New to Eagle- "No Device Specified"

Question

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"

What am I missing or doing wrong?

thanks

dukepro · Accepted Answer

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 
This CAM job consists of twelve sections that generate data for a four layer board. 
" 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 
 Attachments: fixdrills.ulp.zip

dukepro · Answer

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

Former Member · Answer

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