Errors with eagle gerber files for fabirication.

Archive BatchPCB
1

So I’ve finally designed my board, and am trying to get it created. I ran the gerber.cam job/macro, and after adding a new job called Supply AGND, that only has the $AGND layer selected (obviously a ground layer), and telling it to optimize and output with the name *.ly2 (since it is layer 2), it complains about "

!!! APERTURES MISSING - NO PLOTFILE HAS BEEN PRODUCED!"

I told it to emulate apperatures after that, then it only says it once… but i don’t know if that is a workaround, or it just ignores a crucial part of this.

Secondly, I’m trying to use 4pcb.com to make my board, but when i upload my *.drd.#### files (I have two of them, *.drd.0102 and *.drd.0116, presumably for different sizes), the site complains. I use their freedfm part, and select them both as nc drill files, and it complains about having two. What am I supposed to do? Is there a way to make the excellon.cam job compress them into one file, or some other workaround for getting 4pcb.com to work?

EDIT: Okay, i found out they actually mean drills from layer 1 to 2, and layer 1 to 16, but I still need help with how to put up ones 4pcb will accept.

Below is a copy of my GPI file before I added the “emulate appertures” checkbox.

Photoplotter Info File: C:/Program Files/EAGLE-4.16/projects/snrprojsensor/sensor1.gpi

Date : 5/24/2007 12:57:29p

Plotfile : C:/Program Files/EAGLE-4.16/projects/snrprojsensor/sensor1.ly2

Apertures : C:/Program Files/EAGLE-4.16/projects/snrprojsensor/sensor1.whl

Device : Gerber photoplotter

Parameter settings:

Emulate Apertures : no

Emulate Thermal : no

Emulate Annulus : no

Tolerance Draw + : 1.00 %

Tolerance Draw - : 1.00 %

Tolerance Flash + : 1.00 %

Tolerance Flash - : 1.00 %

Rotate : no

Mirror : no

Optimize : yes

Auto fit : yes

OffsetX : 0inch

OffsetY : 0inch

Plotfile Info:

Coordinate Format : 2.4

Coordinate Units : Inch

Data Mode : Absolute

Zero Suppression : None

End Of Block : *

Missing Apertures:

-------- Requested Aperture --------

Shape Size used

thermal 0.0800inch x 0.0600inch 1

annulus 0.0800inch x 0.0000inch 1

annulus 0.0720inch x 0.0000inch 7

thermal 0.0720inch x 0.0520inch 1

annulus 0.0840inch x 0.0000inch 2

thermal 0.0860inch x 0.0660inch 1

annulus 0.0951inch x 0.0000inch 2

annulus 0.0636inch x 0.0000inch 21

thermal 0.0596inch x 0.0396inch 16

Apertures used:

Code Shape Size used

!!! APERTURES MISSING - NO PLOTFILE HAS BEEN PRODUCED!

2

yogurtron:
Secondly, I’m trying to use 4pcb.com to make my board, but when i upload my *.drd.#### files (I have two of them, *.drd.0102 and *.drd.0116, presumably for different sizes), the site complains. I use their freedfm part, and select them both as nc drill files, and it complains about having two. What am I supposed to do? Is there a way to make the excellon.cam job compress them into one file, or some other workaround for getting 4pcb.com to work?

Greetings yogurtron,

4pcb.com isn’t BatchPCB. Have your tried uploading your work to BatchPCB? If that works you’ll need to contact [Advanced Circuits ( for help with their tools).

Comments Welcome!](http://www.4pcb.com/)

3

So I’ve finally designed my board, and am trying to get it created.

How many layers does this board actually have?

I have Eagle 4.11 and i’m not sure what you are doing here.

I have had many double sided boards fabed by Advanced Circuits. I use the gerb274x.cam job file. The default file will only produce a two sided board with the component side .cmp (top) and solder side .sol (bottom) plus the top silkscreen .plc and the top and bottom stops. five files + a .gpi file

The .gpi file should look something like this. (but you don’t really need to worry about it or ever actuallly look at it)

Photoplotter Info File: E:/SAIC/KBTMP/000_7-SP.gpi

Date : 3/13/2007 01:19:40p

Plotfile : E:/SAIC/KBTMP/000_7-SP.sts

Apertures : generated:

Device : Gerber photoplotter with RS-274-X aperture generation

Parameter settings:

Emulate Apertures : no

Emulate Thermal : no

Emulate Annulus : no

Tolerance Draw + : 0.00 %

Tolerance Draw - : 0.00 %

Tolerance Flash + : 0.00 %

Tolerance Flash - : 0.00 %

Rotate : no

Mirror : no

Optimize : yes

Auto fit : yes

OffsetX : 0inch

OffsetY : 0inch

Plotfile Info:

Coordinate Format : 2.4

Coordinate Units : Inch

Data Mode : Absolute

Zero Suppression : None

End Of Block : *

Apertures used:

Code Shape Size used

D10 round 0.3880inch 1

D11 round 0.1380inch 7

D12 round 0.5080inch 2

D13 round 0.1104inch 2

D14 round 0.2245inch 2

D15 round 0.0920inch 140

D16 round 0.1580inch 72

D17 round 0.0740inch 140

D18 round 0.1281inch 2

D19 octagon 0.0780inch 2

D20 oval 0.0520inch x 0.0960inch 2

D21 oval 0.1120inch x 0.0600inch 8

D22 rectangle 0.0474inch x 0.0552inch 12

D23 octagon 0.0630inch 20

D24 rectangle 0.0552inch x 0.0474inch 2

D25 square 0.0480inch 68

D26 octagon 0.0480inch 11

D27 round 0.0480inch 60

It gets generated automatically when using the default settings.

Whatever holes or via’s you have simply run the drillcfg.ulp to create the Excellon rack file, then run the excellon.cam and between those they will generate a .drl .drd and .dri. Advanced needs the .drd .drl .cmp .sol .plc .stc and .sts files in a winzip format and if included the .dri can be listed as other drawing or whatever.

Unless you have blind vias ( haven’t tried that) I can’t think of any reason to ever have two .drd files. ( 4.16 can’t be all that different from 4.11 can it?)

So if you want to deal with Advanced then try dumping the “emulate apetures” and plain “Device : Gerber photoplotter” and just use the 274x.cam, drillcfg.ulp and excellon.cam to produce your output files.

Run the drillcfg.ulp from the “File > Run > drillcfg.ulp” from your board edit window with all layers active. Use the file it produces for your rack file but don’t run your CAM jobs from the board or schematic windows, run them from the Eagle command window. And don’t forget to load your correct “*.brd” file for the gerb274x.cam and and Excellon.cam windows using their “file > Open > Board”. Plus remember where you put your .drl and load it using the RACK button in the excellon.cam window. You have to specify the output file names and destinations as well.

Maybe you are doing something I just don’t understand. But I’ve had a butt load of boards made by Advanced and they have all been very good quality.

4

I use 4pcb quite alot. The only thing better than the quality of their PCBs is their customer service. Making gerbers for them is fairly straight forward. I had to make a couple modifications to the standard Eagle cam file, however. If you’d like - I can send you the modified one.

5

I had to make a couple modifications to the standard Eagle cam file, however. If you’d like - I can send you the modified one.

Which mods have you made?

I recently added the bottom silkscreen layer, I can’t really understand why that wasn’t included in the standard 274x.cam

6

TruAnRksT:

I had to make a couple modifications to the standard Eagle cam file, however. If you’d like - I can send you the modified one.

Which mods have you made?

I recently added the bottom silkscreen layer, I can’t really understand why that wasn’t included in the standard 274x.cam

IIRC - I added a second silkscreen layer, and also had to mirror one of the layers. I did it quite a while ago - so there could be other things that I'm just forgetting.