Each output has two set-up windows, “Page Setup…” and “Configure…”, see the Configuration Menu image. The Page Setup window (See Page Setup image) is common to all documentation outputs, the Configure window content varies between PCB and schematic outputs. To access the set-up windows single right click the output name.

For all PCB print outputs select Page Setup and ensure the Scale Mode is set to Scaled Print and the Scale is 1.00, also the colour set should be Mono, then press Close.

For all schematic outputs select Page Setup and ensure the Scale Mode is set to Fit Document On Page, also the Colour Set should be Colour, then press Close.

Once the page setup for all the outputs has completed it is necessary to setup the configuration (see images following for information).

1. For the “…Layout” output right click the output name again then select Configure (see Configuration Menu image).

2. The new window (see PCB Config – Default image) will display a Multilayer Composite Print, this will need to be changed to generate single images for each Gerber layer.

3. By default, Altium includes all mechanical layers on all PCB prints, it is possible to manually remove the included layers (details following), alternately, it is possible to automatically include just the required layer (typically Mechanical-1). To set the required mechanical layer, select Preferences from the lower left of the PCB Printout Properties window (see PCB Config – Default image). The window displayed in PCB Config – Mechanical Preferences image is now displayed, remove the checkmarks from all the mechanical layers that are not required to be on every Gerber image & then press OK, in this example just Mechanical-1 is included.

4. Right click into the white area beside the layer names under Multilayer Composite Print and select Create Final (see PCB Config – Options image).

5. You will be promoted to confirm the creation of the final print set (see PCB Config – Confirm Action image), select Yes.

The Final Set (and any other PCB documentation outputs) contains Printouts and Layers, the printouts relate to the individual sheets in the PDF file and the Layers are the image(s) that will appear on the sheet.

6. The printout properties window will now be populated with each existing layer of the PCB (see PCB Config – Final Set image), some editing of the list is required to create the desired outputs.

7. This step is only required if the mechanical layer preferences (Step 3) were not changed. For each printout highlight (single left click, See PCB Config – Select Layers image) unwanted mechanical layers (typically just Mech-1 should remain), single right click and select Delete. 

Multiple Layers can be selected by holding down CTRL & mouse click.

Please note that the unwanted layers can only be removed from one Printout at a time, it is not possible to select Layers in different Printouts.

8. There will be unwanted Printouts generated in the Final Set, these are Top Pad Master, Bottom Pad Master & Keep-out Layer plus any mechanical layers that do not contain information you want printed i.e Mech-1,2,13. Single left click the unwanted Printouts using CTRL + mouse click to select multiple Printouts (see PCB Config – Unwanted Printouts image) then single right click and select Delete.

9. Once edited you should have a list similar to that in the PCB Config – Printouts Revised image.

10. Press OK to save the details.

11. For the “…Mask Prints” output right click the output name again then select Configure (see Configuration Menu image).

12. Repeat steps 2-10 with the exception that Create Mask Set should replace Create Final. The result should be as per the PCB Config  Mask Set Revised image below.

13. For the “…Schematics” output right click the output name again then select Configure, the default settings are correct and should be as per the Schematics Config  Multi Sheets Final image below, press OK.

14. Repeat step 13 for the “…RFQ” output. Please note the properties will be as per Schematics Config  Single Sheet Final image.

15. Repeat step 13 for the “…Build” output. Please note the properties will be as per Schematics Config  Single Sheet Final image.

The documentation outputs are now configured, to generate the files it is necessary to use the various Output Containers located on the right hand side of the screen (see Output Containers image).

Left click on the PDF 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 documentation output (see Output Container PDF - Separate image), click in each button to select the printouts to be generated.

By default, Altium adds component links, bookmarks etc. to PDF outputs, whilst helpful, this has the disadvantage of creating large files (>20Mb), it is possible to not include the additional data be adjusting the settings as below:-

1. From the PDF Output Management window, select Advanced.
2. Remove the checkmarks from “Generate Table of Contents”, “Include Component Parameters” and “Generate nets information”.
3. The adjustments listed below for specific outputs can then be followed.

It will be necessary to execute the output generation twice, once to generate the five (in this example) separate files and once for a combined file with both schematics and PCB layout.