brd / gerber differences

zoks77 <communitymanager@premierfarnell.com> wrote:

I have set DRC rules for minimum width and clearance to 5 mils.

Everything is perfectly fine in the board editor, but when gerbers are

generated using the CAM processor, there are some spots with clearance

less than 5 mils. For example, a clearance between a top layer rounded

SMD pad and ground polygon goes down to 4.85 mils (marked by white marks

in the attached image). The problem was detected by the board house

because it violated their DRC. I don't have a gerber viewer that would

support the DRC, but the problem can also be verified bya  measuring

tool. Any idea what to do about this?

I doubt its an Eagle bug. Could it be that your stop layer is included with

the copper and expands all your pads? Another issue cold be caused by wrong

aperture sizes, but if you use gerber274x (need to have the x!) I thought

you would be safe.

Btw I can not see your attached image..

The device used is GERBER_RS274X with 'pos. Coord.' and 'Optimize' options checked. There are no aperture sizes to be defined for this device. For the top copper gerber generation the following layers are included:

1 Top

17 Pads

18 Vias

20 Dimension

I have never had this problem before or at least I have not been aware of it since I have used 8 mils clearance which is well above the technological margin of the board house. Maybe the problem has always been there but it was not critical until the clearance has been reduced to 5 mils. I guess it may be something related to how Eagle makes the gerbers; if you look at the close-up image of the gerber file I've attached to this message you can see the polygon wire protruding slightly from a polygon which is definitely not OK.

I will have no problem getting this board produced but it will cost a bit more because of this. I would just like to find out where the problem is to avoid it in the future without having to increase the DRC width and clearance settings just to be on the safe side (which I cannot be if I don't know why this is happening).

This message has been posted on element14 forums with the image attached (see http://www.element-14.com/community/thread/12274). I guess the image just does not show up in the newsgroup message.

On 3/27/11 9:33 AM, zoks77 wrote:

The device used is GERBER_RS274X with 'pos. Coord.' and 'Optimize' options checked. There are no aperture sizes to be defined for this device. For the top copper gerber generation the following layers are included:

1 Top

17 Pads

18 Vias

20 Dimension

 

I have never had this problem before or at least I have not been aware of it since I have used 8 mils clearance which is well above the technological margin of the board house. Maybe the problem has always been there but it was not critical until the clearance has been reduced to 5 mils. I guess it may be something related to how Eagle makes the gerbers; if you look at the close-up image of the gerber file I've attached to this message you can see the polygon wire protruding slightly from a polygon which is definitely not OK.

 

I will have no problem getting this board produced but it will cost a bit more because of this. I would just like to find out where the problem is to avoid it in the future without having to increase the DRC width and clearance settings just to be on the safe side (which I cannot be if I don't know why this is happening).

 

This message has been posted on element14 forums with the image attached (see http://www.element-14.com/community/thread/12274). I guess the image just does not show up in the newsgroup message.

 

  Image:gerb.png

 

Try using the GERBER_RS274X_25 device which has an extra digit of

precision (2.5 format instead of 2.4 format). I had this same problem

and Cadsoft kindly added the GERBER_RS274X_25 device to resolve the issue.

--

Andrew Sterian

Emsyde Design

Yes, this appears to have solved the issue. Thank you very much!