I am short of finishing my first PCBs and want to include v-scoring. I contacted the PCB manufactures and they tell me to use the GM layer or the GO layer and make there the v-scoring so they can read it from the corresponding Gerber files.
I do not see a GM or a GO layer in KiCad ¿ so how do I do it ?
KiCad can output in Protel File Extensions. It is likely that your manufacturer is referring to those layers. From the file list here, you can see that “GM1” or “GKO” layers are Gerber Mechanical 1 or Gerber Keepout.
This list has slightly more commentary. It indicates GM1 is “board outline” and gko is “keep out”.
I’m guessing that they are expecting (as option 1) that you put the V-cut on the Edge.Cuts layer in KiCad, then in Gerber Options, make sure to select “Use protel filename extensions.”
Last time I just used the drawings layer and drew a line to represent the v score with a big fat text saying “this is a v-score”. You can rename that gerber layer file to .GM1
Hope your manufacturer is ok with that, mine was.
You have the GM1 file listed! You should be able to draw your V cut on the edge cuts layer and it should appear in the GM1 file. You can confirm with the Gerber viewer. I would expect (but do not know for sure) that they can differentiate actual edge cuts and V cuts in the same file (presumably the edge cuts are the outermost outline)
I am not familiar with whether just renaming a file is acceptable with Gerber files.
Anyone more familiar or experienced in manufacturing care to comment?
Internally, there is nothing in a Gerber file to indicate its purpose or function. It is simply a set of commands telling how to “draw a picture”. Once the picture is drawn and placed before a human person, it’s function may be obvious but usually there is external information to tell you what the picture is supposed to represent. Open a Gerber file - any Gerber file - in a good text editor (I like “Notepad++”) and you’ll see what I mean.
So Gerber filenames are completely insensitive to the both the basic name, and the extension. Traditionally, when you submitted Gerber files to a board fabricator you included a “Readme.txt” file that identified the function of each Gerber file. In more recent times, board fabricators have specified particular naming conventions. There must be at least half a dozen “conventions” for using the 3-letter extension to indicate the purpose of the Gerber file, depending on what layout program created the file or which vendor will fabricate the board. E.g., the Gerber file for the top silkscreen layer might be called “Awesome_Circuit_Gerber.slk”, or “Awesome_Circuit_Gerber.tss”, or “Awesome_Circuit_Gerber.tsk”, etc.
(And many of us superannuated old guys will include a text string on the layer itself - e.g., “Top Silkscreen” - placed near to, but outside the actual board perimeter. As a last resort, you hope that a sharp-eyed CAM Operator will see this string on his display and correct any inconsistency before the board is actually fabricated.)
So if I understood correctly your post Y can use the Eco1.user.xxx file, rename to " Customer-desired-V-Scoring… ", send then a Little text file telling them " That is were I want my V.Scoring " Right ?
Well I think that would be worth a Trial and as Long as I have not paid, they will not produce my boards So nothing damaged …
Yes, that’s right. If the fabricator will accept the information transmitted in that way, your problem is solved. Some of them have inflexible internal processes that rely on strictly-enforced file-naming conventions.