Procedure for Transferring PCB layout from HPADS over to LPKF Router

Updated by Khoman Phang on July 22/1999.
Updated by Denis Daly on July 1/2002.

Part 1: Generating Gerber and Excellon data from HPADS
======================================================

A. Create a mask from which Gerber files representing each layer are created:

  1. Bring up the MTOOLS dialog by executing FILE/EXPORT from the layout.

    2. Enter a name with a .gbr extension and set the File Type to Gerber.
    Click OK.
  2. From the resulting window, select Mask to Gerber.

    3. Click OK.
B. Generate Gerber files for each layer EXCLUDING the hole layer:
  1. Dismiss Mtools log window.
  2. In the GERBER window, click on "Gerber File Options"

    3. The defaults should be:

    Gerber unit: mm
    Format: 3.3
    Zero Suppress: Leading
    Data Mode: Absolute
    Circular: 360
    EOB Character: -
    EOJ String: M02
    CR/LF: Suppress
     

  3. In the GERBER window, select "Translate".
  4. Select all required layers (Do not select the "Hole" layer), click OK.

    5. Mtools generates separate Gerber files for each layer
    (e.g. cond.gbr, cond2.gbr)
  5. Once done, the MTools log window comes up. Review it and dismiss it.


    6. NOTE: Check to see whether any flash objects were created. CircuitCAM seems to have difficulty importing flash objects and prefers filled objects. How HP ADS's Gerber translator decides what objects to flash or fill is a mystery. One time, the translator created many flash objects for a particular design. I solved the problem by copying the design (i.e., the .dsn file) over to a new name. This time when it did the Gerber translation, it created only fill objects -- despite the fact that the two designs were identical!
     

  6. From the GERBER window, click "View Gerber".
  7. Verify Gerber layout, then copy over the resulting Gerber into a separate subdirectory.
C. Create the drill file from the hole layer in Excellon format:
  1. From the GERBER window, select "Edit Apertures".
  2. In the Edit Apertures dialog, select "Flash Circles".
  3. In the Map Circles/Holes dialog, verify the circle count and diameters, and that the Update Aperture box is checked. Note the Block Names of the circles.

    4. Click OK.

    NOTE: circle count does NOT simply represent the number of holes! ALL circles appearing on ANY layer are counted.
     

  4. Back in the Edit Aperture dialog, note which D-codes have the block names that were mapped to circles.

    5. Click SAVE.
  5. From the GERBER window, click Translate. Select the hole layer, then click OK. When the MTOOLS log is displayed, look for errors or warnings. If desired, save the log before closing it.
  6. From the GERBER window, click "View Gerber".
  7. From GBRVU, click Aperture. The Aperture dialog appears.
  8. From the Aperture dialog, enter tool numbers (arbitrary assignment beginning with 1) and drill diameters for the D-codes that were noted in step 5. Click OK and save changes.
  9. From GBRVU, execute Tools>Drill>Excellon. Set to NO suppress leading zeroes. Select the hole layer and click OK.


    10. Two files will be created in the project directory with the layer name as a prefix and .drl and .rpt as suffixes (i.e. hole.drl and hole.rpt). hole.drl is the drill file. hole.rpt has the drill tools table.
     

  10. Copy hole.drl and hole.rpt to subdirectory containing the Gerber files. You now have a complete set of files describing the board.


Part 2: Importing Gerber/Excellon Files into CircuitCAM
=======================================================

  1. Transfer Gerber and Excellon files over to the PC controlling the LPKF router.
  2. Start up circuitCAM software.
  3. Load up template for HP ADS files by selecting

    4. File/New/HPADS.cat
    This template sets up the proper scaling and the default aperture and tool lists for you.
     
  4. Import all Gerber files except for the board outline by selecting File/Import.

    5. You can highlight multiple files. For each file, select the appropriate layer on the PCB. Use default aperature and tool lists.
     
  5. Once the layers are displayed, highlight everything on the layout and execute Edit/Path to Polygon (shift-P).
  6. Import board outline Gerber file(e.g. case_dimensions.gbr). With this layer you don't want to convert path to Polygon.
  7. Import Excellon drill file (e.g. hole.drl)
  8. Edit the tool list (Config/FormatConfig/Excellon_Tool List/Tool HP ads).

    9. The settings for the tools that we have can be found in
    Config/FormatConfig/configsLpkfMillDrill/LpkfDrillingTool
    Copy these parameters over to the associated tools in the tool list.

    Example:
    To set up tool T1 to be the same as the 0.8mm spiral drill in LpkfDrillingTools, highlight the tool, then right click to bring up the settings. Its settings are:
    - Circle a:0.8mm
    - Nothing selected in Transform or Draw
    - In Diverge select "User Defined" and enter 0.71mm min and 0.81mm current dimension
     

  9. Insulate top and bottom layers by selecting Edit/insulate
  10. Create board boundary by clicking on board outline and select Edit/Contour Routing. Use default 2mm contour router.
  11. Insert gaps in routed path through icon on lefthand side.
  12. Select and delete original board outline.
  13. At this point you can also remove particular isolation traces if, for example, you wish to merge a pad to a ground plane.
  14. To export the layout in LMD format, display all layers then select File/Export/LPKF CircuitBoardPlotter


Part 3: Importing a LMD design into BoardMaster
===============================================

  1. Select File/Import/(LMD/LPR)
  2. Position design onto unused area
  3. Calibrate universal cutter by routing test traces
  4. Step through each production phase by selecting a phase, highlighting all traces by clicking All+, and clicking Start button.

    To minimize the number of tool changes, build the board in the following order:

    Layer
    -----
    top - MillingTop \
    bot - MillingBottom > 0.2mm universal cutter
    bot - Markingholes /
    bot - Drill (un)plated -- use defined tool set
    bot - cutting outside border

  5. When you click Start, Boardmaster will prompt you to change tools but only when necessary.