topic Re: Incorrect Gerber output? in Fusion Electronics Forum

Incorrect Gerber output?

mphatak68 — Wed, 10 Feb 2021 09:27:39 GMT

Please first see the attached files.

1. OL-Clearance-F3.png:

This shows the Fusion 360 Layer editor, showing the top copper layer only surrounding a NPTH and this clearly shows no additional 'copper ring'.

2. OL-Clearance-EC.png

However, the Eurocircuits Gerber viewer flags a copper ring below the minimum 'outer layer isolation distance' (122um instead of 150um). I have also confirmed the presence of this copper ring using a free Gerber viewer called Cuprum (for Macos).

3. CAM processor Settings

I also attach my CAM processor settings for reference, in case this helps.

Question:

a. Is there some parameter I have set wrongly in generating the copper polygon, which results in the top copper layer creating this additional copper ring? Why am I seeing this?

Any help much appreciated.!

Re: Incorrect Gerber output?

mphatak68 — Wed, 10 Feb 2021 09:59:19 GMT

Just to document my findings on this, I have also tried generating RS-274X (X1) files from the CAM processor, but no difference.

The top copper layer still has a thin ring around the NPTH which violates the minimum clearance at my fab house.

Any suggestions most welcome.

Re: Incorrect Gerber output?

mphatak68 — Wed, 10 Feb 2021 10:59:13 GMT

It seems clear that the Fusion 360 CAM processor is generating plated through holes (PTH) where I have non-plated through holes (NPTH).

Please see attached file from the Eurocircuits analyser, where I have highlighted 4 corner NPTH holes, which are detected as PTH.

Any ideas as to whether this is due to a parameter I have missed or a bug in the CAM processor?

Re: Incorrect Gerber output?

mphatak68 — Wed, 10 Feb 2021 15:22:11 GMT

I have some more evidence to show my theory that Fusion 360 is generating incorrect Gerber data.

Please see attached files.

1. OAR-F3.png

The Fusion 360 layout editor, showing a via with width 1mm and drill hole 0.55mm, which should give an Outer Annular Ring (OAR) = 1-(0.55+0.1)/2 = 0.350/2 = 0.175mm (according to Eurocircuits tolerances).

2. OAR-EC.png

The Eurocircuits Gerber analysis shows a measured OAR of 0.088mm, well below the minimum required of 0.125mm.

Is F360 really generating incorrect Gerber data? Or am I doing something drastically wrong?

Re: Incorrect Gerber output?

engineeringNCMXB — Wed, 10 Feb 2021 18:00:43 GMT

I am nearly finished with my first design done entirely in F360 - planning to test this today and tomorrow. It would be rather disappointing to get all the way to the end only to have a gerber output issue.

Re: Incorrect Gerber output?

mphatak68 — Wed, 10 Feb 2021 18:12:01 GMT

I really hope I am wrong.

I intend to export the F360 files out to Eagle tomorrow and try generating the CAM output from Eagle, to see if this is a Fusion360 issue.

I doubt it will be different, but worth a try.. Will keep you all posted here if I find anything of interest.

Re: Incorrect Gerber output?

jorge_garcia — Wed, 10 Feb 2021 21:17:40 GMT

Hi @mphatak68 ,

When generating these files what CAM job did you use? Since you want to specify plated vs non-plated drills did you make sure to generate two different gerber files? Holes are the Non-Plated through drills, and the drills layer contains the plated through drills. If you are making the distinction you need to make two files one for each layer.

Nothing has been done to the CAM processor recently, so I'm doubtful there is an actual issue in the CAM processor's output but I've been proven wrong before.

Try uploading the files to a different board house with similar tolerances. I've seen Advanced circuits gives this issue with their DFM checker and it's been reported to them various times, but last I checked it hadn't been resolved.

Let me know if there's anything else I can do for you.

Best Regards,

Re: Incorrect Gerber output?

mphatak68 — Thu, 11 Feb 2021 10:40:52 GMT

Hi Jorge

Thanks for your reply. I am answering your questions below:-

1. What CAM job did you use?

I attach the .cam file.

2. Since you want to specify plated vs non-plated drills did you make sure to generate two different gerber files?

I have Gerber files for all copper layers and a .xln file for the drill. Both are generated out by the F360 CAM processor. I attach the zip file containing all layers. Am I missing any files here?

3. Holes are the Non-Plated through drills, and the drills layer contains the plated through drills. If you are making the distinction you need to make two files one for each layer?

Yes, each has its own layer generated out by the CAM processor.

4. Nothing has been done to the CAM processor recently, so I'm doubtful there is an actual issue in the CAM processor's output but I've been proven wrong before.

Thanks for keeping an open mind. I am sure you are right. I just need a solution asap.

5. Try uploading the files to a different board house with similar tolerances. I've seen Advanced circuits gives this issue with their DFM checker and it's been reported to them various times, but last I checked it hadn't been resolved

I have verified the Gerber output with another Gerber viewer (Cuprum). This shows that the generated NPTH holes do in fact have a copper ring around them, which is clearly wrong. I attach the Cuprum image.

Re: Incorrect Gerber output?

mphatak68 — Thu, 11 Feb 2021 11:04:34 GMT

One more thing:-

When I place a new Hole (NPTH), it does not sit on the Holes layer. In fact, nothing appears either in the Drills layer.

With all layers switched off, I still see the NPTH, so I assume this will appear in the .XLN file that is generated from the CAM processor.

What is going on? This seems completely counter-intuitive...

Why does a NPTH Hole not appear in the Holes or Drills layer?

Re: Incorrect Gerber output?

mphatak68 — Thu, 11 Feb 2021 13:52:23 GMT

Re: Incorrect Gerber output?

jorge_garcia — Thu, 11 Feb 2021 18:31:31 GMT

I'm sending you a DM

Best Regards,

Re: Incorrect Gerber output?

jorge_garcia — Fri, 12 Feb 2021 18:09:19 GMT

Hi @mphatak68 ,

After reviewing your design, you have added the board outline and cutouts to all of the copper layers in your gerber output. This is a no-no since you are added mechanical features as copper to those layers and that creates the results you are seeing. Follow the template4 example and you should be OK.

Let me know if there's anything else I can do for you.

Best Regards,

Re: Incorrect Gerber output?

engineeringNCMXB — Fri, 12 Feb 2021 19:22:57 GMT

@jorge_garciathank you for looking at this in detail....I am just shy of pushing Gerbers for a project I have been working on. This thread had me sweating - sounds like all is well.

Re: Incorrect Gerber output?

mphatak68 — Fri, 12 Feb 2021 20:02:17 GMT

Thank you for spotting this, Jorge. and apologies for the mistake on my part.

Apologies also to anyone who might have thought that the F360 CAM Processor was broken in any way.

Mea culpa!