Eurocircuits and V6 .brd files

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

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

http://www.eurocircuits.com/index.php/technology-guidelines/pcb-layout-data/117-cadsoft-eagle-brd-to-gerber-conversion-guidelines

All the best

Warren

--

Viewed / responded via the newsgroup at

news.cadsoft.de

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

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