-V6http://smart-prototyping.com/Prototyping-Services/Electronic-Prototyping/PCB-Prototyping.htmlhttp://iteadstudio.com/store/images/produce/PCB/PCB%20prototype/ITeadstudio_DRC.rarhttp://iteadstudio.com/store/images/produce/PCB/PCB%20prototype/ITeadstudio_CAM.rar

author: zapta
author_rank: Super Contributor
timestamp: October 10, 2015, 05:50:52 pm
content: Quote from: Jeroen3 on October 10, 2015, 05:12:58 pmThat's probably the best choice. Some also have eagle design rules files that match their capabilities. E.g.http://support.oshpark.com/support/solutions/articles/4000019710-eagle-design-rule-files

author: Kemme
author_rank: Contributor
timestamp: October 11, 2015, 02:34:29 pm
content: Thank you for all the replays, they were very valuable for me.Anyway, I chosehttp://www.kikipcb.com/because they are like 5 times cheaper than any other manufacturers I checked.My files were audited and I even had to reupload the files because there was a mistake in one of them. I am really curious about the quality, we will see.