Make Board Paneling Tutorial

Make Board Paneling is a function to modify the data designed with a single sub board into an array type to use manufacturing related features such as Metal Mask Manager, Mounting Emulator, Block JIG Generator, Router-Machine JIG Generator, and so on.

Make Board Paneling using PDBB

  1. Launch PollEx PCB.
  2. From the menu bar, click File > Open and open the PollEx_PCB_Sample_r<revision number>.pdbb file from C:\ProgramData\altair\PollEx\<version>\Examples.
  3. From the menu bar, click Manufacture > Make Board Paneling.
    The design file is saved as a *.pdbb file. The Make Board Paneling dialog opens.
  4. Create array number one.
    1. In the Make Board Paneling dialog, enable the Route checkbox.
    2. Enable the Board Figure checkbox.
    3. Enable the Board Outline checkbox.
    4. Under Placement, select Move To and enter 0 for both X and Y.
    5. Click Add Board.
    Array number one is registered in the array list.
  5. Create array number two.
    1. Enable the Mirror checkbox.
    2. Select Y Mirror.
    3. Under Placement, select Move To and enter 137.2 for X and 0 for Y.
    4. Click Add Board.
    Array number two is registered in the array list.
  6. Create array number three.
    1. Enable the Mirror checkbox.
    2. Select X Mirror.
    3. Under Placement, select Move To and enter 0 for X and 140.8 for Y.
    4. Click Add Board.
    Array number three is registered in the array list.
  7. Create array number four.
    1. Disable the Mirror checkbox.
    2. Enable the Rotation checkbox.
    3. For Rotation Angle, enter 180.
    4. Under Placement, select Move To and enter 137.2 for X and 140.8 for Y.
    5. Click Add Board.
      Array number three is registered in the array list.
    6. Click Apply.
      The original data is copied and arranged as registered in the Array list.


    Figure 1.


    Figure 2.


    Figure 3.
  8. Create Panel outline.
    In the Define Panel outline section, you can define the Panel Board outline.


    Figure 4.
    1. For Start Location, enter -7 for both X and Y.
    2. For End Location, enter 144.2 for X and 147.8 for Y.
    3. For Line Width, enter 0.1.
    4. Click Apply.
      The panel board outline is drawn.
    5. Click Close to close the Make Board Paneling dialog.

Make Board Paneling using Gerber Data

  1. Launch PollEx PCB.
  2. From the menu bar, click File > Open and open the PollEx_PCB_Sample_r<revision number>.pdbb file from C:\ProgramData\altair\PollEx\<version>\Examples.
  3. Import Gerber data.
    When the Metal Mask Gerber of the panel board is prepared, the sub-boards can be automatically calculated by selecting the component pad of the design data and the pad object of the Gerber data.
    1. From the menu bar, click File > Import > Gerber (RS-274D/RS-274X).
      The Import from Gerber (RS-274D/RS-274X) dialog opens.
    2. In the Import from Gerber (RS-274D/RS-274X) dialog, click .
    3. Select all Top-Metal files from C:\ProgramData\altair\PollEx\<version>\Examples\MFG\Data\MetalMaskGerber.
    4. From the tool bar, click to disable routing data.
  4. From the menu bar, click Manufacture > Make Board Paneling.
    The Make Board Paneling dialog opens. The design file is saved as a *.pdbb file. If the file is not saved, the Make Board Paneling cannot be used.


    Figure 5.
  5. Create Array List by selecting CAD and Gerber data.
    1. In the Paneling Object Definition section of the Make Board Paneling dialog, enable the following checkboxes: Route, Board Figure, and Board Outline.
    2. In the Placement section, enable the Object Select checkbox and select CAD Object.
    3. Select the Pad to be used as the reference from the CAD data.


    Figure 6.
  6. Select pad based on Gerber data.
    1. In the Placement section, select Gerber Object.
    2. Select the Pad to be used as the reference from the Gerber data.
      X and Y distance between two selected objects from CAD and Gerber data is automatically calculated.
    3. Click Add Board to enter the first array information in the Array list.


      Figure 7.
    4. Move the main screen to the right-side of the board.
    5. Select the Pad to create the second array board.
      X and Y distance between the two selected objects from CAD and Gerber data is automatically calculated.
    6. Click Add Board to enter the second array information in the Array list.


      Figure 8.
    7. Click Apply.
      The original data is copied and arranged as registered in the Array list.


      Figure 9.
  7. Create Panel outline.
    Use the Get Panel Outline from Gerber option to define the Panel Outline.
    1. Click Get Panel Outline from Gerber.


      Figure 10.
      The Extract Board Outline dialog opens.
    2. In the Extract Board Outline dialog, select Replace.
    3. Click and drag to select a line to be defined as the Board Outline.
    4. Enable the Certain Width checkbox and enter 0.2.


      Figure 11.
    5. Click ALL.
      All lines with the same width as the previously selected line are automatically selected and displayed in purple in the Gerber data.


      Figure 12.
    6. Click Apply in the Extract Board Outline dialog.
      Selected lines from the Gerber data are changed to the Panel Outline.
    7. Click Close in the Make Board Paneling dialog.


      Figure 13.