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).
Open 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.
I downloaded Gerbv (free gerber viewer) to visually check what I've got there
open the gerbers and you should see:
By convention:
cmp = top copper ; include top copper, top pads, and vias + dimension
sol = bottom copper ; include bottom copper, bottom pads, and vias. + dimension
plc = top silkscreen ; include anything you want to be printed on the top of the pcb. + dimension
pmc* = 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 + dimension
sts = bottom soldermask +dimension
dri = drill file
gpi 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.
Home
Help
Search
Login
Register
