Ivex User Reference

To produce a drill file, "CAM | NC Drill..." is selected from the main menu. The dialog box that appears is included as an attachment.  Two files are produced, *.drl (which is a report file that gives you the number of holes produced by each tool) and *.th which is the file that I described to you earlier.  There seems to be no provision for changing the precision (2.4).

AP Circuits does not require the data to arrive in the GCPrevue work file. We require NC data and Gerber data to produce your boards. The following section provided by Paul outlines the necessary procedures that he has taken to get data into GCPrevue.

Should you wish to use the GCPrevue work file in place of the NC and Gerber data outputs for our services keep in mind that we DO NOT support any of the newer GraphiCode versions. GraphiCode product versions that can produce CWK, PWK or WRK are supported.

We do recommend that you examine your data with a 3rd party viewing utility to prevent any anomalies between what you have drafted vrs the manufactured product.  In many instances your cad software’s built-in viewing routine will not show anomalies in your outputs due your cad systems Gerber interpreter.  Using a 3rd party product will ensure that there are no format translation problems. 

The following document explains the steps taken by Paul to create files using IVEX WinBoard version 2.21 and the procedures he used to produce the data sets imported into GCPrevue. There is also a GCPrevue cookbook on our web site that covers basic operation of GCPrevue and the process of importing data, There is also a page containing a few screen shots and loading proceedures.  Paul’s notes are very specific and my prove more valuable to the Ivex operations than these generic models.

WinBoard is a popular product as it is distributed by NTE replacement semiconductors at a price of $75 Canadian. Also available at the same price is a Schematic capture/drafting tool WinDraft.  Both of these products have a 200 pin limit, but these limit can be raised at a reasonable cost. Also available from the IVEX web site is DEMO versions with a 100 pin limit.   As stated in the AP circuits documentation you should view the output from your CAD program using a GERBER plotter file viewing program. The AP Circuits site has available for download a DOS version of GCPrevue

The remainder of the document explains how to get the required information from WinBoard into this Work File. Once you have the PCB layout complete, it looks OK when printed and it passes the Dynamic Rules Checks (DRC), you are ready to produce the 4 files required from WinBoard.  These files are the Plotter output for the TOP layer, the Plotter output for the Bottom layer, the Gerber drill files which determine where to drill the holes, and the drill list which determines what size drill bits to use.

To help differentiate the layers and insure they are not mirrored or reversed AP Circuits recommends placing some TEXT on the TOP (component) layer. This must be text that is actually written in copper, not on a silk screen, so make sure you don't create any shorts with this text.

To produce the required files from WinBoard follow the steps outlined below.

1. From the Menu Bar select CAM then Photo Plot
2. In the Plot dialog that appears press the 'Object Selection' button.
3. Press the 'Copper' button to output only the copper traces, then OK.
4. Next press the 'Layer Selection' button.
5. In the 'Print/Plot Layer Selection' dialog deselect the Solder Entry and ensure the component entry is selected then Press OK. You may wish to select the Preview option to make sure everything is OK.
6. Press the Plot button.

The default settings in the Gerber Setup screen should be OK for the GCPrevue program. Note these are not in the format the AP Circuits prefers, this is why the final file sent to AP Circuits is generated by GCPrevue. The settings should be as follows.

• Format: RS274-X
• Units: Inch
• Coordinates: Absolute Zeros Suppression: None
• Nb Digits m: 2
• Nb Decimals n: 4
• End Of Block: (empty)
• Add CR/LF: (empty)
• Press the Plot button.

Give the resulting file a name that reflects that it is the TOP layer. It is best to use the GBR extension so GCPrevue will recognize the file type. Next print the bottom layer.

1. From the Plot Dialog press the 'Layer Selection' button and deselect the Component (Top) layer and select the Solder (Bottom) layer.
2. The Object selection should be retained from the (Top) layer plot.
3. Press OK.
4. Press the 'Plot button none of the settings in the 'Gerber Setup' dialog should need changing at this point, so
5. Just press the 'Plot' button again.
6. This time give the output file a name that reflects that this is the bottom layer. Once again retain the .GRB extension.

The only file required at this point is the drill file.

• Select 'Close' in the 'Plot' dialog
• from the menu Bar select CAM and NC Drill. The default values should work OK with GCPrevue. These values are listed below.
• Units: mil
• X Offset: 0
• Y Offset: 0
• Format: Decimal
• Hole Size Maximum: not enabled
• Press the 'OK ' button and select a file name that reflects the project while retaining the .DRL extension.

The NC Drill option creates several files the one loaded by GCPrevue has the same name as given in the step above but has the '.TH' extension. The Drill file with .DRL contains a listing of drill sizes that must be manually entered into GCPrevue. You now should have the 4 files required.  We now have to load them into GCPrevue, and correct their orientation.  By default WinBoard mirrors output in the X direction.  Although it is possible to compensate for when generating the Plotter output this is not possible when producing the drill file.  GCPrevue allows us to correct this mirrored condition.

Run GCPrevue. The default screen that comes up in GCPrevue shows the Layer List at the top, the aperture list in the bottom left and the drill rack in the bottom right.  The layer list window is where the plotter output files for the top and layer bottom are loaded.  Also loaded in this window is the NC-Drill file which determines where holes are drilled and what tool is used.  Note that the NC-Drill file only indicates what tool number to use for a hole.  It does not indicate what size each tool is. This information is defined in the drill rack window.  This window list in inches the size of each tool referenced by NC-Drill file.

The Aperture window in the lower left list defines patterns used to generate the plot. The Photo file is just a series of draw commands that say draw from here to her using this size pen. The Aperture list defines what size pens to use, so to speak.

GCPrevue will automatically extract the information for the Aperture window from the Plotter files. Although WinBoard defines the drill sizes in the NC-Drill, GCPrevue will not read the sizes from this file and instead will assign a default size to all tools defined in the NC-Drill file. For this reason the Drill Rack must be defined manually as follows:

1. Print the NC drill file that has the .DRL extension. It contains the tool list (drill sizes and reference number). This file can be opened and printed with Windows Notepad as it is in ASCII format.

By default GCPrevue starts in the layer list window edit mode, therefore press 'ESC' to access the Menu Bar and select the Drills option.

1. Press <CTRL><m> and select the Edit option. 
2. Refer to the page you printed (see above) to determine the number of Tools (drill sizes).
3. Next edit the drill rack using the sizes in the print out. Once all information is entered press <ENTER> on the last row to exit the edit mode.

We are now ready to load files for the different layers:

1. Press ESC to access the menu Bar and select the Layers option.
2. Type in the file names for each layer as indicated below, the F10 key can be used to get directory listings.  The number one layer shows on top of layer two and so on. Therefore the files created by WinBoard should be added in the order shown below. 
3. Because the drill holes are always made smaller then the pads they are in, they must be made the top layer or they will be hidden by the pads.

The 'Layer List' screen should now show the 3 files we have selected. All the required information has now been given to the program the next step is have GCPrevue progress it all. GCPrevue will not properly load the NC-Drill file in the auto mode, you will have to load it using the NCDrill.PDF. Do the following:

1. Highlight the NC-Drill file press <CTRL><m>
2. select load from the pop up menu.
3. Select 'Drill' from the POP-UP Data type menu.
4. In the next dialog move to the 'Format:' field and press F10
5. select NCDRILL.PDF from the input format files.
6. Move to the 'Zero Suppress:' field press F10 and select 'Decimal'.
7. Press enter to proceed. The Drill data should now load correctly.  Now the two plot layers can be loaded.  Follow the these steps to do this:
8. Press <CTRL><m> and select Load.
9. In the Data type Dialog select Auto.
10. In the 'Load Auto data ' dialog enter 2-3 at the 'Layers:' prompt. Press ENTER.
11. A 'File Load Error' dialog may appear stating skipping header info.  Click OK on this error message.
12. Press <CTRL><m> and select the View option.  At this point you should see the plot from WinBoard. It however it will upside down and Mirrored in the X direction. Do the following To correct this:
13. Press <ctrl><m> to access the menu bar.
14. Select 'Edit' from the menu bar and then 'Rotate'. Verify that 'All' is in the Layers prompt and set the Rotate amount to 180 degrees.
15. Select 'Edit' from the menu bar and then 'Mirror X'. Verify that 'All' is in the Layers prompt and press OK. The plot should now look correct.
16. The final step is to save a project file. 
17. Press <CTRL><M> from within the Layer edit window.
18. Select the Save All option specify a file name and use the .CWK extension. You may also wish exit and restart GCPrevue and attempt to reload the PCB from the project file just to make sure the file you send is correct.

The methods you can use to send this file are well documented elsewhere on this WEB Site so look them up there. You can also download a Windows 95 version of GCPrevue from the following WebSite. This Windows will allow you to generate color plots of your PCB using any color printer that supports Windows. The Windows version will load the Project file created by the DOS version of GCPrevue. It will however not save to the .CWK project file format.  The project file format it saves to IS NOT supported by AP Circuits. This means the project file you send to AP Circuits must be created using the DOS version of GCPrevue http://www.graphicode.com/