Just mailed two designs to Eurocircuits this afternoon made by Eagle V6.
Received a reject as 'does not look to be a valid .brd file'.
I wonder if they know about the changes in V6?
Robert
Just mailed two designs to Eurocircuits this afternoon made by Eagle V6.
Received a reject as 'does not look to be a valid .brd file'.
I wonder if they know about the changes in V6?
Robert
Robert <robert@nospam.ch> wrote:
Just mailed two designs to Eurocircuits this afternoon made by Eagle V6.
Received a reject as 'does not look to be a valid .brd file'.
I wonder if they know about the changes in V6?
The new version is out only some two weeks. Give them some time. Board review
for eurocircuit is in India to my knowledge, so perhaps even some more time
is needed.
Also think about delivering Gerber RS2xx. That way, data is fixed and not
subject to subtile differences in setup.
Bye
--
Uwe Bonnes bon@elektron.ikp.physik.tu-darmstadt.de
Institut fuer Kernphysik Schlossgartenstrasse 9 64289 Darmstadt
-
Tel. 06151 162516 -
Fax. 06151 164321 -
On 22/12/2011 21:13, Uwe Bonnes wrote:
Robert<robert@nospam.ch> wrote:
>> Just mailed two designs to Eurocircuits this afternoon made by Eagle V6.
>> Received a reject as 'does not look to be a valid .brd file'.
>> I wonder if they know about the changes in V6?
The new version is out only some two weeks. Give them some time. Board review
for eurocircuit is in India to my knowledge, so perhaps even some more time
is needed.
Also think about delivering Gerber RS2xx. That way, data is fixed and not
subject to subtile differences in setup.
Bye
Hmm, that will likely stop it solid. Altough Eurocircuits did build good
boards based on .brd files for me in the past. Not having generated
Gerber files at all, I will have some reading to do, as we want to build
prototypes for customers in a few weeks. This is the moment where I
regret to have upgraded to V6 early.
In the online help, 'GERBER' does not do much, but I saw a gerber.cam
file. Should the result be a collection of files, like a drill file etc?
Cancelling and trying another board house right now might get me in the
same problem again.
Robert
On 22/12/2011 22:02, Robert wrote:
On 22/12/2011 21:13, Uwe Bonnes wrote:
>> Robert<robert@nospam.ch> wrote:
>>> Just mailed two designs to Eurocircuits this afternoon made by Eagle V6.
>>> Received a reject as 'does not look to be a valid .brd file'.
>>> I wonder if they know about the changes in V6?
>>
>> The new version is out only some two weeks. Give them some time. Board
>> review
>> for eurocircuit is in India to my knowledge, so perhaps even some more
>> time
>> is needed.
>>
>> Also think about delivering Gerber RS2xx. That way, data is fixed and not
>> subject to subtile differences in setup.
>>
>> Bye
Hmm, that will likely stop it solid. Altough Eurocircuits did build good
boards based on .brd files for me in the past. Not having generated
Gerber files at all, I will have some reading to do, as we want to build
prototypes for customers in a few weeks. This is the moment where I
regret to have upgraded to V6 early.
In the online help, 'GERBER' does not do much, but I saw a gerber.cam
file. Should the result be a collection of files, like a drill file etc?
Cancelling and trying another board house right now might get me in the
same problem again.
Robert
Well, that did not look that hard. Found the instructions, generated
drill file and a 4-layer Gerber, zipped them up and updated my order.
Hopefully that was the right way.
Robert
>>
>> Robert
>>
Well, that did not look that hard. Found the instructions, generated
drill file and a 4-layer Gerber, zipped them up and updated my order.
Hopefully that was the right way.
Robert
>
It is very important to verify that all the necessary files are there,
contain the correct layers and are not mirrored.
Robert wrote:
On 22/12/2011 21:13, Uwe Bonnes wrote:
>> Robert<robert@nospam.ch> wrote:
>>> Just mailed two designs to Eurocircuits this afternoon made by
>>> Eagle V6. Received a reject as 'does not look to be a valid .brd
>>> file'.
>>> I wonder if they know about the changes in V6?
>>
>> The new version is out only some two weeks. Give them some time.
>> Board review for eurocircuit is in India to my knowledge, so perhaps
>> even some more time is needed.
>>
>> Also think about delivering Gerber RS2xx. That way, data is fixed
>> and not subject to subtile differences in setup.
>>
>> Bye
Hmm, that will likely stop it solid. Altough Eurocircuits did build
good boards based on .brd files for me in the past. Not having
generated Gerber files at all, I will have some reading to do, as we
want to build prototypes for customers in a few weeks. This is the
moment where I regret to have upgraded to V6 early.
In the online help, 'GERBER' does not do much, but I saw a gerber.cam
file. Should the result be a collection of files, like a drill file
etc?
Cancelling and trying another board house right now might get me in
the same problem again.
Robert
Review the tutorial that ships with Eagle, found in the DOCs folder.
Section: Output of drawings and manufacturing data.
Gerber is simple and nothing to be affraid of. Note a drill file will need
generating as well as the multiple files for the layers considerd Gerber.
Before shipping gerbers, view them yourself. using a viewer. GC-Prevue and
gerbv are a couple to try.
It also helps if you understand the order of the process steps the
manufacturer uses. That way you don't flipout when you view a Gerber copper
layer with no holes depicted.
Eurocircuits have a page
All the best
Warren
--
Viewed / responded via the newsgroup at
news.cadsoft.de
On 22/12/2011 23:17, Warren Brayshaw wrote:
It also helps if you understand the order of the process steps the
manufacturer uses. That way you don't flipout when you view a Gerber copper
layer with no holes depicted.
Eurocircuits have a page
>
All the best
Warren
>
Warren, thank you, that is a page I should have read first. Anyway, I
think I followed the rules and submitted what was needed. The result
will tell.
Best wishes for Chrismas and the new year.
Regards, Robert
Hi Robert,
Have a look here:
http://www.eurocircuits.fr/images/stories/ec09/ec-design-guidelines-englsih-1-2010-v3.pdf
They describe the data formats they accept.
And this one
http://eurocircuits.info/phpBB3/download/EC-Eagle-Guidelines-ENGLISH-1-2010-V1.pdf
on how to create Gerber files using Eagle.
There's no difference between version 5 and 6
"Robert" schreef in bericht news:jd0951$glu$1@cheetah.cadsoft.de...
On 22/12/2011 22:02, Robert wrote:
On 22/12/2011 21:13, Uwe Bonnes wrote:
>> Robert<robert@nospam.ch> wrote:
>>> Just mailed two designs to Eurocircuits this afternoon made by Eagle V6.
>>> Received a reject as 'does not look to be a valid .brd file'.
>>> I wonder if they know about the changes in V6?
>>
>> The new version is out only some two weeks. Give them some time. Board
>> review
>> for eurocircuit is in India to my knowledge, so perhaps even some more
>> time
>> is needed.
>>
>> Also think about delivering Gerber RS2xx. That way, data is fixed and not
>> subject to subtile differences in setup.
>>
>> Bye
Hmm, that will likely stop it solid. Altough Eurocircuits did build good
boards based on .brd files for me in the past. Not having generated
Gerber files at all, I will have some reading to do, as we want to build
prototypes for customers in a few weeks. This is the moment where I
regret to have upgraded to V6 early.
In the online help, 'GERBER' does not do much, but I saw a gerber.cam
file. Should the result be a collection of files, like a drill file etc?
Cancelling and trying another board house right now might get me in the
same problem again.
Robert
Well, that did not look that hard. Found the instructions, generated
drill file and a 4-layer Gerber, zipped them up and updated my order.
Hopefully that was the right way.
Robert
Hello Robert,
We received your order at Eurocircuits.
We would like to draw your attention to the following message on the EAGLE-CADsoft website. It might be related to the problem you experienced.
--------------------------------------------------
WARNING: Most unfortunately, after the whole release process for version 6.0.0 had been finished, it turned out that there is a bug in the polygon handling of the CAM Processor.
If a board contains signal polygons that have their "Orphans" parameter set to "off", and the CAM Processor is used to generate production data with the "pos. Coord" (positive coordinates) option turned on, and if this actually leads to an offset in the CAM data, it can happen that parts of the signal polygons are not drawn, even though they are not orphans, and vice versa.
This may lead to missing electrical connections or copper in places where this is not intended.
As an immediate workaround you can turn the "pos. Coord" option off.
We are working on a solution for this and will release a fixed version as soon as possible.
Sorry for the inconvenience.
------------------------------------------
It is advisable to check any result before releasing your data.
If Gerbers are generated, these can be checked with an independent freeware Gerber viewer GCPrevue for example (www.graphicode.com).
Regards,
Luc
On 23/12/2011 16:44, luc.smets@gmail.com wrote:
Hello Robert,
We received your order at Eurocircuits.
We would like to draw your attention to the following message on the EAGLE-CADsoft website. It might be related to the problem you experienced.
--------------------------------------------------
WARNING: Most unfortunately, after the whole release process for version 6.0.0 had been finished, it turned out that there is a bug in the polygon handling of the CAM Processor.
If a board contains signal polygons that have their "Orphans" parameter set to "off", and the CAM Processor is used to generate production data with the "pos. Coord" (positive coordinates) option turned on, and if this actually leads to an offset in the CAM data, it can happen that parts of the signal polygons are not drawn, even though they are not orphans, and vice versa.
This may lead to missing electrical connections or copper in places where this is not intended.
As an immediate workaround you can turn the "pos. Coord" option off.
We are working on a solution for this and will release a fixed version as soon as possible.
Sorry for the inconvenience.
------------------------------------------
It is advisable to check any result before releasing your data.
If Gerbers are generated, these can be checked with an independent freeware Gerber viewer GCPrevue for example (www.graphicode.com (http://www.graphicode.com)).
Regards,
Luc
>
Thanks Luc, will do.
Robert
On 23/12/2011 09:24, Robert wrote:
On 22/12/2011 23:17, Warren Brayshaw wrote:
>> It also helps if you understand the order of the process steps the
>> manufacturer uses. That way you don't flipout when you view a Gerber
>> copper
>> layer with no holes depicted.
>> Eurocircuits have a page
>>
>>
>>
>> All the best
>> Warren
>>
>>
Warren, thank you, that is a page I should have read first. Anyway, I
think I followed the rules and submitted what was needed. The result
will tell.
Best wishes for Chrismas and the new year.
Regards, Robert
Well, the 4 layer boards came back with a layer missing. I used the ULP
to generate the Gerber files for a 4 layer board and send it to
Eurocircuits. When asking confirmation by mail, the answer was that it
would be processed as a 4 layer board.
I downloaded GC-Prevue, but can't make sense of it (it asks for file
extensions that are not part of the many Gerber files I created). The
HELP menu assumes that you know how to operate it.
Is there a document that describes how to open Gerber files in GC-Prevue?
Which board house accepts .BRD files of Eagle 6? I made 100+ boards this
way, never a problem.
Robert
Is there a document that describes how to open Gerber files in GC-Prevue?
To use GC Prevue, open the program, then go to File>Import and select
all of your gerber files and then you get a chance to select layer
colors etc.
Is there a document that describes how to open Gerber files in GC-Prevue?
To use GC Prevue, open the program, then go to File>Import and select
all of your gerber files and then you get a chance to select layer
colors etc.
On 13/01/2012 23:25, Doug wrote:
>>
>> Is there a document that describes how to open Gerber files in GC-Prevue?
>>
>
To use GC Prevue, open the program, then go to File>Import and select
all of your gerber files and then you get a chance to select layer
colors etc.
Doug, thanks. At least I see something, so I repeated the whole process:
Followed Eurocircuits guidelines for a 4 layer board:
- Ran CAM processor, selected gerb274x-4layer.cam, activated Dimension
in every layer.
- Processed the job
- Did the same for the drill file.
- Zipped it all up.
Imported the zip file in GC Prevue.
End up with 3 Hole/Rout layers (.dri, .drd, .gpi),
and 10 Unknown physical layers P1-P10 with extensions .pls, .plc, etc.
Displayed like:
Physical layers
(v)P1 Unknown "Qbus_V21.pls"
+(v)P1.1 "Qbus_V21.pls"[a001]
...
GC-Prevue reports 0 errors.
Would this be related to gerb274x-4layer.cam not being compatible with
Eagle V6?
Robert
Robert <Robert@nospam.ch> wrote:
On 13/01/2012 23:25, Doug wrote:
>>
>>>
>>> Is there a document that describes how to open Gerber files in GC-Prevue?
>>>
>>
>> To use GC Prevue, open the program, then go to File>Import and select
>> all of your gerber files and then you get a chance to select layer
>> colors etc.
>>
Doug, thanks. At least I see something, so I repeated the whole process:
Followed Eurocircuits guidelines for a 4 layer board:
- Ran CAM processor, selected gerb274x-4layer.cam, activated Dimension in every layer.
- Processed the job
- Did the same for the drill file.
- Zipped it all up.
Imported the zip file in GC Prevue.
End up with 3 Hole/Rout layers (.dri, .drd, .gpi),
and 10 Unknown physical layers P1-P10 with extensions .pls, .plc, etc.
Displayed like:
Physical layers
(v)P1 Unknown "Qbus_V21.pls"
+(v)P1.1 "Qbus_V21.pls"[a001]
...
GC-Prevue reports 0 errors.
Would this be related to gerb274x-4layer.cam not being compatible with Eagle V6?
Robert
Im curious, what layers did you draw om and what layers does the cam file
process?
I would not recommend using any cam file unless you really know how it
works.
Op Sat, 14 Jan 2012 10:29:52 +0100 schreef Robert <Robert@nospam.ch>:
On 13/01/2012 23:25, Doug wrote:
>>
>>>
>>> Is there a document that describes how to open Gerber files in
>>> GC-Prevue?
>>>
>>
>> To use GC Prevue, open the program, then go to File>Import and select
>> all of your gerber files and then you get a chance to select layer
>> colors etc.
>>
Doug, thanks. At least I see something, so I repeated the whole process:
Followed Eurocircuits guidelines for a 4 layer board:
- Ran CAM processor, selected gerb274x-4layer.cam, activated Dimension
in every layer.
- Processed the job
- Did the same for the drill file.
- Zipped it all up.
Imported the zip file in GC Prevue.
End up with 3 Hole/Rout layers (.dri, .drd, .gpi),
and 10 Unknown physical layers P1-P10 with extensions .pls, .plc, etc.
Displayed like:
Physical layers
(v)P1 Unknown "Qbus_V21.pls"
+(v)P1.1 "Qbus_V21.pls"[a001]
...
GC-Prevue reports 0 errors.
Would this be related to gerb274x-4layer.cam not being compatible with
Eagle V6?
Robert
>
Hello Robert,
You don't need to process the .dri file (= ASCII info file) or any of the
.GPI files (same). All drill info is contained within the .drd file, at
least when you use the EXCELLON drill device.
In the Eagle documentation (help > generating output) you can find what
the CAM extensions are used for:
-
File Layers Meaning
-
*.cmp Top, Via, Pad Component side
*.ly2 Route2, Via, Pad Inner signal layer
*.ly3 Route3, Via, Pad Inner signal layer
*.ly4 $User1 Inner supply layer
... ...
*.sol Bot, Via, Pad Solder side
*.plc tPl, Dim, tName, Silkscreen comp. side
*.pls bPl, Dim, bName, Silkscreen solder side
*.stc tStop Solder stop mask comp. side
*.sts bStop Solder stop mask sold. side
*.drd Drills, Holes Drill data for NC drill st.
-
The "unknown" layers in GC Prevue are just because you didn't gave them a
name. While importing you are given the chance to name the layer and
indicate it's purpose. 'signal', 'soldermask', etc. and 'top', 'bottom',
etc. are indicated in drop lists.
I don't think you should (need to) activate the dimension layer in every
layer. At least I don't. I make one layer that I call .fab, where the
'dimension' layer is included along with the 'drills' and 'holes' layer.
When you plot every layer with the GERBER_RS274X device you should import
them (as Doug said) as a "physical layer". The .drd file should be
imported as a "hole /rout layer". When 'autoguessing' the settings in the
drill file GC Prevue often get's it wrong. If hat happens, you'll see the
drills plotted in (totally) wrong places. Just delete the hole/rout layer
and the associated aperture file and start the import again. This time, in
the "Import - Verify File Information" window, right click on the NC drill
file and choose "Modify format parameters..." . look for the right
settings, especially "whole digits" (2), "precision" (4) and the right
format for the "embedded drill table units" (inches or mm).
remember that the way gerber files are made are a bit 'loose', meaning
things like file extensions are not defined (every program uses different
ones) and PCB manufacturers sometimes have different idea's of what should
be included in what layer and in what format. So it is always wise to see
if your intended PCB manufacturer has an explanation of how he expects
things and if not, give 'm a call.
That said, I've made hundred's of PCB's with different manufacturers and
never really had a problem. I've used GC Prevue for more than 10 years and
it always worked fine. As said, it sometimes only needs a little attention
when importing the drill file.
Good luck,
Richard
On 14/01/2012 14:35, Richard Herman wrote:
Hello Robert,
You don't need to process the .dri file (= ASCII info file) or any of
the .GPI files (same). All drill info is contained within the .drd file,
at least when you use the EXCELLON drill device.
In the Eagle documentation (help > generating output) you can find what
the CAM extensions are used for:
-------------------------------------------------------
File Layers Meaning
-------------------------------------------------------
*.cmp Top, Via, Pad Component side
*.ly2 Route2, Via, Pad Inner signal layer
*.ly3 Route3, Via, Pad Inner signal layer
*.ly4 $User1 Inner supply layer
... ...
*.sol Bot, Via, Pad Solder side
*.plc tPl, Dim, tName, Silkscreen comp. side
*.pls bPl, Dim, bName, Silkscreen solder side
*.stc tStop Solder stop mask comp. side
*.sts bStop Solder stop mask sold. side
*.drd Drills, Holes Drill data for NC drill st.
-------------------------------------------------------
The "unknown" layers in GC Prevue are just because you didn't gave them
a name. While importing you are given the chance to name the layer and
indicate it's purpose. 'signal', 'soldermask', etc. and 'top', 'bottom',
etc. are indicated in drop lists.
I don't think you should (need to) activate the dimension layer in every
layer. At least I don't. I make one layer that I call .fab, where the
'dimension' layer is included along with the 'drills' and 'holes' layer.
When you plot every layer with the GERBER_RS274X device you should
import them (as Doug said) as a "physical layer". The .drd file should
be imported as a "hole /rout layer". When 'autoguessing' the settings in
the drill file GC Prevue often get's it wrong. If hat happens, you'll
see the drills plotted in (totally) wrong places. Just delete the
hole/rout layer and the associated aperture file and start the import
again. This time, in the "Import - Verify File Information" window,
right click on the NC drill file and choose "Modify format
parameters..." . look for the right settings, especially "whole digits"
(2), "precision" (4) and the right format for the "embedded drill table
units" (inches or mm).
remember that the way gerber files are made are a bit 'loose', meaning
things like file extensions are not defined (every program uses
different ones) and PCB manufacturers sometimes have different idea's of
what should be included in what layer and in what format. So it is
always wise to see if your intended PCB manufacturer has an explanation
of how he expects things and if not, give 'm a call.
That said, I've made hundred's of PCB's with different manufacturers and
never really had a problem. I've used GC Prevue for more than 10 years
and it always worked fine. As said, it sometimes only needs a little
attention when importing the drill file.
Good luck,
Richard
Richard, thanks a lot. I spend a lot of time trying to display a single
layer in GC Prevue (an application from hell if you are new to this),
but did not succeed. However I found a great viewer on the web,
GerberLogix (free for non commercial use) which is a breeze to use.
I see that layer 3 (in Eagle), which became .L15 in the Gerber files,
was completely wrong, no wiring. This is probably because the quad layer
board was defined in Eagle as (123*16). Have to read more about that.
Anyway, thanks for the advice.
Regards, Robert