KB: Convert from Gerber to PCB

Created: March 25, 2021 | Updated: September 4, 2023

Creating a PCB from a Gerber file

Starting in Version: 18.0
Up to Version: Current

Solution Details

This documentateion goes into a great deal of detail for this topic (with screenshots):

Here is a summary:
The Gerber files can be reverse engineered. Note that if your board has any through holes, meaning it is more complex than a single-layer piece of routing, then you must provide at least two Gerber files, one for the top, the other for the bottom and an NC Drill file (ASCII). 
All Gerber layers in the CAMtastic document must be assigned to an appropriate layer type. CAMtastic attempts to do this for you, matching the extensions of your Gerbers with those listed in the Layer Types Detection Template, but you should always review the Layers Table for completeness and accuracy. Mechanical layers should be set to Temporary. 
Once all layers are correctly assigned, you should review the Layers Order Table, ensuring that the stack-up of the board is correct. 
This facilitates the next step, which is to group drill layers in the Layers Sets Table. If your entire board uses through-hole technology, the only set to define is one for all the layers, this step may even be skipped. But if your board contains blind and/or buried vias, you must designate each drill set individually, associate the corresponding NC Drill file, and select all layers through which that drill set will pass. 
At this point, you may extract a netlist from the CAMtastic file, as this will trace nets from one layer to another according to the layer stackup and drill-pairing sets you have provided. If you included IPC netlist files with your Gerber and NC Drill files, you may restore the original net names. An IPC netlist will also differentiate between through-hole vias and free pads in your new PCB file. 
When CAMtastic exports a PCB, a board outline will automatically be generated. To do this intelligently, it requires a closed polyline to be present upon a Border-type layer. If no closed polylines can be found on this layer, or if multiple layers have been designated as borders in the Layers Table, you will probably not get the Board Shape you desire. In CAMtastic, closure is a property, not attained simply by looping a series of lines back to the starting point. Such lines, if they exist already, may be joined by choosing Edit ► Objects ► Join. If you want to draw your own closed polyline, right-click after selecting its final vertex, and choose Close
All split planes must be defined by closed polylines on the internal plane layers. Island planes may have their borders converted to a closed polyline by joining, but split planes that share their outlines with other splits or with the pullback traces along the board edge must be redrawn. Nested planes such as islands within split planes are not supported by the CAMtastic Export to PCB, but they are supported in Altium Designer's PCB editor. You will simply need to reassign the correct nets to island split planes once you finish the Export from CAMtastic. 
In conclusion, CAMtastic’s Export to PCB function will create a board very much like the original. To truly rebuild a board will still take some manual labor, such as replacing primitives with footprints, simply copy and paste groups of primitives into a PCB library, then replace the originals with the new footprints. Additionally, the Layer Pairs in the Layer Stack Manager, should they be required, have to be redefined manually. 

This document is older, but may still be of interest:


This is the simplified process. 
  1. File ► New ► CAM Document 
  2. File Import Gerber(s) 
  3. File Import Drill (Browse to drill file) 
    1. If you don't have a drill file you can create one by placing a via on a new PcbDoc then export it as NC drill
  4. Tables Layers (assign the layer types)
  5. Tables Layers Order (Confirm the logical & physical Layer order is correct) 
  6. Tables Layers Sets (ensure your drill span shows up here)
  7. Tools Netlist Extract 
  8. File Export Export to PCB 
If you are working with a footprint Gerber, then you may try opening it in Altium Designer, and perform:
File Export DXF
Then open the PcbLib (File Import AutoCAD) or PcbDoc (perform File Import DXF/DWG)
Was this article helpful?
Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
200 characters remaining
You are reporting an issue with the following selected text
and/or image within the active document: