This is a multi-part message in MIME format. --------------407D21E04EE6 Content-Type: text/plain; charset=us-ascii Content-Transfer-Encoding: 7bit Greg Hartung wrote: > My question is how to get Eagle to create the fabrication and drill files. Greg, we have used Eagle twice now to send gerber compatible files to a production house. Eagle makes good files but uses non-standard file extensions. Boards came out exact and perfect each time. Cant ask for more then that! I downloaded the technical help file from a PCB manufacturer that explains more about the way they need the files prepped, try at; www.becman.com/engineer.htm (I will also attach this info for you) Find out from your board people which actual files they need. Try to talk to the tech guy, not the sales guy! :o) From my written notes (hope this is right) eagle makes files/extensions: WHL aperture wheel (??) PLC silksreen legend component side (GTO) CMP copper component side (GTL) STC solder stop mask comp side (GTS) SOL copper colder side (GBL) STS solder stop mask solder side (GBS) (and eagle makes these excellon drill files) DRL tool rack file (??) DRD excellon output (TXT)?? DRI drill information file (??) The (GTO) etc are the equivalent gerber extensions they will need. You will need to use the excellon job in eagle as well as the normal output, the tutorial tells exactly what to do (I will attach the tute sent to me by the eagle tech guy) Hope all of this makes sense. If you look at most of the above gerber files in a text editor, it seems they are simple text listings of CNC commands. Any board production house worth their salt should have a gerber viewer that can recognise and test your files and rename the extension if they really have to! I am fairly impressed with Eagle for small jobs, just wished they used proper Gerber file extensions but guess copyright etc prevents that?? What do you call 10,000 lawyers at the botton of the ocean? ;o) If you still cant get it happening, please email me off list and I will try to help. -Roman --------------407D21E04EE6 Content-Type: text/plain; charset=iso-8859-1; name="roman.txt" Content-Disposition: inline; filename="roman.txt" Content-Transfer-Encoding: quoted-printable X-MIME-Autoconverted: from 8bit to quoted-printable by centauri.ezy.net.au id PAA11289 I have completed the tutorial, and ran the CAM processor to generate Gerber file= s. According to the tutorial, there should be 6 files, one of which should b= e named "democmp.cmp". According to the tutorial, this file defines the component side of the board. This file is not being created by the CAM processor. Is this data actually saved with a different extension? Also, I tried to create the drilling data using the EXCELLON.CAM job. The program reported that it could not find the file "democmp.drl", and apparently did not create the drilling data. Am I doing something wrong here? Thanks, Ivan Johnston From:=20 Ed Robledo Newsgroups:=20 eagle.support.eng References:=20 1 Hi Sir, Please follow these steps: Creating Gerber Files and Excellon Files with EAGLE 3.55 EAGLE provides a CAM job file, which will create your GERBER files for a,= 2 layer board in an easy fashion. Please follow these steps: Gerber Files 1- Load your board on the screen. To do this from the EAGLE Control Pane= l, click on File/Open/Board and select the board you will use. 2- Click on the Icon on the top Tool bar that says ULP. When the dialog b= ox appears select the ULP file called DRILLCFG.ULP from the ULP directory. = In a matter of seconds the command line you will notice a message saying ULP h= as finished. 3- Now click on the Icon that stands for the CAM Processor. This will loa= d the CAM Processor Screen. From this screen click on File/Open/Job (when asked= to save =93Modified Job=94 reply NO) and select the CAM job called GERBER.CA= M from the CAM directory and click OK. Romans note!! Now is the time to click the boxes, ie names etc that you might not want included in the Gerber files. I turned names off as I didn't want them on the component screen. 4- Now click on the button that says Process Job. This will prompt you wi= th 2 messages. The first message will be =93Delete the $$$ file after process=94= this is a dummy file which EAGLE creates, click OK. The second message is =93More= than one signal layer Active=94, Click OK to this message as well. Depending of th= e size and complexity of the board, the entire process will take a few minutes o= r a few hours. 5- When the CAM Processor stops all process it means it has finished. Thi= s process created several files that will have the same name as your board = with different extensions: .WHL Aperture Wheel File .PLC Silk Screen Component side .CMP Copper Component side .STC Solder Stop mask Component side .SOL Copper Solder side .STS Solder Stop mask Solder side EXCELLON FILES (Make sure you have done step 1 and 2 before proceeding with Excellon fil= es) 6- Directly from the CAM processor click on File/Open/Job and select the = CAM Job called EXCELLON.CAM from the CAM directory, then click OK. 7- Now click on the small button that says Process. This will begin the E= XCELLON file generation. Normally this process only takes a few seconds. 8- The following files are created when the process ends. .DRL Tool Rack File .DRD Excellon Output .DRI Drill Information file Subject:=20 Re: CAM Processor - Gerber Files Date:=20 Thu, 15 Jul 1999 19:53:52 -0700 From:=20 "ilj" Newsgroups:=20 eagle.support.eng References:=20 1 , 2 Ed Robledo wrote in message <378BAB26.A8BAC415@cadsoftusa.com>... >Hi Sir, >Please follow these steps: > Thank You, Ed. I followed your instructions, and still could not find the .CMP file. Fortunately, I discovered that for some reason the Windows 98 Explorer removes the .CMP extension when it displays the files. The .CMP file is displayed with a telephone icon, so I think that Windows is mistaking it = for some sort of system file. Regards, Ivan Subject:=20 Re: Error in generating Gerber files Date:=20 Thu, 22 Jul 1999 15:24:22 -0400 From:=20 Ed Robledo Newsgroups:=20 eagle.support.eng References:=20 1 Hi Dave, Edit the file called EAGLE.DEF file located in your EAGLE root directory.= Look for the driver called [GERBERAUTO]. Bellow the statement that says Units=3D= inch leave a space and place the command Decimals=3D6. This should take care o= f the error. Hope this is it, Ed --------------------------------------------------- ROMAN - here is the text from the BEC home page File Types We accept data in the following formats: Protel for Windows (v2.8, v3.2 or older)=20 Autotrax=20 Gerber files with Drill and Route files=20 Transfer Methods We insist that files transferred to us, are compressed using either PKzip= or similar program. This helps to shorten transfer time, and reduces the possibility of file = and data corruption. Files can be sent to us by the following methods: Email Attachments to bec@ats.com.au=20 BBS (Dial-in +61 7 3889 6574)=20 Floppy Disk (Head Office - PO Box 5282, Brendale, Qld 4500, Australi= a)=20 Information about Protel and Autrotrax If you are using Protel for windows we can accept a Binary pcb file. The = pcb file should contain enough information for drilling and routing. Edge of board must b= e defined by either a KEEP OUT LAYER or MECHANICAL LAYER 1 (BOARD LAYER in Autotrax) track of b= etween 0.005" and 0.012". See notes ond defining the border. Boards will be made with the l= ayers as specified on the program. i.e. top layer on top, bottom layer on bottom. This means th= at a single sided board with tracks on the top will be made as such. When panelising files = tick DUPLICATE DESIGNATORS under the OPTIONS PREFERENCES. This will ensure that componen= ts are not re-numbered when copying files. Drilling information will be generated from the drill= ing information stored in the PCB. You should check that: There are no holes on SMD pads unless specifically required. (Some j= obs do need holes on single layer pads)=20 Hole sizes are correct. (We will automatically enlarge holes on PTH = boards to compensate for plating)=20 Useful hints for Autotrax users: Block reading pcbs will ensure that components are not re-numbered w= hen panelising.=20 TRAXSTD.LIB has most hole sizes wrong and some times puts holes on s= ingle layer pads.=20 Single layer pads some times show "HOLE SIZE NOT USED". This does no= t mean there is no hole. Set the pad layer to multi layer then set the hole size to the= required size (0 for no hole) and then set the pad layer back to the original layer.=20 Strings are only displayed and printed in multiples of 0.012" with a= minimum size of 0.036". Using sizes that are not multiples of 0.012" could result in= strings overwriting other parts of the pcb.=20 Currently under PROTEL software version d 2.8 or lower there is no suppor= t for unplated holes or plated slots. If any unplated holes or plated slots are required, a pa= per drawing clearly specifying which holes are unplated and/or where the plated slots are and= what size. Alternatively the mechanical layer 2 can be used to define the plated slo= ts by placing a track of the slot width starting from the beginning of the slot and ending at t= he end of the slot. No other markings or dimensions should appear on this layer.=20 Information about Gerber and Drill Files LAYER FILE EXTENSION EXAMPLE Top Layer GTL example.gtl Bottom Layer GBL example.gbl Top Overlay GTO example.gto Bottom Overlay GBO example.gbo Top Solder Mask GTS example.gts Bottom Solder Mask GBS example.gbs Border for Routing GKO or GM1 example.gko OR example= .gm1 Plated Holes Drill File TXT example.txt Unplated Holes Drill File NPT example.npt Plated Slots GDS example.gds Schematic Design Note Drill files should be Excellon format no. 2 with sizes are included = in the header.=20 The preferred format for drill and gerber files is Imperial, 2 integ= er digits, 3 decimal digits, absolute type with no zero suppression.=20 Gerber files should be RS274-X. If other formats are used the file f= ormat, integer and decimal digits, aperture table, absolute or relative, metric or impe= rial and zero suppression settings must be supplied.=20 Files should not be mirror imaged and should be plotterd as viewed f= rom the top layer.=20 Files should be generated in such a way that the are aligned with ea= ch other. ie do not use auto centre or similar features that place different offsets on = different layers.=20 Plated slots should be defined placing a track of the slot width sta= rting from the begining of the slot and ending at the end of the slot. No other mar= kings or dimensions should appear on the PLATED SLOTS plot.=20 Panelisation Guidelines We will automatically panelise your design to fit as many pcbs as possibl= e on the panel you specify. This means we will determine which orientation will fit best (ho= rizontal or vertical) and will repeat the design in the X and the Y directions to fill the pane= l. We will not place copies of the design with different rotations in order to fit more copies= . If you wish to put more than one design in the panel or panelise in a more efficient way, yo= u have to copy all different designs in to one single file. We will step and repeat this sin= gle file as many times as it will fit in the standard panel. ie. if you have 4 designs that occu= py an area of 4x4" we will fit 8 sets in a 10.6x16.6" panel.=20 Please note: For routing purposes we need 0.1"(2.5mm) or more separation between = the boards.=20 Boards smaller than 1"x1" will be left in the panel with break out t= abs.=20 Panelised job should be oriented such that the X size corresponds to= the 16.6" side of our panel.=20 Defining the Border The edge of the board will be on the centre of the line defining the edge= of the pcb. The line will not be plotted on the board.=20 Make sure that: The track defining the edge is one single closed track=20 The begining of a border track always coincides with the end of anot= her border track.=20 That at any point in the edge of the pcb there are always 2 tracks t= erminating or starting. Do not place any other markings on the border layer or plo= t.=20 --------------407D21E04EE6-- -- http://www.piclist.com hint: The PICList is archived three different ways. See http://www.piclist.com/#archives for details.