Eagle file SparkFun Aperature error

Archive BatchPCB
1

I’m tired, it’s late and I got a file to pass Eagle but Sparkfun DRC gives me:

There were errors in the Top Layer File. Please address them and resubmit the zip file. Details bellow:

Checked Aperture 10 (0.0520): Passed

Checked Aperture 11 (0.0520x0.0520): Passed

Checked Aperture 12 (0.1400): Passed

Checked Aperture 13 (0.0433x0.0394): Passed

Checked Aperture 14 (0.0520x0.1040): Passed

Checked Aperture 15 (0.0240x0.0100): Passed

Checked Aperture 16 (0.0100x0.0240): Passed

Checked Aperture 17 (0.1299x0.1299): Passed

Checked Aperture 18 (0.0171x0.0171): Passed

Checked Aperture 19 (0.0050): Failed

Error - Aperture too thin

Checked Aperture 20 (0.0240): Passed

Checked Aperture 21 (0.0100): Passed

Checked Aperture 22 (0.0160): Passed

Checked Aperture 23 (0.0436): Passed

Any hints as to where I can find Aperature 19 so that I can correct it?

Smiley

2

Hi Smiley. Nice to run into you over here.

Try creating a separate DRC file for Spark Fun PCBs. On the Sizes tab, set Minimum Drill to 20 mil. When you run DRC, the DRC error list will show every hole that’s less than 20 mil. You can click on each error and EAGLE will draw a line to and highlight the associated aperture.

Don

3

its a 5 mil trace, I believe. If you open the gerber (.cmp, I’d guess) with a gerber viewer like viewmate, you should be able to see a thin line. If you select it (select/selection tool) and then properties (select/properties), it should show D code 19. You’ll need to widen it out.

It may be text on the copper layer.

4

SmileyMicros:
Checked Aperture 19 (0.0050): Failed

Error - Aperture too thin

Smiley

This is what I do if I’m in a hurry. Just open your gerber file that contains the line giving you the error and change the 0.0050 to 0.0080. Next open the file in Viewmate and double check that everything is ok. Changing the value to 0.0080 changes the 5mil trace to 8mil.

-Bill

5

phalanx:

SmileyMicros:
Checked Aperture 19 (0.0050): Failed

Error - Aperture too thin

Smiley

This is what I do if I’m in a hurry. Just open your gerber file that contains the line giving you the error and change the 0.0050 to 0.0080. Next open the file in Viewmate and double check that everything is ok. Changing the value to 0.0080 changes the 5mil trace to 8mil.

-Bill

yeah, that will work but remember that when ever you tweak the board and regen the gerber, you have to make that change again. I’d recommend just figuring out what the source of it is and fix that in the board layout.

6

In case this helps anyone:

We had a 44-pin TQFP with > 8mil spacing. Owen then rotated the part 45 degrees and exported via eagle.

Sending the design through the aperature script it failed horribly with a 0.0035 problem. 3.5mil?! Where the heck was that? We searched and there were no traces on the board that we could find. But when eagle rotated the part, it mimicked the pads with small traces that were 3.5mils wide, but the overall pads where ok. The script is not smart enough to tell the difference.

Anyone else experience problems with the aperature script? It’s really to stop designs that have smaller than 20mil drills.

-Nathan

7

I opened one of the Eagle generated files in Notepad and deleted a line that I think was %ADD19 something and it passed your tests. I eagerly await the boards to see if they pass the reality check. The really stupid thing I did was not taking notes so now I don’t remember exactly which file nor which line so I get to figure it out anew the next time this happens.

Thanks,

Smiley

8

deleting an aperture will mess up the gerber and probably the board. Look at it with viewmate tobe sure.

9

I did look at it in ViewMate and couldn’t see anything obvious. I suspect that aperture was spurious, but I’ll report back when I get and test the boards.

Smiley

10

I had the same error when I submitted a board. I manually went through the files and found where it was .0060 and changed it to .0080 and it worked. My question is… where do I go in Eagle to change a setting once-and-for-all so that I never have to manually go in and adjust it anymore?

Is there a CAm or a ULP that I can just run that will look for an aperature smaller than .0080 and change it? That would be best… I would run it, save the file, then process the Gerber CAM.

Let me know,

Thanks… Jerry

11

sparky:
In case this helps anyone:

We had a 44-pin TQFP with > 8mil spacing. Owen then rotated the part 45 degrees and exported via eagle.

Sending the design through the aperature script it failed horribly with a 0.0035 problem. 3.5mil?! Where the heck was that? We searched and there were no traces on the board that we could find. But when eagle rotated the part, it mimicked the pads with small traces that were 3.5mils wide, but the overall pads where ok. The script is not smart enough to tell the difference.

I encountered this exact same problem today. Of course, I saw this post after I came to the same conclusion. Rotating parts 45 degrees (as you know) is very common, and on my board, necessary to keep board size down. I redid the board with the part not rotated, and it passes the DRC bot, but I really don’t like how close the traces are now (crosstalk concerns) or the fact that I had to move one of my headers over .2 inches so it is now out of line with its sister.

I don’t think it is that the script is not smart enough to tell the difference. I think Gerber, aging format that it is, must not have a notion of rotation, at least not smaller than 90 degrees, or it does and EAGLE doesn’t know about them.

If there is a way to make rotated parts work with BatchPCB, I’d really like to know about it.

12

I just tried to load a board with parts rotated 45 degrees and got the same aperture error. After some trial and error I found that I changed the roundness of the smd pads on my rotated parts to 50% it accepted my board.

I hope this is helpful to someone.

13

board smoker:
I just tried to load a board with parts rotated 45 degrees and got the same aperture error. After some trial and error I found that I changed the roundness of the smd pads on my rotated parts to 50% it accepted my board.

I hope this is helpful to someone.

I don’t have much experience with PCB CAD software and was wondering if anyone could help me with my problem or expand on the above quote. Essentially I’m getting error for the same problem, is there a way i can modify my problem IC as it is?

14

sebmadgwick:
I don’t have much experience with PCB CAD software and was wondering if anyone could help me with my problem or expand on the above quote. Essentially I’m getting error for the same problem, is there a way i can modify my problem IC as it is?

Greetings (No Name Supplied),

The production of PCBs is complex. It’s a multi-step, multi-tool

process. Plus. we are trying to hit a moving target as newer

devices are introduced with ever smaller feature sizes (pad

counts. pin counts, pad geometry and spacing).

The earliest automation tools were film printers

made by [Gerber Systems Corp. Which has become a standard

for the PCB industry.

As a practical matter the Gerber data file consists of aperture

data and XY co-ords.

The problem that you have run into (along with many of us) is

that elements in a legal Gerber file may be out of limit for the

production house or data checker (the BatchPCB bot in our

case).

To pass the bot the files must conform to the min geometry

imposed by the service (BatchPCB) and the supplier (GP in

China). There’s no magic or sleight of hand here - it just a

fact of life.

To pass the bot you may have to rebuild your PCB design

using parts that conform to the bot standards.

This may be upset by rotation of ‘good’ parts that create

one or more illegal Gerber data points that trip the bot.

In the long term there are two paths to a solution. (1)

change the bot to detect and ignore fragments that are

illegal but part of a larger polygon. (2) Design alternative

parts for use in CAD that are rotated and legal.

I’m not sure where we stand. Perhaps someone has done

the spade work to get legal parts for CAD, or has tweaked

their Gerbers to pass on a case by case basis? The later

is the fastest way past the problem but also the hardest

to support (revisions, sharing, reorders, etc.).

Comments Welcome!](Gerber format - Wikipedia)

15

Well… I’m back.

Did anyone ever make some kind of a CAM processor job that we can run to avoid this? I’m really getting tired of hand editing the files to look for the incorrect aperture. It is always a .00600 instead of a .00800 doing the failure.

Anyone?

Anyone?

Jerry

16

The only real 100% guaranteed solution that I know of is to pop open the conflicting copper gerber file, delete all of the drill data except for the part that uses the conflicting aperture, pop it open in viewmate, see what it draws, and then go make the necessary changes in your board layout tool.

17

I increased the size of the aperture significantly (like from 0.005 to 0.5) to make the area of the board it really obvious in ViewMate, and then I changed it to 0.001 so I could precisely locate the area of the PCB (as the entire PCB area was a big dot otherwise).

That made it very obvious that the problem was the MLF44 footprint (for an AVR) I was using that had rounded pads. I opened the part in the library editor and made all the pads square, which fixed the issue.

Of course, that was one of only two library parts on the entire board that I didn’t make myself - so typical!