6.1.2 Fabrication Outputs

  1. Click on “Add New Fabrication Output” and from the new window select Gerber Files and then [PCB Document].
  2. Click on “Add New Fabrication Output” and from the new window select NC Drill Files and then [PCB Document].
  3. Click on “Add New Fabrication Output” and from the new window select ODB++ Files and then [PCB Document].
  4. The outputs have now been specified and require a small amount of configuration.
  5. Single right click, Gerber Files and select Configure.
  6. The General tab should be have Inches and 2:5 selected, see Gerber – General Default image.
  7. The Layers tab will by default not have any layers selected (see image Gerber – Layers Default image). Select the Plot check box for all required layers and add Mechanical-1 to all layers, image Gerber – Layers Configured illustrates the required layers for a board with SMT components on both sides.
  8. The Drill Drawing tab will by default not have any plots selected (see image Gerber – Drill Drawing Default image). Select the two Plot All Used Drill Pairs boxes as per image Gerber – Drill Drawing Configured.
  9. The Apertures tab should have Embedded Apertures selected as per image Gerber – Apertures Default.
  10. The Advanced tab should have the options selected as per image Gerber – Advanced Default. The only time the settings need to change is for a very large design at which point the Film Size will change to allow the design to fit.
  11. The Gerber setup is now complete, press OK.

Figure 31 Gerber - General Default

Figure 32 Gerber  Layers Default

Figure 33 Gerber  Layers Configured

Figure 34 Gerber - Drill Drawing Default

Figure 35 Gerber  Drill Drawing Configured

Figure 36 Gerber - Apertures Default

Figure 37 Gerber - Advanced Default

12. Single right click, NC Drill Files and select Configure.

13. The Altium default values as per image NC Drill  Default should be used, press OK.

14. Single right click, ODB++ Files and select Configure.

15. By Default Altium includes all layers in the ODB++ file (see image ODB++ - Default image), inclusion of the mechanical layers in the past has proved to cause problem so they along with the keepout layer should be deselected as per image ODB++ - Configured then press OK.

Figure 38 NC Drill - Default

Figure 39 ODB++ - Default

Figure 40 ODB++ - Configured

The fabrication outputs are now configured, to generate the files left click on the Folder Structure logo in the Output Containers section, once the area is highlighted blue you will see a round button at the right hand end of each Fabrication output (see Output Container Folder), click in each button to select the file to be generated.

Figure 41 Output Container Folder

  1. In the Folder Structure section of the output containers click on Change, the window will be as per the Folder Settings  Default image.
  2. Single left click on Nonewhich will display the Folder Settings  No Container image, select [Container Name] (Folder Structure) or [Container Name] (Generate Files) as per image Folder Settings  Container Selected then press Done.
  3. The window should now look as per image Folder Settings  Configured.
  4. It is advised that Gerber files are checked using the CAMtastic application (supplied with Altium), to automatically load the Gerber files into CAMtastic after generation press Advanced from the Folder Structure Settings window then select Gerber Output from the CAMtastic Auto-load Options (see Folder Settings  Page View image).
  5. This completes the configuration, press OK.

Select Generate Content from the output container section, the files will be generated and once complete the Gerbers files will be displayed in CAMtastic (this will take some time).

Figure 42 Folder Settings - Default

Figure 43 Folder Settings  No Container

Figure 44 Folder Settings - Container Selected

Figure 45 Folder Settings  Configured

Figure 46 Folder Settings  Page View