Gerber lines in ground plane

[Anonymous]

My manufacturer is asking me to remove those lines from the ground gerber layer

I've been searching information about this problem and I've found nothing, I don't know if it has a specific name or it isn't a real problem

It's a problem of the gerber file?

I'm using Eagle 8.3.2 and GERBER_RS274X as device output

The polygon properties:

polygon pour: solid

isolate: 0

rank: 6

Orphans: uncheck

Thermals: check

I've edited this last options, and none of them seems to solve the problem. I've also selected the polygon pour as hatch but instead of line I see dots

The cam file I'm usign to generate the gerber file is this

I'll really appreciate any help

[Anonymous]

@jorge_garcia Thanks for your answer, I must admit it's a very weird error and I'm sure that It can't be happening to all users because there is like 2 more post related to this topic.

That .def file you mention is generate when you create a new project or once when you install Eagle? I've tried eagle in Windows 10 and Ubuntu, and both cases I've the same problem.

The last thing, I'd like to apologize, if I offended anyone with my comment. I really feel very sorry for everyone affected by the hurricane. I sincerely hope that they can recover and move forward in this difficult time.

[rachaelATWH4]

---

@jorge.garcia wrote:

@Anonymous This type of error could have been caused by a defective eagle.def file, I have no idea how that could have happened in your case but that is the only thing I can think of that hasn't been mentioned so far in this thread.

---

Hi Jorge,

When I tried @Anonymous's project I could see the issue on my machine and I definitely don't have a defective eagle.def. However, I only ever used gerbv previously for viewing my Gerber outputs so maybe I just haven't noticed any discrepancy.

So I have just gone through everything again. The originally uploaded Gerber file and the one I generated from the project both render correctly in gerbv on my machine. However, when I view them in gerbview (from KiCAD and not to be confused with gerbv) I can see the lines which are apparently an issue to the board manufacturer. In gerbview I can see which D codes are being used for the lines which are causing the issue and in this case it's listing it as D40. Examining the Gerber file I can see D40 is specified as 0.007 inch. If I manually adjust the file to 0.0077 inch and reload it into gerbview the issue goes away.

Now, I'm not an expert on the Gerber format or how this translates into a manufacturing process. I suspect you can't just go changing this value and expect things to work as this is specifying a tool size so I guess it needs to be a certain size within some tolerance. Maybe it's worth loading up the Gerber layer as generated from EAGLE and the Gerber layer as generated from KiCAD into gerbview and then do Miscellaneous->List DCodes and have a look if they are set up differently between the two versions.

I suspect there is an issue relating to rounding going on somewhere and it's likely in Gerbview, and also Altiums viewer that the PCB manufacturer was using. Using the original data I can view the output correctly in gerbv and Cameron can view it correctly in Viewmate and I've never had a board house complain about lines in my power planes so I don't think there is actually anything wrong with the process EAGLE uses for generating the data.

Best Regards,

Rachael

[jorge_garcia]

Hi Guillermo,

That is very cool of you, thank you. No worries and no harm done. I see below that Rachael is seeing the same behavior and I know her setup is good.

I'm going to check your files out and bring them to our CAM developer and his team who are experts in the Gerber standard and maybe they will be able to enlighten us as to what is going on.

Thanks for sharing the files, I'll get back once I have something to report here.

Please let us know if there's anything else we can do for you.

Best Regards,

[Anonymous]

Hi,

I have been reading the changelog of the last releases and seems there is not change related to this issue

does eagle keep working the same way redering the gerber file?

[jorge_garcia]

Hello @Anonymous,

I hope you're doing well today. EAGLE 8.4.1 doesn't have any improvements in this area. Our hope is to include these improvements in our next major release 8.5.0 but I can't guarantee anything because there are a lot of changes being made to a very critical part of EAGLE the CAM processor so we don't want to rush it. When it releases we want to make sure that it's as bulletproof as we can make it.

Best Regards,

[Anonymous]

Hello,  I had the same problem with lines in ground plane pour

what I did was:

1) change from Solid pour  to  Hatch pour in order to enable the space parameter.

2) Set the value of space = width  (i.e. 6 mils).   

3) generate Gerber files and open, now appears as a solid ground. 

have a good day.

Eagle 7.3

[C.Nicks]

As an FYI, the lines seen in ground planes tend to be artifacts of the viewer due to the lines of the polygon being extremely close together.
In Viewmate, sometimes the display shows them, but it changes with the zoom and movement.

Note: Seeing the lines in the planes should not affect the actual finished product. Even with the old CAM processor, I never had a board house bring up any issues in regards to the plane and they have all shown up with intact planes. The gerber processors they use to prepare the files are quite different than the free viewers we use.