I’m a bit confused and I think I have some struggles with generating a proper board outline/edge gerber for my PCB design. I have a cirlar PCB design, with a circle defined in the Edge cut layer. As shown in the attached images, the PCB is rendered as a circular PCB in the 3d viewer. Unfortuantely, I am not able to generate gerbers that results in a circular PCB in different gerber viewers, see the square PCB in gerber viewer. I undertand that this may also be that the gerber viewer has not properly loaded the outline file. In the Kicad gerber viewer, the board edge layer is loaded (renamed to .gml) and shown in green.
Can anyone help me a bit with how I can troubleshoot this, or help me confirm that the outline file is correct?
Btw, I’m targeting Dirty Cheap PCBs. Running Kicad 4.0.2 on Windows 7
- Edge Cut layer contrast mode
- Kicad 3d View
- Plot settings
- Gerber viewer (grbv)
- Kicad gerber viewer
Below are the content of the generated Edge Cuts gerber file.
G04 #@! TF.FileFunction,Profile,NP*
G04 Gerber Fmt 4.6, Leading zero omitted, Abs format (unit mm)*
G04 Created by KiCad (PCBNEW 4.0.2-stable) date 23.04.2016 18:12:41*
G04 APERTURE LIST*
G04 APERTURE END LIST*
For test, I removed the circle and replaced it with a 5-sided outline, it loads fine in grbv,
So it seems like it something wrong with my circle.
Do you have the same problem if you use 4x circular arcs to form the circle?
I tried this
circular-outline.gbr (379 Bytes)
And both times I get a circle shown, so the tools are able to do it.
You could also try CircuitPeople and some other website that had an online 3d gerber viewer (that was buggy last time I tried it a year ago).
Question is are the fab house’s tools are up to the task of making a circle or not?
As @cbernardo mentioned, the safe bet is to draw four 90 degree arcs, as arcs must have been with the format for a long time and are a basic element that works - circles not so much.
Some Gerber viewers struggle with the circle and in fact some fabs use an old version of CAM350 which will not interpret those Gerber files correctly and cause all sorts of problems in the PCB fabrication. If Gerber viewers are giving you a hard time then it’s best to use 4x arcs to represent a circle even though that’s a nuisance. The issue was identified over a year ago but KiCad is not at fault in this instance and it makes no sense to corrupt kicad’s output for the sake of keeping someone else’s defective software happy.
It makes sense if all you are trying to do is make a PCB and not trying to change the world. Most KiCad users are just trying to make a PCB.
Forcing fab houses to change their ways by knowingly making life hard for users is stupid. It is this sort of thing that stops me donating to KiCad. Because supporting bad behaviour is wrong - according to KiCad. KiCad needs to focus more on users and not just being “in the right”.
Btw, you are doing great work with the 3d viewer, thanks.
It’s not all about kicad; this problem plagues many industries at many levels. Someone comes along selling defective software and people work around it, and for the sake of one big retailer who doesn’t care to adhere to standards everyone else avoids using useful features. It’s really not worth supporting other peoples’ broken software and perpetuating this problem. Unfortunately the Gerber specification hasn’t got a formal verification process so anyone can do a bad job and say “hey, I’ve got Gerber output” or “we read Gerber files”. Even UCAMCO recommends that people don’t support defective software (but of course they can’t enforce that). IPC-2581 is the next thing and people are working on validation tools; I’m hoping the consortium gets to the point where you can’t claim to support the standard without going through a certification process. Hopefully we won’t have the numerous problems which have plagued Gerber over the years.
A good compromise would be to issue warnings that you are using Gerber features known to have compatibility problems
The fab would need to do this or the ordering website… or do you get warnings in OrCAD or Altium that you’re producing Gerbers that have features which aren’t 100% supported by some Chinese fabs?
Thanks everyone, this was a bit confusing, and it does not help that the gerber viewers handles file extension very differently.
I tried 4x arc and compared with my original circle in a few different tools, and the support for circle is varying.
I don’t know if Dirty Cheap PCBs support circle or not, but I think I will try with the original design with the circle, and see if they accept it or not. (If someone know, please tell)
Thanks for all help
grbv viewer comes with a circular PCB example “Lily pad”, same as on mayhewlabs.com, and the content of the outline gerber file is 300+entries of XY coordinates. I guess that is also a way to represent the circle.
Don’t trust what you see. The gerber viewer may be one thing, but the CAM software used by the fab is a different thing altogether. Ultimately you won’t know unless you ask the fab to do a manufacturing check.
Ok, I understand. I just thought that since some of the gerber viewers did not load the outline at all, if the CAM software would have similar issues, the board fab would reject the design because due to missing outline?
Anyway, I have updated my design with 4 arcs now to be on the safe side.
Thanks for your help.
I’d suggest using FAB 3000 or it’s free cousin DFM Now. In my experience these have one of the most true Gerber parsers (i.e. WYSIWYG).