Altium: PCB Layers configuration when importing footprints

Question

This is my first time using Altium and I'm still a beginner with PCB design. I want to import the symbols and footprints of the components from different sources (Websites, existing projects...) but I'm concerned about the layers configuration, because the footprints might be using different layers. So I want to know how to solve that problem without having to redo the footprint? Also would importing all the components symbols and footprints from the same website (for example, SnapEDA) mean that they all have the same layer-configuration?

Answer 1

On the PCB, you can:

• Enable all layers (bottom-left tab in PCB view, "LS" (Layer Sets), or D T A key sequence; or there may be another shortcut / menu in newer versions, I use AD16)
• SHIFT+S (single layer mode) and flip through layers (or NUM+, NUM-, etc.), see which layers are used and which need to be swapped to your preference
• Select the components that have incorrect layers, untick "Lock Primitives" in Properties (suggest leaving Properties dialog/panel always open on the side for quick reference)
• Go to those layers, select objects, and change the Layer parameter in Properties
• Remember to re-lock primitives on all modified parts! (The selection can be stored and recalled with CTRL+1 and ALT+1 (or other numbers) respectively, if you like.)

This is a somewhat brittle solution, as updates from library will wipe the changes. You are encouraged to either update the libraries themselves (saved locally, they're yours to play with, license terms notwithstanding), or build your own by copy-pasting components or library contents into others.

Advanced: this can also be done without unlocking primitives, using the query system.

• Open the Query panel/dialog
• Enter query: OnLayer('Mechanical 7') (or whatever layers shouldn't be used); this will select all objects on the quoted layer. Note name must be an exact match; check L (Layers / View Configuration) for names (also D K (Layer Stackup) to edit copper layer names).
• In Properties, change the Layer parameter to the correct value.

For some reason, objects selected and edited in this way are not prevented by the primitives lock.

Footprints can also contain copper layers; if no useful objects have been placed on them, they can be removed in the Layer Stack Manager. (Double-check your layer and dielectric thicknesses, names and ordering; they may be messed up as a result.)