Hi!
Is it feasible to hand–edit a Gerber File to amend the Silkscreen Font?
. . .I have downloaded a set of Gerber Files to make Bob Cordell's Distortion Analyser from a GitHub Repository, but the files provided originally were done from Eagle 9.3.2. which doesn't have a means to amend the silkscreen Font!
. . .However, I do have several of my own designs which I used the Silkscreen Font I would like to use, so if the Gerber Command lines that plot the Silkscreen Letters and numbers can be identified, would the modified Gerbers come out with thie font I desire if I change the Gerber Lines for the Eagle Boards Silkscreen to the ones I made?
. . .The GitHub Repository for the THD Analyzer doesn't provide the Native *.brd Eagle Files, so I can't directly import them for graphical modification!
. . .I know JLC's Photo Plotting machines successfully deal with T.T.F. PCB silkscreen as I have PCBs successfully manufactured with them, such as my design for a 1967 Vintage C.T.V. replacement PCB I made with "Grotesque" silkscreen to match the original 1967 board!
. . .(If I made a "dummy" board design with one component on it and then added the silkscreen text for each letter and number, etc., in the font I want to use in the desired style, would that indicate which Gerber Command is produced by letter?)
Chris Williams
Is the problem vector v. proportional font? Some board houses can fix that for you.
I stayed at Eagle 7.xx. With that version, you can change from proportional to vector.
Edit: I am not sure about backward compatibility from ver. 9.x, but if you zip and post the file, I will try it for you.
Hi!
Is it feasible to hand–edit a Gerber File to amend the Silkscreen Font?
By hand?
Gerber isn't like Postscript and only has very low-level drawing commands. It doesn't have any commands to handle text per se.
The letters are drawn with line and arc commands.
It is theoretically possible for Eagle to use an aperture macro for each different letter but I doubt it.
However you can open Gerber files with for example gerbv and delete the items you don't want. Then you can merge in your own silkscreen layer. I don't know if gerbv can merge layers but it shouldn't be too hard to do by hand if needed.
There are editors around for Gerber files, but it's quite specialized software. PCB manufacturers use it for example for panelization.
Your TTF text is also not really TTF. The PCB software has converted the text to separate vectors, and put those vectors in the gerber files. (It is probably possible to generate D-codes or macro's for each letter to create a "font" like think in a gerber file, but I don't know if such a thing is really done).
It may be possible to create a simple PCB project, create gerbers from it, and then hand-copy a part of the content from one gerber file to another to add some text, but it will need experimentation and it's error prone.
In KiCad it is quite easy to back import a set of Gerber files to create a PCB file.
The result is not perfect, for example it does not have real footprints, because those don't exist in Gerber files. But the result is usable. If you want to go further, it is easy (but it takes some time) to remove the constructs that are supposed to represent the pads / footprints, and put real footprints on the PCB.
. . .I have downloaded a set of Gerber Files to make Bob Cordell's Distortion Analyser from a GitHub Repository, but the files provided originally were done from Eagle 9.3.2. which doesn't have a means to amend the silkscreen Font!
Chris Williams
My apologies. I misunderstood that sentence and assumed you also had access to the Eagle files. If that is not the case, then I agree with the others. I cannot help with Eagle.
The quick answer to this is no, text on Gerber is just graphics, there no notion of font or text.
But if there isn't too much text to change, what you could do is use a Gerber editor, remove all elements that pertain to silkscreen text and replace them manually with new ones.