oshpark & gerber...

[Hul Tytus]

Ospark.com\'s quote section took a gerber .zip file (generated by Eagle
version 3.5) and stated that the .drl file was \"not a valid drill file\" and
the .drd file \"did not contain tool size info\". Assuming for now that \"tool
size\" is synonamous with drill size. The Eagle here wouldn\'t accept the
instructions shown in Oshpark\'s .cam file for Eagle, unfortunantly.
I had no luck getting a file or files from them that specified drill size &
drill location. The idea being to write a program to translate the .drl & .drd
files generated here to the form accepted by Oshpark\'s web site.
I\'m hoping someone here who has used Oshpark (or 4pcb.com?) will send me a
Gerber file(s) or portion thereof that specifies drill size & drill location
to serve as a model for the above mentioned translater. A complete gerber .zip
file, if convenient, would serve as well. Also, it needn\'t be generated by
Eagle but just be in accordance with the Gerber specs.
That could be sent to me via email at gbx@rs-big-print.com with the gerber
file(s) attached or placed in the message itself as shown below. [Warning -
anything sent to the ht@panix.com email address shown here would be flushed.]
Or it could be added to a usenet message, as shown below.

Hul

; gpsallp.drl diameters of drill
T01 0.020in
T02 0.032in
T03 0.035in
T04 0.040in
T05 0.055in
T06 0.056in
T07 0.070in
T08 0.140in
T09 0.193in

; gpsallp.drd hole locations
%
T01
X606Y1197
X606Y1532
X901Y1352
X1191Y1357
X1196Y1267
X1371Y1482
X1446Y1282
X1521Y1327
X1506Y1472
X1456Y1017
X1906Y1197
X1906Y1532
X2201Y1352
X2491Y1357
X2496Y1267
X2671Y1482
X2746Y1282
X2821Y1327
X2806Y1472
X2756Y1017
X1959Y3032
X2279Y3102
X2539Y3247
X2649Y3247
X2696Y3287
X2751Y3287
X2801Y3307
X2831Y3352
X2836Y3412
X2806Y3467
X2751Y3492
X2696Y3492
X2334Y3782
X1506Y3472
X1521Y3327
X1446Y3282
X1371Y3482
X1196Y3267
X1191Y3357
X901Y3352
X606Y3197
X606Y3532
X1456Y3017
X1531Y5182
X1131Y6677
X1131Y7232
X2741Y7192
X2751Y7357
X2781Y7452
X2836Y7402
X2781Y6752
X2751Y6657
X2741Y6492
X2836Y6702
T02
X1831Y5767
X1831Y5692
X1831Y5617
etc...

 

[Ed Lee]

On Saturday, February 26, 2022 at 7:46:42 AM UTC-8, Hul Tytus wrote:

Ospark.com\'s quote section took a gerber .zip file (generated by Eagle
version 3.5) and stated that the .drl file was \"not a valid drill file\" and
the .drd file \"did not contain tool size info\". Assuming for now that \"tool
size\" is synonamous with drill size. The Eagle here wouldn\'t accept the
instructions shown in Oshpark\'s .cam file for Eagle, unfortunantly.

Use Excellon Drill format, not Gerber.

Download a gerber viewer than can handle both. Import Gerber and export Excellon.

 

[Johann Klammer]

Unsure if this applies to your problem:
here\'s the start of some drill file for JLCPCBs CAM job
(the tool sizes are prepended to the drill insns inside the same file)
also:

M48 Defines the start of an M48 part program header
M72 │ Inch Measuring Mode

minimum.XLN:

%
M48
M72
T01C0.0120
T02C0.0360
T03C0.1260
%
T01
X5585Y3473
X6835Y3473
X7585Y3723
X8585Y4223
X9085Y4723
X8835Y5223
X9335Y5973
X9835Y6223
X10335Y5723
[...]

 

[Rick C]

On Saturday, February 26, 2022 at 10:46:42 AM UTC-5, Hul Tytus wrote:

Ospark.com\'s quote section took a gerber .zip file (generated by Eagle
version 3.5) and stated that the .drl file was \"not a valid drill file\" and
the .drd file \"did not contain tool size info\". Assuming for now that \"tool
size\" is synonamous with drill size. The Eagle here wouldn\'t accept the
instructions shown in Oshpark\'s .cam file for Eagle, unfortunantly.
I had no luck getting a file or files from them that specified drill size &
drill location. The idea being to write a program to translate the .drl & .drd
files generated here to the form accepted by Oshpark\'s web site.
I\'m hoping someone here who has used Oshpark (or 4pcb.com?) will send me a
Gerber file(s) or portion thereof that specifies drill size & drill location
to serve as a model for the above mentioned translater. A complete gerber .zip
file, if convenient, would serve as well. Also, it needn\'t be generated by
Eagle but just be in accordance with the Gerber specs.
That could be sent to me via email at g...@rs-big-print.com with the gerber
file(s) attached or placed in the message itself as shown below. [Warning -
anything sent to the h...@panix.com email address shown here would be flushed.]
Or it could be added to a usenet message, as shown below.

Hul

; gpsallp.drl diameters of drill
T01 0.020in
T02 0.032in
T03 0.035in
T04 0.040in
T05 0.055in
T06 0.056in
T07 0.070in
T08 0.140in
T09 0.193in

Are your drill sizes the drill size or the finished hole size? Remember that plating adds to (or subtracts from actually) the hole size. I believe a half oz plating is common, so a full oz inside the hole or -0.0014 inches/-0.035 mm smaller opening.

--

Rick C.

- Get 1,000 miles of free Supercharging
- Tesla referral code - https://ts.la/richard11209

 

[Hul Tytus]

The files Eagle here is producing is in, or stated to be in, Excellon format and the
files shown in my message are the result. The question seems to be what exactly is Oshpark
seeking. That\'s why I\'d like to see some files that Oshpark is happy with.

Hul

Ed Lee <edward.ming.lee@gmail.com> wrote:

On Saturday, February 26, 2022 at 7:46:42 AM UTC-8, Hul Tytus wrote:
Ospark.com\'s quote section took a gerber .zip file (generated by Eagle
version 3.5) and stated that the .drl file was \"not a valid drill file\" and
the .drd file \"did not contain tool size info\". Assuming for now that \"tool
size\" is synonamous with drill size. The Eagle here wouldn\'t accept the
instructions shown in Oshpark\'s .cam file for Eagle, unfortunantly.

Use Excellon Drill format, not Gerber.

Download a gerber viewer than can handle both. Import Gerber and export Excellon.

 

[Lasse Langwadt Christensen]

https://docs.oshpark.com/design-tools/eagle/
https://docs.oshpark.com/design-tools/eagle/generating-gerbers/

 

[Hul Tytus]

Thanks Johann. The .xln file suffix is what\'s shown in Oshpark\'s .cam file
and the combining of drill size & location fits. The M48 code I haven\'t seen
before. Does that relate to other files? Stated differently, what\'s a
\"part program header\"? The M72 code seems familiar. What you\'ve shown is enough
to translate the files here for a try on Oshpark\'s web site.

Hul

Johann Klammer <klammerj@nospam.a1.net> wrote:

Unsure if this applies to your problem:
here\'s the start of some drill file for JLCPCBs CAM job
(the tool sizes are prepended to the drill insns inside the same file)
also:

M48 Defines the start of an M48 part program header
M72 ??? Inch Measuring Mode

minimum.XLN:

%
M48
M72
T01C0.0120
T02C0.0360
T03C0.1260
%
T01
X5585Y3473
X6835Y3473
X7585Y3723
X8585Y4223
X9085Y4723
X8835Y5223
X9335Y5973
X9835Y6223
X10335Y5723
[...]

 

[Hul Tytus]

The drill sizes shown are drill sizes not hole sizes. That\'s usually stated
in a readme file, but I suspect that\'s seldom read these days.

Hul

Rick C <gnuarm.deletethisbit@gmail.com> wrote:

On Saturday, February 26, 2022 at 10:46:42 AM UTC-5, Hul Tytus wrote:
Ospark.com\'s quote section took a gerber .zip file (generated by Eagle
version 3.5) and stated that the .drl file was \"not a valid drill file\" and
the .drd file \"did not contain tool size info\". Assuming for now that \"tool
size\" is synonamous with drill size. The Eagle here wouldn\'t accept the
instructions shown in Oshpark\'s .cam file for Eagle, unfortunantly.
I had no luck getting a file or files from them that specified drill size &
drill location. The idea being to write a program to translate the .drl & .drd
files generated here to the form accepted by Oshpark\'s web site.
I\'m hoping someone here who has used Oshpark (or 4pcb.com?) will send me a
Gerber file(s) or portion thereof that specifies drill size & drill location
to serve as a model for the above mentioned translater. A complete gerber .zip
file, if convenient, would serve as well. Also, it needn\'t be generated by
Eagle but just be in accordance with the Gerber specs.
That could be sent to me via email at g...@rs-big-print.com with the gerber
file(s) attached or placed in the message itself as shown below. [Warning -
anything sent to the h...@panix.com email address shown here would be flushed.]
Or it could be added to a usenet message, as shown below.

Hul

; gpsallp.drl diameters of drill
T01 0.020in
T02 0.032in
T03 0.035in
T04 0.040in
T05 0.055in
T06 0.056in
T07 0.070in
T08 0.140in
T09 0.193in

Are your drill sizes the drill size or the finished hole size? Remember that plating adds to (or subtracts from actually) the hole size. I believe a half oz plating is common, so a full oz inside the hole or -0.0014 inches/-0.035 mm smaller opening.

--

Rick C.

- Get 1,000 miles of free Supercharging
- Tesla referral code - https://ts.la/richard11209

 

[Rick C]

On Saturday, February 26, 2022 at 5:57:00 PM UTC-5, Hul Tytus wrote:

Rick C <gnuarm.del...@gmail.com> wrote:
On Saturday, February 26, 2022 at 10:46:42 AM UTC-5, Hul Tytus wrote:
Ospark.com\'s quote section took a gerber .zip file (generated by Eagle
version 3.5) and stated that the .drl file was \"not a valid drill file\" and
the .drd file \"did not contain tool size info\". Assuming for now that \"tool
size\" is synonamous with drill size. The Eagle here wouldn\'t accept the
instructions shown in Oshpark\'s .cam file for Eagle, unfortunantly.
I had no luck getting a file or files from them that specified drill size &
drill location. The idea being to write a program to translate the .drl & .drd
files generated here to the form accepted by Oshpark\'s web site.
I\'m hoping someone here who has used Oshpark (or 4pcb.com?) will send me a
Gerber file(s) or portion thereof that specifies drill size & drill location
to serve as a model for the above mentioned translater. A complete gerber .zip
file, if convenient, would serve as well. Also, it needn\'t be generated by
Eagle but just be in accordance with the Gerber specs.
That could be sent to me via email at g...@rs-big-print.com with the gerber
file(s) attached or placed in the message itself as shown below. [Warning -
anything sent to the h...@panix.com email address shown here would be flushed.]
Or it could be added to a usenet message, as shown below.

Hul

; gpsallp.drl diameters of drill
T01 0.020in
T02 0.032in
T03 0.035in
T04 0.040in
T05 0.055in
T06 0.056in
T07 0.070in
T08 0.140in
T09 0.193in

Are your drill sizes the drill size or the finished hole size? Remember that plating adds to (or subtracts from actually) the hole size. I believe a half oz plating is common, so a full oz inside the hole or -0.0014 inches/-0.035 mm smaller opening.

The drill sizes shown are drill sizes not hole sizes. That\'s usually stated
in a readme file, but I suspect that\'s seldom read these days.

Don\'t assume no one reads your readme file. I am often asked questions about my boards and if they don\'t find the readme file they always complain about that.

Your files are not the format they are expecting. It is meaningless to say \"Excellon\" format, because there is no Excellon standard. Excellon Automation is a company that makes equipment and they use various formats for their various equipment. Gerber was the same way, but to avoid all the confusion a standards body formalized it as RS-274X for the most recent and most widely used version.

After doing your searching for you, I found that Excellon 2 format is a superset of an IPC format spec.

https://en.wikipedia.org/wiki/PCB_NC_formats#Excellon_format

The specification provided by Excellon Automation has \"issues\" and can not be used without problems. I use gerbv to view Gerber files and drill files.. This program is very picky and typically finds fault with the drill files produced by the layout tool I use, however, it displays the drill holes with the Gerber files, so good enough.

Try loading your drill file(s) into gerbv and see if it accepts that format.. Otherwise, I suggest you find an Eagle forum and ask others there how they work around the problem.

I\'m curious, so I will ask about this in a forum for FreePCB that I use. It\'s a good group of people... mostly. lol

--

Rick C.

+ Get 1,000 miles of free Supercharging
+ Tesla referral code - https://ts.la/richard11209

 

[Rick C]

Here is a drill file from FreePCB

;Holesize 1 = 10.0 MILS
;Holesize 2 = 40.0 MILS
;Holesize 3 = 47.0 MILS
;Holesize 4 = 33.0 MILS
;Holesize 5 = 100.0 MILS
M48
INCH,00.0000
T01C0.010
T02C0.040
T03C0.047
T04C0.033
T05C0.100
%
G05
G90
T01
X006461Y005374
X002942Y003838
X006333Y003966
X002933Y003444
....

Gerbv complains about the INCH command...
\"Found junk after INCH command.\"

I seem to recall digging into that error before and never got a resolution.

--

Rick C.

-- Get 1,000 miles of free Supercharging
-- Tesla referral code - https://ts.la/richard11209

 

[Johann Klammer]

On 02/26/2022 11:53 PM, Hul Tytus wrote:

Thanks Johann. The .xln file suffix is what\'s shown in Oshpark\'s .cam file
and the combining of drill size & location fits. The M48 code I haven\'t seen
before. Does that relate to other files? Stated differently, what\'s a
\"part program header\"? The M72 code seems familiar. What you\'ve shown is enough
to translate the files here for a try on Oshpark\'s web site.

Hul

Oh, yes it\'s excellon format, like lee said.
The codes I found on wikipedia/internet archive..
The file itself was output by an old eagle version(6.5.0).
the boardhouses typically provide you with cam scripts. go look for those.

 

[Johann Klammer]

It\'s of course possible that the autodesk types broke it in the meantime.
And then there\'s the stuff the standards people sometimes do, not sticking
to established best practices but introducing incompatibilities
to maximize their sales.

 

[Hul Tytus]

I\'ve looked at some of those but it\'s mostly a duplicate Eagle
with numerous examples, which can be useful. Unfortunantly,
they don\'t show the Eagle version used here.
What I\'m looking for is gerber files that Oshpark is happy with.
The info Johann Klamm (sp?) posted on the drill files served
very well and Oshpark acceptes the drill files that have been
altered in accordance with Johann\'s data.
But, Oshpark doesn\'t like the outline in the .ref file. That
requires another Gerber file that has an outline that Oshpark
accepts!

Hul

Lasse Langwadt Christensen <langwadt@fonz.dk> wrote:

https://docs.oshpark.com/design-tools/eagle/
https://docs.oshpark.com/design-tools/eagle/generating-gerbers/

 

[Hul Tytus]

Johann - the data you posted did the trick and Oshpark is now accepting
the drill file. But they can\'t find an outline. I had thought that an
outline in a .ref file would work but it doesn\'t. Do you have file with an
outline that you could post here? Would be appreciated if possible.
Just guessing for now that Oshpark opens the .ref file and looks for a
Gerber code announcing an outline. And possibly that is a modern Gerber
code not included the .ref files the Eagle here is generating.

Hul


Johann Klammer <klammerj@nospam.a1.net> wrote:

On 02/26/2022 11:53 PM, Hul Tytus wrote:
Thanks Johann. The .xln file suffix is what\'s shown in Oshpark\'s .cam file
and the combining of drill size & location fits. The M48 code I haven\'t seen
before. Does that relate to other files? Stated differently, what\'s a
\"part program header\"? The M72 code seems familiar. What you\'ve shown is enough
to translate the files here for a try on Oshpark\'s web site.

Hul

Oh, yes it\'s excellon format, like lee said.
The codes I found on wikipedia/internet archive..
The file itself was output by an old eagle version(6.5.0).
the boardhouses typically provide you with cam scripts. go look for those.

 

[Hul Tytus]

Rick - thanks for the drill file below. The altered drill file (no longer files) here
is working but I\'ll keep your code on record in case of trouble with another pcb maker.
The remaining problem is supplying Oshpark with an outline. I had thought a .ref file
with an outline would work but it didnt. I\'m guessing a Gerber code of some sort is needed
to mark the outline. Once again a Gerber file with an outline accepted by Oshpark is
needed.

Hul

Rick C <gnuarm.deletethisbit@gmail.com> wrote:

Here is a drill file from FreePCB

;Holesize 1 = 10.0 MILS
;Holesize 2 = 40.0 MILS
;Holesize 3 = 47.0 MILS
;Holesize 4 = 33.0 MILS
;Holesize 5 = 100.0 MILS
M48
INCH,00.0000
T01C0.010
T02C0.040
T03C0.047
T04C0.033
T05C0.100
%
G05
G90
T01
X006461Y005374
X002942Y003838
X006333Y003966
X002933Y003444
...

Gerbv complains about the INCH command...
\"Found junk after INCH command.\"

I seem to recall digging into that error before and never got a resolution.

--

Rick C.

-- Get 1,000 miles of free Supercharging
-- Tesla referral code - https://ts.la/richard11209

 

[Lasse Langwadt Christensen]

søndag den 27. februar 2022 kl. 14.56.54 UTC+1 skrev Hul Tytus:

Rick - thanks for the drill file below. The altered drill file (no longer files) here
is working but I\'ll keep your code on record in case of trouble with another pcb maker.
The remaining problem is supplying Oshpark with an outline. I had thought a .ref file
with an outline would work but it didnt. I\'m guessing a Gerber code of some sort is needed
to mark the outline. Once again a Gerber file with an outline accepted by Oshpark is
needed.
Hul

tried renaming it to .gko ?

 

[Hul Tytus]

Lasse - tried renaming the file with the outline .gko and it
didn\'t work but Oshpark looked which is changing in the right
direction. Oshpark said roughly \"the .gko file is not a valid
Gerber outline\".
I\'m hoping you have a .gko file that has worked and you would
post a copy here. That would then be used as a model for generating
the outline for a .gko to go with the Eagle here.

Hul

Lasse Langwadt Christensen <langwadt@fonz.dk> wrote:

s??ndag den 27. februar 2022 kl. 14.56.54 UTC+1 skrev Hul Tytus:
Rick - thanks for the drill file below. The altered drill file (no longer files) here
is working but I\'ll keep your code on record in case of trouble with another pcb maker.
The remaining problem is supplying Oshpark with an outline. I had thought a .ref file
with an outline would work but it didnt. I\'m guessing a Gerber code of some sort is needed
to mark the outline. Once again a Gerber file with an outline accepted by Oshpark is
needed.
Hul


tried renaming it to .gko ?

 

[Rick C]

This file seems a bit more complex than needed.

On Sunday, February 27, 2022 at 4:21:56 PM UTC-5, Hul Tytus wrote:

Lasse - tried renaming the file with the outline .gko and it
didn\'t work but Oshpark looked which is changing in the right
direction. Oshpark said roughly \"the .gko file is not a valid
Gerber outline\".
I\'m hoping you have a .gko file that has worked and you would
post a copy here. That would then be used as a model for generating
the outline for a .gko to go with the Eagle here.
Hul

G04 FreePCB MFC Application*
G04 Version: FreePCB--481036337*
G04 WebSite: www.freepcb.dev*
G04 C:\\Arius\\Boards_new\\TDC_upgrade\\Layout\\TestFreePCB2\\CAM(MS-DCARD_2-1)(2-26-2022)\\BOARD_OUTLINE.gbr*
G04 board outline layer *
G04 Scale: 100 percent, Rotated: No, Reflected: No *
%FSLAX24Y24*%
%MOIN*%
%LN board outline *%
G04 Rounded Rectangle Macro, params: W/2, H/2, R *
%AMRNDREC*
21,1,$1+$1,$2+$2-$3-$3,0,0,0*
21,1,$1+$1-$3-$3,$2+$2,0,0,0*
1,1,$3+$3,$1-$3,$2-$3*
1,1,$3+$3,$3-$1,$2-$3*
1,1,$3+$3,$1-$3,$3-$2*
1,1,$3+$3,$3-$1,$3-$2*%
G04 Rectangular Thermal Macro, params: W/4, H/4, TW/4, TC/4 *
%AMRECTHERM*
21,1,$1+$1-$3-$3-$4-$4,$2+$2-$3-$3-$4-$4-$4-$4,0-$1-$3-$4,0-$2-$3,0*
21,1,$1+$1-$3-$3-$4-$4-$4-$4,$2+$2-$3-$3-$4-$4,0-$1-$3,0-$2-$3-$4,0*
1,1,$4+$4+$4+$4,0-$1-$1+$4+$4,0-$2-$2+$4+$4*
1,1,$4+$4+$4+$4,0-$1-$1+$4+$4,0-$3-$3-$4-$4*
1,1,$4+$4+$4+$4,0-$3-$3-$4-$4,0-$2-$2+$4+$4*
21,1,$1+$1-$3-$3-$4-$4,$2+$2-$3-$3-$4-$4-$4-$4,0-$1-$3-$4,$2+$3,0*
21,1,$1+$1-$3-$3-$4-$4-$4-$4,$2+$2-$3-$3-$4-$4,0-$1-$3,$2+$3+$4,0*
1,1,$4+$4+$4+$4,0-$1-$1+$4+$4,$2+$2-$4-$4*
1,1,$4+$4+$4+$4,0-$1-$1+$4+$4,$3+$3+$4+$4*
1,1,$4+$4+$4+$4,0-$3-$3-$4-$4,$2+$2-$4-$4*
21,1,$1+$1-$3-$3-$4-$4,$2+$2-$3-$3-$4-$4-$4-$4,$1+$3+$4,0-$2-$3,0*
21,1,$1+$1-$3-$3-$4-$4-$4-$4,$2+$2-$3-$3-$4-$4,$1+$3,0-$2-$3-$4,0*
1,1,$4+$4+$4+$4,$1+$1-$4-$4,0-$2-$2+$4+$4*
1,1,$4+$4+$4+$4,$1+$1-$4-$4,0-$3-$3-$4-$4*
1,1,$4+$4+$4+$4,$3+$3+$4+$4,0-$2-$2+$4+$4*
21,1,$1+$1-$3-$3-$4-$4,$2+$2-$3-$3-$4-$4-$4-$4,$1+$3+$4,$2+$3,0*
21,1,$1+$1-$3-$3-$4-$4-$4-$4,$2+$2-$3-$3-$4-$4,$1+$3,$2+$3+$4,0*
1,1,$4+$4+$4+$4,$1+$1-$4-$4,$2+$2-$4-$4*
1,1,$4+$4+$4+$4,$1+$1-$4-$4,$3+$3+$4+$4*
1,1,$4+$4+$4+$4,$3+$3+$4+$4,$2+$2-$4-$4*%
%AMRECTHERM_45*
21,1,$1+$1+$1+$1,$2+$2+$2+$2-$4-$4-$4-$4-$4-$4-$4-$4-$4-$4-$3-$3,0,0,0*
21,1,$1+$1+$1+$1-$4-$4-$4-$4-$4-$4-$4-$4-$4-$4-$3-$3,$2+$2+$2+$2,0,0,0*
1,1,$4+$4+$4+$4,$1+$1-$4-$4,$2+$2-$4-$4-$4-$4-$4-$3*
1,1,$4+$4+$4+$4,$1+$1-$4-$4,0-$2-$2+$4+$4+$4+$4+$4+$3*
1,1,$4+$4+$4+$4,$1+$1-$4-$4-$4-$4-$4-$3,$2+$2-$4-$4*
1,1,$4+$4+$4+$4,0-$1-$1+$4+$4+$4+$4+$4+$3,$2+$2-$4-$4*
1,1,$4+$4+$4+$4,0-$1-$1+$4+$4,$2+$2-$4-$4-$4-$4-$4-$3*
1,1,$4+$4+$4+$4,0-$1-$1+$4+$4,0-$2-$2+$4+$4+$4+$4+$4+$3*
1,1,$4+$4+$4+$4,$1+$1-$4-$4-$4-$4-$4-$3,0-$2-$2+$4+$4*
1,1,$4+$4+$4+$4,0-$1-$1+$4+$4+$4+$4+$4+$3,0-$2-$2+$4+$4*%
%ADD10C,0.010000*%
G90*
G70D02*
G04 begin color: clBlack*
%LPD*%

G04 Step and Repeat for panelization *

G04 ----------------------- Draw board outline (positive)*

G04 -------------- Draw Parts, Pads, Traces, Vias and Text (positive)*

G04 Draw traces*

G04 Draw Text*
G54D10*
G01X0Y0D02*
G01X45275Y0D01*
G01X45275Y8503D01*
G01X0Y8503D01*
G01X0Y0D01*
M00*
M02*

Lasse Langwadt Christensen <lang...@fonz.dk> wrote:
s??ndag den 27. februar 2022 kl. 14.56.54 UTC+1 skrev Hul Tytus:
Rick - thanks for the drill file below. The altered drill file (no longer files) here
is working but I\'ll keep your code on record in case of trouble with another pcb maker.
The remaining problem is supplying Oshpark with an outline. I had thought a .ref file
with an outline would work but it didnt. I\'m guessing a Gerber code of some sort is needed
to mark the outline. Once again a Gerber file with an outline accepted by Oshpark is
needed.
Hul


tried renaming it to .gko ?

Can you post your file so we can see what it contains?

And I again, ask that you not top post. Makes it hard to read when the rest of us use bottom posting.

--

Rick C.

+- Get 1,000 miles of free Supercharging
+- Tesla referral code - https://ts.la/richard11209

 

[Johann Klammer]

On 02/27/2022 10:21 PM, Hul Tytus wrote:

Lasse - tried renaming the file with the outline .gko and it
didn\'t work but Oshpark looked which is changing in the right
direction. Oshpark said roughly \"the .gko file is not a valid
Gerber outline\".
I\'m hoping you have a .gko file that has worked and you would
post a copy here. That would then be used as a model for generating
the outline for a .gko to go with the Eagle here.

Hul

Lasse Langwadt Christensen <langwadt@fonz.dk> wrote:
s??ndag den 27. februar 2022 kl. 14.56.54 UTC+1 skrev Hul Tytus:
Rick - thanks for the drill file below. The altered drill file (no longer files) here
is working but I\'ll keep your code on record in case of trouble with another pcb maker.
The remaining problem is supplying Oshpark with an outline. I had thought a .ref file
with an outline would work but it didnt. I\'m guessing a Gerber code of some sort is needed
to mark the outline. Once again a Gerber file with an outline accepted by Oshpark is
needed.
Hul


tried renaming it to .gko ?

try creating annew project and paint the outline as a 6 mil trace in the top copper layer
generate gerbers and rename the top layer file to gko.

(or does eagle 3.5 allow creating a layer named outline? what exactly can it do?)

 

[Hul Tytus]

Thanks Rick. I\'ll give that a try with just the apparantly
needed code. I\'ll let you know what happens.

Hul

Rick C <gnuarm.deletethisbit@gmail.com> wrote:

This file seems a bit more complex than needed.

On Sunday, February 27, 2022 at 4:21:56 PM UTC-5, Hul Tytus wrote:
Lasse - tried renaming the file with the outline .gko and it
didn\'t work but Oshpark looked which is changing in the right
direction. Oshpark said roughly \"the .gko file is not a valid
Gerber outline\".
I\'m hoping you have a .gko file that has worked and you would
post a copy here. That would then be used as a model for generating
the outline for a .gko to go with the Eagle here.
Hul
G04 FreePCB MFC Application*
G04 Version: FreePCB--481036337*
G04 WebSite: www.freepcb.dev*
G04 C:\\Arius\\Boards_new\\TDC_upgrade\\Layout\\TestFreePCB2\\CAM(MS-DCARD_2-1)(2-26-2022)\\BOARD_OUTLINE.gbr*
G04 board outline layer *
G04 Scale: 100 percent, Rotated: No, Reflected: No *
%FSLAX24Y24*%
%MOIN*%
%LN board outline *%
G04 Rounded Rectangle Macro, params: W/2, H/2, R *
%AMRNDREC*
21,1,$1+$1,$2+$2-$3-$3,0,0,0*
21,1,$1+$1-$3-$3,$2+$2,0,0,0*
1,1,$3+$3,$1-$3,$2-$3*
1,1,$3+$3,$3-$1,$2-$3*
1,1,$3+$3,$1-$3,$3-$2*
1,1,$3+$3,$3-$1,$3-$2*%
G04 Rectangular Thermal Macro, params: W/4, H/4, TW/4, TC/4 *
%AMRECTHERM*
21,1,$1+$1-$3-$3-$4-$4,$2+$2-$3-$3-$4-$4-$4-$4,0-$1-$3-$4,0-$2-$3,0*
21,1,$1+$1-$3-$3-$4-$4-$4-$4,$2+$2-$3-$3-$4-$4,0-$1-$3,0-$2-$3-$4,0*
1,1,$4+$4+$4+$4,0-$1-$1+$4+$4,0-$2-$2+$4+$4*
1,1,$4+$4+$4+$4,0-$1-$1+$4+$4,0-$3-$3-$4-$4*
1,1,$4+$4+$4+$4,0-$3-$3-$4-$4,0-$2-$2+$4+$4*
21,1,$1+$1-$3-$3-$4-$4,$2+$2-$3-$3-$4-$4-$4-$4,0-$1-$3-$4,$2+$3,0*
21,1,$1+$1-$3-$3-$4-$4-$4-$4,$2+$2-$3-$3-$4-$4,0-$1-$3,$2+$3+$4,0*
1,1,$4+$4+$4+$4,0-$1-$1+$4+$4,$2+$2-$4-$4*
1,1,$4+$4+$4+$4,0-$1-$1+$4+$4,$3+$3+$4+$4*
1,1,$4+$4+$4+$4,0-$3-$3-$4-$4,$2+$2-$4-$4*
21,1,$1+$1-$3-$3-$4-$4,$2+$2-$3-$3-$4-$4-$4-$4,$1+$3+$4,0-$2-$3,0*
21,1,$1+$1-$3-$3-$4-$4-$4-$4,$2+$2-$3-$3-$4-$4,$1+$3,0-$2-$3-$4,0*
1,1,$4+$4+$4+$4,$1+$1-$4-$4,0-$2-$2+$4+$4*
1,1,$4+$4+$4+$4,$1+$1-$4-$4,0-$3-$3-$4-$4*
1,1,$4+$4+$4+$4,$3+$3+$4+$4,0-$2-$2+$4+$4*
21,1,$1+$1-$3-$3-$4-$4,$2+$2-$3-$3-$4-$4-$4-$4,$1+$3+$4,$2+$3,0*
21,1,$1+$1-$3-$3-$4-$4-$4-$4,$2+$2-$3-$3-$4-$4,$1+$3,$2+$3+$4,0*
1,1,$4+$4+$4+$4,$1+$1-$4-$4,$2+$2-$4-$4*
1,1,$4+$4+$4+$4,$1+$1-$4-$4,$3+$3+$4+$4*
1,1,$4+$4+$4+$4,$3+$3+$4+$4,$2+$2-$4-$4*%
%AMRECTHERM_45*
21,1,$1+$1+$1+$1,$2+$2+$2+$2-$4-$4-$4-$4-$4-$4-$4-$4-$4-$4-$3-$3,0,0,0*
21,1,$1+$1+$1+$1-$4-$4-$4-$4-$4-$4-$4-$4-$4-$4-$3-$3,$2+$2+$2+$2,0,0,0*
1,1,$4+$4+$4+$4,$1+$1-$4-$4,$2+$2-$4-$4-$4-$4-$4-$3*
1,1,$4+$4+$4+$4,$1+$1-$4-$4,0-$2-$2+$4+$4+$4+$4+$4+$3*
1,1,$4+$4+$4+$4,$1+$1-$4-$4-$4-$4-$4-$3,$2+$2-$4-$4*
1,1,$4+$4+$4+$4,0-$1-$1+$4+$4+$4+$4+$4+$3,$2+$2-$4-$4*
1,1,$4+$4+$4+$4,0-$1-$1+$4+$4,$2+$2-$4-$4-$4-$4-$4-$3*
1,1,$4+$4+$4+$4,0-$1-$1+$4+$4,0-$2-$2+$4+$4+$4+$4+$4+$3*
1,1,$4+$4+$4+$4,$1+$1-$4-$4-$4-$4-$4-$3,0-$2-$2+$4+$4*
1,1,$4+$4+$4+$4,0-$1-$1+$4+$4+$4+$4+$4+$3,0-$2-$2+$4+$4*%
%ADD10C,0.010000*%
G90*
G70D02*
G04 begin color: clBlack*
%LPD*%

G04 Step and Repeat for panelization *

G04 ----------------------- Draw board outline (positive)*

G04 -------------- Draw Parts, Pads, Traces, Vias and Text (positive)*

G04 Draw traces*

G04 Draw Text*
G54D10*
G01X0Y0D02*
G01X45275Y0D01*
G01X45275Y8503D01*
G01X0Y8503D01*
G01X0Y0D01*
M00*
M02*

Lasse Langwadt Christensen <lang...@fonz.dk> wrote:
s??ndag den 27. februar 2022 kl. 14.56.54 UTC+1 skrev Hul Tytus:
Rick - thanks for the drill file below. The altered drill file (no longer files) here
is working but I\'ll keep your code on record in case of trouble with another pcb maker.
The remaining problem is supplying Oshpark with an outline. I had thought a .ref file
with an outline would work but it didnt. I\'m guessing a Gerber code of some sort is needed
to mark the outline. Once again a Gerber file with an outline accepted by Oshpark is
needed.
Hul


tried renaming it to .gko ?

Can you post your file so we can see what it contains?

And I again, ask that you not top post. Makes it hard to read when the rest of us use bottom posting.

--

Rick C.

+- Get 1,000 miles of free Supercharging
+- Tesla referral code - https://ts.la/richard11209