New to Eagle- "No Device Specified"

On 11/29/2012 04:44 PM, japper wrote:

Hi,

I am new to Eagle 6.3 and have board layed out and all errors have been fixed.

 

I am trying to make some Gerber files but need a little help....

 

With the board layout open, I click on the CAM icon and I enter a name and path for my file in the file box and then click process Job

but I must be missing something because I get an error rmessage that tells me "No Device Specified"

It's asking for the output format - essentially the device on which the

gerber files will be used.  Look at each section of your CAM job in the

"Output" pane - it's right below the "Job" pane.  For most board houses,

you'll want to set the Device pull-down menu to"GERBER_RS274X".  For the

drill file, you'll want to set it to "EXCELLON".

However, the Drill file section will want to know file that specifies

the rack of drill bits to be used.  To generate this file, use the ULP

"drillcfg" and save the file to your project directory.  Then in the

"Drill file" section of your CAM job, set the "Rack" text field to this

file name.

Now try clicking on "Process Job".

"Process Job" processes each section in sequence.  So it's the same as

selecting each Section tab and clicking on "Process Section".  You can

use the latter technique to determine exactly which section is problematic.

One other item that will make it easier for your board house is the

"pos. Coord" check box in the "Style" pane of each section.  With this

turned on, the CAM processor will shift the section up and to the right

to the extent necessary to make sure all features are contained entirely

in Quadrant I (that is, x and y coordinates are positive).  But the CAM

processor does this on a section-by-section basis which can result in

different layers being shifted different distances.  I have found it

best to leave this box unchecked.  It makes it easier for the board

house to align the layers, and when viewing the gerber output with a

viewer (gerbv for instance) the layers will be aligned properly.

HTH,

    - Chuck

In article <k98rsq$aqs$1@cheetah.cadsoft.de>, chuck.huber@dukepro.com

says...

 

On 11/29/2012 04:44 PM, japper wrote:

Hi,

I am new to Eagle 6.3 and have board layed out and all errors have been fixed.

 

The instructions for this suggest a serious amount of software

development should be done on this part of the process ?

Thanks Chuck-

I am working through this but not sure if  I am doing this correctly or not… Here is what I have done so far:

I used the drillcfg.ulp that created snowflake.dri which I then saved to my project directory (C:\My Documents\Eagle\Snowflake) but was not able to find the Rack" text field or the "Drill file" section of my CAM job. The help says that this is in the CAM main menu but doesn’t really say how to get to this menu…

On the Eagle Cam processor window there are thumb tabs for each section marked with an “*”

I have two of these…

The first section

Output device is set to GERBER_RS274X, File is set to C:\Program Files\Eagle-6.3.0/cam/Snowflake and contains the following layers: 

1 Top, 16 Bottom, 17 Pads, 18 Vias, 19 Unrouted, 20 Dimension, 21 tPlace, 22 bPlace, 23 tOrigins, 24 bOrigins, 25 tNames, 26 bNames, 27 tValues, 28 bValues, 29 tStop, 30 bStop, 31 tCream, 32 bCream, 33 tFinish, 34 bFinish, 35 tGlue, 36 bGlue, 37, tTest, 38 bTest, 39 tKeepout, 40 bKeepout, 41 tRestrict, 42 bRestrict, 43 vRestrict, 44 Drills, 45 Holes, 46 Milling, 47 Measures, 48 Document, 49 Reference, 51 tDocu, 52 bDocu,  101 Patch_Top, 102 Vscore, 103 tMap, 104 Name, 105 tPlate, 106 bPlate, 107 Crop, 116 Patch_BOT

The second section

Output device is set to EXCELLON, File is set to C:\Program Files\Eagle-6.3.0/cam/Snowflake and contains the following layers: 

44 Drills, 45 Holes, 46 milling, 47 Measures

I get a warning that states “More than 1 signal layer active and when I OK this window,

it creates the following files:

C:\Program Files\Eagle-6.3.0/cam/Snowflake.gpi,

C:\Program Files\Eagle-6.3.0/cam/Snowflake.dri,

C:\Program Files\Eagle-6.3.0/cam/Snowflake

Am I doing this correct?

I thought that I might try to view these with GC-Viewer but it didn’t like any of these files…

Also, what actually makes a complete set of Gerber files that a PCB manufacturer would need?

Is this the gpi, dri and any other files?

Please advise and thanks again!

On 11/30/2012 08:56 AM, japper wrote:

Thanks Chuck-

 

I am working through this but not sure if  I am doing this correctly

or not… Here is what I have done so far:

 

I used the drillcfg.ulp that created snowflake.dri which I then saved

to my project directory (C:\My Documents\Eagle\Snowflake) but was not

able to find the Rack" text field or the "Drill file" section of my

CAM job. The help says that this is in the CAM main menu but doesn’t

really say how to get to this menu…

 

On the Eagle Cam processor window there are thumb tabs for each

section marked with an “*” I have two of these…

I see.  It appears that you have not loaded a cam job.  Try saving the

attached file in your project directory, then in the cam processor click

File->Open->Job and select this file.

It's an ascii text file so you can edit it with notepad, vim, emacs, or

any plain text editor of your choice.  It contains sections for a

4-layer board, but I have commented out the two sections for the inner

copper layer.

Once you load this CAM job, click on the section titled "Drill".  In it,

you will see the "Rack" field.  I have pre-populated it with

Snowflake-RevA.drl.  Either change this value to the .drl file you saved

from drillcfg, or save your drillcfg output to this file name.

 

The first section Output device is set to GERBER_RS274X, File is

set to C:\Program Files\Eagle-6.3.0/cam/Snowflake and contains the

following layers: 1 Top, 16 Bottom, 17 Pads, 18 Vias, 19 Unrouted, 20

Dimension, 21 tPlace, 22 bPlace, 23 tOrigins, 24 bOrigins, 25 tNames,

26 bNames, 27 tValues, 28 bValues, 29 tStop, 30 bStop, 31 tCream, 32

bCream, 33 tFinish, 34 bFinish, 35 tGlue, 36 bGlue, 37, tTest, 38

bTest, 39 tKeepout, 40 bKeepout, 41 tRestrict, 42 bRestrict, 43

vRestrict, 44 Drills, 45 Holes, 46 Milling, 47 Measures, 48 Document,

49 Reference, 51 tDocu, 52 bDocu,  101 Patch_Top, 102 Vscore, 103

tMap, 104 Name, 105 tPlate, 106 bPlate, 107 Crop, 116 Patch_BOT

Yeah... This is way too much.  What you're looking for is one section

per layer.  So you'll wind up with one for the top silkscreen, one for

the top solder mask, one for the top copper, etc.

I get a warning that states “More than 1 signal layer active and when

I OK this window, it creates the following files:

That's a reasonable warning.  It's trying to put all the signal layers

in a single gerber file.

This is where knowing a little bit of how the boards are fabricated will

help.  Each gerber file (one per section) is used in different places in

the fabrication process.  The first thing the board house will do is to

drill holes in the copper-covered fiberglass core.  Then they'll plate

these holes through to provide a connection from the top to the bottom

layer through each hole.  This is where the Excellon drill file is used

(.exc, I think).

The third step is to etch away the unwanted copper on the top and bottom

layers (two separate patterns requiring two separate gerber files.

Then they'll apply a solder mask and remove areas that should not be

covered with mask.  Again, since the top and bottom mask layers are

different, two different gerber files are required.

The last step is to apply a silkscreen to the top and optionally the

bottom of the board.  Got it yet? Two different patterns require two

different gerber files.

All in all, you'll wind up with 6 or 7 different gerber files - one for

each step in the fabrication process.

Am I doing this correct?

You're on the right track, but you need to break the layers up into

different sections.

If you examine the attached snowflake.cam with a text editor, you'll

find that it appears very much like a .ini file.  The first section

describes the job and what sections comprise the job.  Then each

following section, delineated with the section name in square brackets,

is section-specific information.

A note of caution: I have commented out two of the sections in the job

section.  Thus if you save this as-is from within the CAM processor, the

sections commented out will not be included in the saved file.  It'd be

a good idea to save the attached file for future reference.

I thought that I might try to view these with GC-Viewer but it didn’t

like any of these files…

I believe gerbv has a Windows version.  Wouldn't swear to it, though.

Also, what actually makes a complete set of Gerber files that a PCB

manufacturer would need? Is this the gpi, dri and any other files?

The board house does not need the .gpi or the .dri files.  I usually

toss these.

HTH,

    - Chuck

Thanks Chuck. I will look over this ini file and learn from it.

Almost there... I did point update the Cam file to point to the .drl file I saved

from the drillcfg but when processin the job I get the  the following message:

DRILLS MISSING - NO DRILL FILE HAS BEEN PRODUCED!

Is this OK?

Also, what sections did you comment out of the cam file?

I appreciate your expert help!

On 11/30/2012 03:52 PM, japper wrote:

Thanks Chuck. I will look over this ini file and learn from it.

 

Almost there... I did point update the Cam file to point to  the .drl file I saved

from the drillcfg but when processin the job I get the  the following message:

 

DRILLS MISSING - NO DRILL FILE HAS BEEN PRODUCED!

 

Is this OK?

From your board editor, click Options->Set->Drill->Set.  This sets the

list of drills to use in your design to the sizes that are actually

present in the board.  Then run the CAM processor again.

Be advised that some of your vias may be in metric.  If you get any

drill sizes that are fractions of a mil, these need to be changed to an

even mil size.

The attached ULP, fixdrills.ulp, will round every via to the nearest

mil.  After running it, set your drill list again (see above), and run

the CAM processor.

Also, what sections did you comment out of the cam file?

It was for the two inner layers.  The file I provided earlier was for a

4-layer board.  To avoid confusion, I just commented out the two inner

layers, but left their respective sections in tact further on down the

file.  Look in the top of the file in the "[CAM Processor Job]" section.

You'll see two sections that are commented out with a leading hash mark.

    Description="

Your Job Description Here

\nThis CAM job
consists of twelve sections that generate data for a four layer board.

\n"

    Section=NonPTHoles

    Section=Drill

    Section=TopScreen

    Section=TopPaste

    Section=TopCu

    Section=TopMask

    Section=BotScreen

    Section=BotPaste

    Section=BotCu

    Section=BotMask

    #Section=Inner2

    #Section=Inner15

I also left the NonPTHoles in place as an example.  On some boards, we

have to have certain holes non-plated.  This adds to the cost of the

board since an extra drilling process may be required after the

plate-through process, but in some cases it is necessary.  This section

tells the board house which holes should NOT be plated.  Depending on

the size of the hole, this may be combined with the milling step where

each board is being cut out of a much larger panel.  Because I am not

intimetly familiar with the criteria, I leave that decision to them,

just as long as I get the desired results.

For a garden-variety 2-layer board, you can most likely comment out or

delete the NonPTHoles section.

You should probably also change the job description to something more

suitable to your project.

 

I appreciate your expert help!

 

Glad to be of assistance.

Best regards,

    - Chuck

Chuck-

I spoke too soon...

I ran the fixdrills.ulp, set my drill list again, and run the CAM processor,

pointed it to the latest drill file, and I sget the following message when

I try to process the job: 

DRILLS MISSING - NO DRILL FILE HAS BEEN PRODUCED!

.

I would attach the cam file but I am not sure how to attach files to this post...

thanks

Chuck-

Here is what the drill file has:

Generated by EAGLE CAM Processor 6.3.0

Drill Station Info File: C:/eagle/SnowFlake/Snowflake-ExcellonDrill.dri

Date              : 12/1/2012 2:29:19 AM
Drills            : C:/eagle/SnowFlake/snoflake.drl
Device            : Excellon drill station

Parameter settings:

Tolerance Drill + :  0.00 %
Tolerance Drill - :  0.00 %
Rotate            : no
Mirror            : no
Optimize          : yes
Auto fit          : no
OffsetX           : 0inch
OffsetY           : 0inch
Layers            : Drills Holes

Drill File Info:

Data Mode         : Absolute
Units             : 1/10000 Inch

Missing Drills:

-- Requested --

Size       used

0.1400inch     5
0.0320inch    84
0.0400inch    29
0.1300inch     1
0.0360inch     8

Drills used:

Code  Size       used

T01   0.0276inch     3
T04   0.0394inch     6

Total number of drills: 9

!!!!!!!!! DRILLS MISSING - NO DRILL FILE HAS BEEN PRODUCED!

hi,

you must specify a tolerance, eg +/- 2.5%

r

thanks!

That fixed it!