1. Blog>
  2. How to Export Gerber File From PCB Wizard

How to Export Gerber File From PCB Wizard

by: Jul 18,2023 2548 Views 0 Comments Posted in PCB Design Tutorial

Tutorial PCB design Gerber PCB Wizard

Generate Gerber

Select the menu bar, click on "Tools" -> "CAD/CAM" -> "Export Gerber", as shown in the following figure.

Figure 1. Export Gerber Menu Bar Option

After clicking, a new interface will pop up. Please follow the settings indicated by the red box in the figure below.

Figure2. Gerber Setting Interface

Then click OK, and the generated Gerber file will be located in the same path as the .pcb file.

Figure3. Generated Files

For the PCB manufacturer, besides recognizing that files with the ".drl" extension are drill files, they do not know the functions of files with the .gb0, .gb1, .gb2, and .gb3 extensions. Therefore, we need to perform a naming conversion based on Figure 2 to adopt the Protel naming format.

After renaming:

  • .gb0 is renamed to .GKO (Board Outline).
  • .gb1 is renamed to .GBL (Bottom Copper Layer).
  • .gb2 is renamed to .GTL (Top Copper Layer).
  • .gb3 is renamed to .GTO (Top Silkscreen Layer).

Figure 4. File Extension Modification

When checking these files, it will be noticed that the soldermask layer files are missing. Next, let's generate them.

Generate Soldermask

Select the menu bar again, and click on "Tools" -> "CAD/CAM" -> "Export Gerber." After that, the Gerber settings window will appear. follow the settings indicated by the red box in the figure below (check the option "Plot pads only"). Click OK.

Figure 5. Select Plot pads only

Click OK, the generated file is as shown below:

Figure 6. Generated Soldermask Files

As shown in the above figure, the .gb0 and .gb3 files are not required and can be deleted. Rename .gb1 to .GBS and .gb2 to .GTS.

Figure 7. File Extension Modification

Fix the Drill Files

The problem with the PCB Wizard is that the drill file is not a proper Excellon file, it lacks the header. This means that there will always be a need for someone to manually input the tool sizes before manufacturing. Some PCB manufacturers do not accept incomplete drill files, using the default tool size during import will result in all vias being the same. To avoid this issue, we need to process the drill file after exporting Gerber.

Open the .inf file in the Gerber folder using Notepad, and scroll to the bottom. Copy the tool size "T01   .020".

Figure 8. Copy Tool Size

By opening the .drl file in the Gerber folder with Notepad, we can see the content as shown in the following figure: The units and tool sizes are missing between M48 and %.

Figure9. Open .drl file by Notepad

Now we will need to add the unit "INCH" below M48 (the unit used when exporting Gerber). Then, paste the copied tool size "T01   .020" under the "INCH" unit. We need to modify the pasted tool size to the format: tool name T01, followed by the capital letter C, and then the size 0.020. The final result should appear as shown in the following figure.

Figure 10. The fixed Drill File

Save the file.

Join us
Wanna be a dedicated PCBWay writer? We definately look forward to having you with us.
  • Comments(0)
You can only upload 1 files in total. Each file cannot exceed 2MB. Supports JPG, JPEG, GIF, PNG, BMP
0 / 10000
    Back to top