To panelize the PCB from altium do the following:

1) from your PCB document click File→Fabrication output→gerber files. This will create a camtastic document (CAMtastic1.Cam).

2) from your PCB document click File→Fabrication output→NC drill files. Check the Generate Board Edge Rout paths and set Rout tool Dia =10mil. Click Ok. This will produce another camtastic file (CAMtastic2.Cam). From this camtastic file click file→export→save drill. Save the drl file (cam.drl).

3) Now go back to CAMtastic1.cam document. Click File→import→Drill. Select the cam.drl file you created in step 2.

4) Now in Camtastic1.cam click Tools→Panelize. Select the whole board by clicking and dragging when selected click again and all parts on the board should be selected. Press Shift+ F9, this should bring up the panelize menu. Choose your dimensions and then click ok.

5) Now you should see the panelized version. Now click File→Export→Gerber and these should include the cam.drl file. Make sure you UNCHECK cam.drl because freedfm wants a drill file that is not a gerber file and this process produces gerber files. You need to do the drill in a separate step.

6) To save the drill file do File→Export→Save drill. Then make sure you select the cam.drl layer should be the last layer. Click ok and this should save the right drl file.

7) Done.

To panelize different designs on one PCB go to PCB panelize different