Eurocircuits and V6 .brd files

On 15.01.2012 16:48, Richard Herman wrote:

 

BTW: I got a free license for GerberLogix, which you suggested a few

posts back, to see how it works/looks/feels. It is indeed a lot easier

than GC Prevue, but I don't know how accepted it's output is with

boardhouses (if that's important to you). My current PCB manufacturer

accepts GC Prevue .GWK files for manufacturing and/or checking boards

(they also accept Eagle .BRD files, but I've never used that).

 

>

Richard

Hello Richard, maybe because I am new to this, I find the whole process

very 'unautomated'.

Assuming that individual Gerber files are the standard, I am looking to

create an ULP that counts all used layers and generates a board specific

CAM file (board_name.cam). Which will put all Gerber files in a

subdirectory and generates another subdirectory with all layer images.

I did not find anything existing of this nature.

Robert

On 15.01.2012 16:48, Richard Herman wrote:

 

BTW: I got a free license for GerberLogix, which you suggested a few

posts back, to see how it works/looks/feels. It is indeed a lot easier

than GC Prevue, but I don't know how accepted it's output is with

boardhouses (if that's important to you). My current PCB manufacturer

accepts GC Prevue .GWK files for manufacturing and/or checking boards

(they also accept Eagle .BRD files, but I've never used that).

 

 

Richard

Hello Richard, maybe because I am new to this, I find the whole process

very 'unautomated'.

Assuming that individual Gerber files are the standard, I am looking to

create an ULP that counts all used layers and generates a board specific

CAM file (board_name.cam). Which will put all Gerber files in a

subdirectory and generates another subdirectory with all layer images.

I did not find anything existing of this nature.

Robert

Op Sun, 15 Jan 2012 16:17:18 +0100 schreef Robert Boers <robert@nospam.ch>:

Thank you Richard. But I don't think it is obvious, as my question was 

concerning supply layers. In Eagle V6 supply layers are converted to 

signal layers, unlike in Eagle V5. So in V6 there is no special 

treatment needed and it becomes a .Lox layer. In Eagle V5 a supply layer 

is represented inverted and requires inversion. Correct?

Robert

Hello Robert,

Correct. in V6 supply layers do not exist anymore. If your design started 

as a V5 design which was converted to V6, the supply layer is now a normal 

inner layer with a signal polygon on it.

A snippet from the V6 changelog:

• Supply layers:

   - Supply layers (i.e. layers with names that start with a '$') are no 

longer

     treated special. Layers for supply signals now need to be realized 

using

     signal polygons.

Since they are not treated special (not inverted), it still looks obvious 

to me: Use the settings for an inner layer. Am I missing something?

If the design was converted from V5 to V6, make sure to check the layer 

for correct connection.

BTW: I got a free license for GerberLogix, which you suggested a few posts 

back, to see how it works/looks/feels. It is indeed a lot easier than GC 

Prevue, but I don't know how accepted it's output is with boardhouses (if 

that's important to you). My current PCB manufacturer accepts GC Prevue 

.GWK files for manufacturing and/or checking boards (they also accept 

Eagle .BRD files, but I've never used that).

Richard

On 15.01.2012 14:46, Richard Herman wrote:

Op Sun, 15 Jan 2012 10:41:45 +0100 schreef Robert <Robert@nospam.ch>:

 

>> To answer part of my own questions, I found that I can setup a cam job

>> for each layer that I need.

>> The only question left is for generating a Gerber of an internal power

>> plane. Do I include there also the pads (17), via(18) and

>> dimension(20) layer?

>>

>> Robert

>>

>>

>>>

>>> Morton, after some testing I found where the problem is. The

>>> gerb274x-4layer.cam only looks at top, bottom, layer 2 and 15. I have

>>> not found out how I can get it to look at my layer 3.

>>>

>>> Furthermore, it will only deal with layer 2 and 15 as signal layers, and

>>> I have my layer 2 defined as ground plane. Since I got my design error

>>> free after some manual work, I'd like to keep it. Is there a way in

>>> Eagle to move the layers to match gerb274x-4layer.cam or another way to

>>> create Gerber files from my current design?

>>>

>>> Regards, Robert

>>>

>>

>

 

Hello Robert,

 

>

Because there isn't an always correct answer for this, visiting the

Eurocircuits link Warren mentioned a few post earlier, gives me this:

 

Layer conversion rules - syntax:

 

Layer function (.file extension) consists of Eagle layer(s) : Eagle

layer number & function + …

 

Solder stop Component side (.STC) = 20 Dimension layer + 29 tStop laye

Silkscreen Component side (.PLC) = 20 Dimension layer + 21 tPlace layer

+ 25 tNames layer

Componentside (.CMP) = 1 Top layer + 17 Pads layer + 18 Vias layer + 20

Dimension layer

Inner layers (.Lox) = x Inner layer + 17 Pads layer + 18 Vias layer + 20

Dimension layer

Solderside (.SOL) = 16 Bot layer + 17 Pads layer + 18 Vias layer + 20

Dimension layer

Solder stop Solder side (.STS) = 30 bStop layer + 20 Dimension layer

Silkscreen Solder side (.PLS) = 22 bPlace layer + 26 bNames layer + 20

Dimension layer

Milling (.MILING) = 46 Milling layer + 47 Measures layer + 20 Dimension

Layer

Excellon drill (.DRD) = 44 Drills layer + 45 Holes laye

Cream frame Componentside(.PMC) = 31 tCream layer + 20 Dimension layer

Cream frame Solderside (.PMS) = 32 bCream layer + 20 Dimension layer

 

>

So the answer seems pretty obvious....

 

>

Richard

Thank you Richard. But I don't think it is obvious, as my question was

concerning supply layers. In Eagle V6 supply layers are converted to

signal layers, unlike in Eagle V5. So in V6 there is no special

treatment needed and it becomes a .Lox layer. In Eagle V5 a supply layer

is represented inverted and requires inversion. Correct?

Robert

Op Sun, 15 Jan 2012 10:41:45 +0100 schreef Robert <Robert@nospam.ch>:

To answer part of my own questions, I found that I can setup a cam job 

for each layer that I need.

The only question left is for generating a Gerber of an internal power 

plane. Do I include there also the pads (17), via(18) and dimension(20) 

layer?

 

Robert

 

>>

>> Morton, after some testing I found where the problem is. The

>> gerb274x-4layer.cam only looks at top, bottom, layer 2 and 15. I have

>> not found out how I can get it to look at my layer 3.

>>

>> Furthermore, it will only deal with layer 2 and 15 as signal layers, and

>> I have my layer 2 defined as ground plane. Since I got my design error

>> free after some manual work, I'd like to keep it. Is there a way in

>> Eagle to move the layers to match gerb274x-4layer.cam or another way to

>> create Gerber files from my current design?

>>

>> Regards, Robert

>>

>

Hello Robert,

Because there isn't an always correct answer for this, visiting the 

Eurocircuits link Warren mentioned a few post earlier, gives me this:

Layer conversion rules - syntax:

Layer function (.file extension)     consists of Eagle layer(s) : Eagle layer 

number & function + …

Solder stop Component side (.STC)     = 20 Dimension layer + 29 tStop laye

Silkscreen Component side (.PLC)      = 20 Dimension layer + 21 tPlace layer + 

25 tNames layer

Componentside (.CMP)                    = 1 Top layer + 17 Pads layer + 18 Vias layer 

+ 20 Dimension layer

Inner layers (.Lox)                    = x Inner layer + 17 Pads layer + 18 Vias layer + 

20 Dimension layer

Solderside (.SOL)                         = 16 Bot layer + 17 Pads layer + 18 Vias layer + 20 

Dimension layer

Solder stop Solder side (.STS)        = 30 bStop layer + 20 Dimension layer

Silkscreen Solder side (.PLS)         = 22 bPlace layer + 26 bNames layer + 20 

Dimension layer

Milling (.MILING)                  = 46 Milling layer + 47 Measures layer + 20 

Dimension Layer

Excellon drill (.DRD)                   = 44 Drills layer + 45 Holes laye

Cream frame Componentside(.PMC)       = 31 tCream layer + 20 Dimension layer

Cream frame Solderside (.PMS)      = 32 bCream layer + 20 Dimension layer

So the answer seems pretty obvious....

Richard

To answer part of my own questions, I found that I can setup a cam job

for each layer that I need.

The only question left is for generating a Gerber of an internal power

plane. Do I include there also the pads (17), via(18) and dimension(20)

layer?

Robert

 

Morton, after some testing I found where the problem is. The

gerb274x-4layer.cam only looks at top, bottom, layer 2 and 15. I have

not found out how I can get it to look at my layer 3.

 

Furthermore, it will only deal with layer 2 and 15 as signal layers, and

I have my layer 2 defined as ground plane. Since I got my design error

free after some manual work, I'd like to keep it. Is there a way in

Eagle to move the layers to match gerb274x-4layer.cam or another way to

create Gerber files from my current design?

 

Regards, Robert

 

On 14/01/2012 22:24, Morten Leikvoll wrote:

Robert<Robert@nospam.ch>  wrote:

>> On 14/01/2012 17:44, Olin Lathrop wrote:

>>> Robert wrote on Sat, 14 January 2012 11:33

>>>> 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).

>>>

>>> That sounds like you used layers 1, 2, 3 and 16, but wrote out layers 1, 2,

>>> 15, and 16.  I always use consecutive layers from one except that the

>>> bottom layer is 16 to avoid any confusion.  Still, that should have been

>>> easily spotted when previewing the gerber files, so I still don't see how

>>> that could have happened.

>>

>> Well, I simply ran the gerb274x-4layer.cam job. It generates tabs for the

>> internal layers .ly2 and .l15 with above Eagle layer definition. No idea

>> that that was wrong. Will investigate.

>>

>> Robert

 

I suspected that. Maybe a future cam proc could warn about data in copper

layers that isnt associated with a job?

Morton, after some testing I found where the problem is. The

gerb274x-4layer.cam only looks at top, bottom, layer 2 and 15. I have

not found out how I can get it to look at my layer 3.

Furthermore, it will only deal with layer 2 and 15 as signal layers, and

I have my layer 2 defined as ground plane. Since I got my design error

free after some manual work, I'd like to keep it. Is there a way in

Eagle to move the layers to match gerb274x-4layer.cam or another way to

create Gerber files from my current design?

Regards, Robert

Robert <Robert@nospam.ch> wrote:

On 14/01/2012 17:44, Olin Lathrop wrote:

>> Robert wrote on Sat, 14 January 2012 11:33

>>> 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).

>>

>> That sounds like you used layers 1, 2, 3 and 16, but wrote out layers 1, 2,

>> 15, and 16.  I always use consecutive layers from one except that the

>> bottom layer is 16 to avoid any confusion.  Still, that should have been

>> easily spotted when previewing the gerber files, so I still don't see how

>> that could have happened.

 

Well, I simply ran the gerb274x-4layer.cam job. It generates tabs for the

internal layers .ly2 and .l15 with above Eagle layer definition. No idea

that that was wrong. Will investigate.

 

Robert

I suspected that. Maybe a future cam proc could warn about data in copper

layers that isnt associated with a job?

On 14/01/2012 17:44, Olin Lathrop wrote:

Robert wrote on Sat, 14 January 2012 11:33

>> 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).

 

That sounds like you used layers 1, 2, 3 and 16, but wrote out layers 1, 2,

15, and 16.  I always use consecutive layers from one except that the

bottom layer is 16 to avoid any confusion.  Still, that should have been

easily spotted when previewing the gerber files, so I still don't see how

that could have happened.

Well, I simply ran the gerb274x-4layer.cam job. It generates tabs for

the internal layers .ly2 and .l15 with above Eagle layer definition. No

idea that that was wrong. Will investigate.

Robert

Robert wrote on Sat, 14 January 2012 11:33

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).

That sounds like you used layers 1, 2, 3 and 16, but wrote out layers 1, 2,

15, and 16.  I always use consecutive layers from one except that the

bottom layer is 16 to avoid any confusion.  Still, that should have been

easily spotted when previewing the gerber files, so I still don't see how

that could have happened.

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.