Eagle Gerbers and Excellon Drill Plots?

Go To Last Post
30 posts / 0 new
Author
Message
#1
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Greetings -

I may be having a problem here, or maybe not. I have a board that I have just tried to generate the Gerber plots and a drill file. Because I am doing this on a Mac and because I can't find a MacOS gerber viewer and because I am a bit lazy, I have been using the following on-line gerber viewer:

http://www.gerber-viewer.com/

When I plot the drill plot, it is on the order of 10X larger than the board. The viewer has a distance scale and the gerbers plot correctly, but the drill chart does not.

At this point, I don't know for sure that there IS a problem with my stuff and if there is, WHERE it could be. This evening, I will try some of the other on-line viewers. I may need to step back and install a Windoze viewer on my VMWare/WinXP but it would be nice not to have that hassle.

So, anyone with experience plotting Eagle gerbers and the drill file together? Do they come out right?

Thanks
Jim

 

Until Black Lives Matter, we do not have "All Lives Matter"!

 

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

They ought to - though I've only done it once, and can't for the life of me remember what the name of the program I used was. That's the downside to working through a fever and on a tight deadline.

What you can check is if there's any form of scaling applied, either in the viewer or in the drill/gerber export. The files are nerd-readable, so you should be able to open them and check if there's some scaling there, and you might be able to match up some of the drillings to location values that are all inside the board, thus proving a viewer bug.
It might even be that the gerbers are re-scaled incorrectly in the viewer and the drills aren't, not the more obvious other way around. You never know what bugs these viewers may have. Does the viewer give you any distance measurements that you can verify?

If you're willing, posting the files here could let us poor windows-users check in one of the many available offline viewers, though I can understand the issue with proprietary stuff. Just remember to compress the files, so that we can detect if the 'net has been nasty and dropped the tail end of the file.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

When creating the gerber files from my Eagle designs, I've found that Eagle does the hole placements in the drill file to four decimal place accuracy instead of the three decimal place accuracy used in all the other files. The problem is that the Gerber files don't store the decimal point, they expect you to know where it is.
I don't know how to change this in Eagle, it would be nice if I could. My work-around for now is to fix it when I pull the file into the software controlling the PCB milling machine I use to make circuit boards.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

My experience of using "Viewplot" (Win32 based) was that the gerbers and the drill file from Eagle simply lined up and displayed without error. But I was following a FAQ on the Sparkfun site and it told you the options you needed to set to get the drill file read correctly. One options involved "2 4" which I think meant 2 leading and 4 decimal places perhaps? This was in the Load file dialog of "Viewplot". Maybe other viewers loading Excellon have an option like this?

EDIT: this was the tutorial:

http://www.sparkfun.com/commerce...

there it says:

Quote:
Be sure to select the drill file type '2:4 Leading' to matchup the holes to the layers.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Thanks.

I guess the next thing is to try a different viewer.

I also need to go through that tutorial to make sure everything is set up right. I've been though the Eagle "documentation" but like any comprehensive set of instructions for complex software, its easy to get lost in the details and miss something that is really important at the very end.

Cheers and thanks
Jim

 

Until Black Lives Matter, we do not have "All Lives Matter"!

 

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Jim,

Email me the gerber/drill files

I use graphicode gerber CAM package ( software used by PCB shops to set up production artwork)

I can give You an opinion of the quality of output.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Great - appreciate that. Later this eve (western US time).

I'll post it on a file sharing site (SendSpace) and leave a URL here.

Thanks
Jim

 

Until Black Lives Matter, we do not have "All Lives Matter"!

 

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

ignoramus -

Here are the zipped gerber+excellon files. Thanks for your help. I thought it would be much larger. It could have easily been attached to an e-mail. Oh , well!

http://www.sendspace.com/file/xi...

If you have not used send-space, be sure to scroll to the bottom of the page past the bogus down-load buttons.

Jim

 

Until Black Lives Matter, we do not have "All Lives Matter"!

 

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Jim,

If it helps this is what I see in Viewplot if I turn off "filled" (otherwise the copper pour with all layers showing obliterates most detail):

That looks like the drill file is fine.

There does appear to be a pad or a "blob" on the silkscreen in the top left mounting hole though?

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

For what it's worth, I just gave it a go with Jim's online viewer. There's a checkbox you can use to view the configuration details, and in principle you can set it to "2.4 leading" in that box. However, it doesn't seem to make any difference what settings I choose, I get the same problem that Jim describes.

I ran into the same problem with ViewMate the other day, but I was able to correct it by changing the settings to 4.2 leading. This makes me wonder if the online viewer is perhaps ignoring these settings.

Michael

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

It should be possible to install this on a mac
http://gerbv.sourceforge.net/
Have only tried it in windoze, but works good for me.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Jim,

According to my software the drill file format is:

1.4
Absolute
Inch
Leading zero suppression
Quadrant arc

This last setting is probably unimportant but certainly the first four settings are a must

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Michael try 1.4 LZ Imperial

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Ahhh, good catch on that "blob". It is a misplaced index mark for a connector! I didn't spot that.

I will try gerby. Thanks for the pointer.

Jim

 

Until Black Lives Matter, we do not have "All Lives Matter"!

 

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hello, can anyone help me decode this drill file?
I am trying to understand the drill file format; I was able to understand most of its portion except the coordinates where we have to drill holes. I referred this link http://web.archive.org/web/20071...

but I could not understand (or either the holes are not placed where I expected them to be).

This is my sample drill file
%
M48
M72
T01C0.0320
T02C0.0354
T03C0.0400
T04C0.0433
T05C0.0630
T06C0.1260
%
.
.
.
T06
X1175Y1300
X2356Y2481
X25978Y2481
X25978Y30828
X2356Y30828
M30

I am concentrating on T06 because these are manually placed holes and were easy to keep track or change.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

M72 declares the drill file is in imperial units ( inches)
M71 would make it metric
Also check what format You are outputting.. probably leading zero suppression judging by the very first line after T06 line.
Does this help?

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I could understand these things. The only thing I did not understand is how are they specifying the coordinates. I made a guess but I did not succeed.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

OK.. where did You expect to see T06 holes?

What are the XY coordinates of the holes?
When outputting the holes ( which CAD package?) what were Your settings for hole output?

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Quote:
OK.. where did You expect to see T06 holes?

I have holes of T06 at
0,0
3,3
63,3
3,75
63,75

(coordinates are in mm)

This is what eagle displays when I look at the position property of these holes.

I expected them to be expressed in inches in the drill file, but I can't find them.

Quote:
When outputting the holes ( which CAD package?) what were Your settings for hole output?

I selected excellon.cam job to generate the drill files. (Please correct if I understand your question to be wrong). And I did not select any other settings. Those are same which eagle keeps by default.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

OK..
the first location

X1175Y1300

If output format is 2.4 Leading Zeros suppressed then if first hole is at 0,0 the next hole is at 3,3mm which equates to 0.1181,0.1181inches.
or
X1175Y1300 + (0.1181,0.1181)= X(0.1175 + 0.1181)Y(0.1300 + 0.1181)

which gives us X0.2356Y0.2481

Or more in line with formatting condition 2.4LZS
X2356Y2481 as per second line of the drill file and so on down the list.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Ok. I got it about the coordinates 3,3 and onwards, but what about coordinate 0,0? How will I figure form the drill file that I have to drill my first hole at 0,0. I had checked for the offset in both X and Y direction when I generate the drill file in eagle using the excellon.cam job and both the offsets are set to 0. Then why the locations 0,0 are being displayed as X1175Y1300?
Thanks for your help.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

the offset in the drill file is in line with the CAM output specification absolute zero or relative zero.

Up to You to specify output coordinates.

Read up on Eagle CAM output settings.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I had read the eagle cam output settings (from the cam processor window) there the offset in x and y direction is 0,0. Then why such a thing? What is wrong?

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

The offset generated is different for all the tools. I am unable to figure out the file format. Can anyone help?

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Put up samples of files You can not determine the formats of.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Put up samples of files You can not determine the formats of.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

This is my complete drill file.

%
M48
M72
T01C0.0004
T02C0.0276
T03C0.0433
T04C0.0520
T05C0.0630
T06C0.1260
%
T01
X17406Y770
X15753Y7069
X16737Y7266
X17958Y7305
T02
X7950Y4053
X7950Y2053
T03
X4714Y1431
X4714Y2431
X4714Y3431
X4714Y4431
X4714Y5431
T04
X20281Y6270
X25081Y6270
X25881Y3920
X25081Y1570
X20281Y1570
T05
X4643Y6967
X4643Y8935
X23879Y8971
X25847Y8971
T06
X28233Y9392
X28154Y1675
M30

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

This is the drill information file generated by eagle.

Generated by EAGLE CAM Processor 6.1.0

Drill Station Info File: C:/Users/Mahesh/Documents/eagle/Timer/Timer SMD.dri

Date : 5/5/2013 1:17:22 PM
Drills : generated
Device : Excellon drill station

Parameter settings:

Tolerance Drill + : 2.50 %
Tolerance Drill - : 2.50 %
Rotate : no
Mirror : no
Optimize : yes
Auto fit : yes
OffsetX : 0inch
OffsetY : 0inch
Layers : Drills Holes

Drill File Info:

Data Mode : Absolute
Units : 1/10000 Inch

Drills used:

Code Size used

T01 0.0004inch 4
T02 0.0276inch 2
T03 0.0433inch 5
T04 0.0520inch 5
T05 0.0630inch 4
T06 0.1260inch 2

Total number of drills: 22

Plotfiles:

C:/Users/Mahesh/Documents/eagle/Timer/Timer SMD.drd

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Quote:
%
T01
X17406Y770
X15753Y7069
X16737Y7266
X17958Y7305

I think that if you have "positive coordinates" checked in the CAM dialog, EAGLE will generate drill coordinates with an offset such that the most negative thing in your drawing (NOT just the lowest-coordinate hole) will be entirely within positive coordinate space. And then adds some additional offset just in case. If you want the drill coordinates to match the eagle coordinates, try unchecking "pos. coord"

The manual says:

Quote:
 Pos. Coords.: Avoids negative coordinate values for the output. The drawing will be moved near the coordinate's axis,
even if it is already in the positive coordinates range.
Negative values can lead to errors with a lot of devices!
This option should be set on always by default. Switching it off, transfers the coordinate values from the Layout Editor unchanged.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Ok. So the most negative coordinate is considered as zero to avoid negative coordinates, but how will I figure it out that which is my zero if I only have the drill file?