This page is to help with understanding how to export your board in a format that manufacturers can use make your board. To do this we will be creating a series of files known as Gerber files that contain the information we input on each layer of the PCB in the Altium PCB Design workspace.
The information that the manufacturer uses to know where to remove material to create the edges and holes of your board is contained in the mechanical layers of the board. In particular, even though we defined the outline of the board in Altium using some sort of polygon, we need to trace the board outline onto Mechanical Layer 1. This can be done in a few ways.
Create Primitives From Board Shape
Altium has a built-in tool to trace the board outline onto a layer. This is found by selecting Design -> Board Shape -> Create Primitives From Board Shape. Once you have selected this a pop-up window will appear. The width option will trace the board outline with lines of the specified width and the layer option will specify on what layer the board outline is traced. While the width of the line is not important when it comes to manufacturing setting a reasonable value such as 20mil or so will make the board outline easy to see. For our purposes change the Layer option to Mechanical Layer 1.
If you don't see this option in the Design drop-down menu make sure that you have the PCB you want to edit in the active window. This will automatically change each dropdown menu for the context of PCB editing.
Alternatively, you can opt to trace the board outline manually. Select Mechanical Layer 1. Use the Line tool to trace the perimeter of the board. The Line tool can be found by going to Place -> Line or by selecting it from the toolbar in the active PCB Editor window.
The Gerber Setup Wizard
We are now ready to export our board as a series of Gerber files. Make sure that the board you want exported is selected and go to File -> Fabrication Outputs -> Gerber Files. This will open a wizard that allows you to customize how your files are exported.
In the General tab of the wizard make sure that the Unit is selected to inches and the format is selected to 2:5. The units may change depending on the manufacturer but many manufacturers in the US use the imperial measuring system as a standard. The format has to do with how precise the final files will be. The format 2:5 specifies that the precision will be up to 0.01mil.
Once you have selected these options move to the Layer tab of the wizard. This allows you to select which layers will be exported as Gerber files. We want to select all of the layers that we used to design our board in Altium, so to do this we locate the Plot Layers drop-down menu and select the Used On option. You will notice that after selecting this all of the layers in our design were automatically checked for export.
Finally, for a basic design, we can leave all of the other settings at their default values. Click OK to close the wizard.
Understanding the Gerber Files
After hitting OK on the wizard you will see that a new file has been created in the Source Documents tab of the Projects panel. It will have a name along the lines of CAMtastic1.cam. This file is an interim document used to generate the individual Gerber files for each layer. It can be ignored and even deleted if desired. To find the individual Gerber files that were created click on the Generated folder in the Properties panel and navigate into the CAMtastic! Documents folder.
If you have been following along so far you will notice that there are a series of files that have the format of boardFilename.G** where * represents some character (e.g. .GTL, .GBO, .GTP, .GM1, etc.). The G in the extension stands for Gerber and the following two characters represent the layer that was used to generate the file. For example .GTL stands for Gerber Top Layer, .GBO stands for Gerber Bottom Overlay, and .GM1 stands for Gerber Mechanical 1. Verify that each of the files makes sense with how you designed the board. If you are creating a stencil for surface mount components be sure that the .GTP layer (Gerber Top Paste) includes all of the pads of the SMD components without any oddities.
Creating Drill Files
Even though we have created Gerber files for the board layers we still need to create an additional set of files to define the holes to drill. This is done in a similar manner as generating the Gerber files. Go to File -> Fabrication Outputs -> NC Drill Files. This will open a popup window similar to the Gerber Setup Wizard. Once again set the units to inches and the format to 2:5. Check the box that says "Generate separate NC Drill Files for plated & non-plated holes". Leave the other settings as their defaults and click OK. You will notice another Camtastic file has been created in the source documents. This one similarly can be ignored. If you navigate to where your Gerber files are located you will see new text documents containing the information for the holes to be drilled. Verify that this appears correct.
Zip The Files
You now have all the files needed for a manufacturer to be able to reproduce your board. In order to send it to a manufacturer we will need to zip the files together. To do this, navigate to the location of your Altium project in your file explorer. Once inside your project folder you will see a folder titled something like "Project Outputs for...". Navigate into this folder and verify that it contains the Gerber and Drill files you just created. You will notice that there are several other files in this folder as well. These can be ignored. Zip up the folder. It is a good idea to send this zip file to yourself via email as you will most likely be making a purchase through a computer in the ECEN office.
Congratulations! You successfully exported files for your custom PCB to be manufactured!