How to Generate Gerber and Drill Files in PCB Wizard
PCB Wizard is an easy-to-use package for designing single-sided and double-sided printed circuit boards (PCBs) from New Wave Concepts Limited.
To produce Gerber files, select Tools → CAD/CAM → Export Gerber from the menu bar.
A window will appear that allows you to specify some options.
Select all layers.
Check Place each exported layer in a separate output file
Include aperture table within output file will be automatically checked if RS-274X is used.
Check Fill pad drill holes
Now click OK, some Gerber files and the drill file will be generated in the project folder.
Let’s have a look at the generated files:
With these file names, we can’t be told what’s the function of each file. Even though we can see the function of each file in Figure 2, but when we pass the files to a PCB fab house, this important information will be lost. JLCPCB prefers Protel naming conversions, so let’s change the filename extensions according to Figure 2.
|By default, filename extensions are hidden in Windows, for how to show them, just google "show filename extensions windows".|
Rename .gb0 to .GKO (board outline)
Rename .gb1 to .GBL (bottom copper layer)
Rename .gb2 to .GTL (top copper layer)
Rename .gb3 to .GTO (top silkscreen)
Now the folder looks like this:
If we look at these files, we can see the files for soldermask are missing, let’s generate them.
Again, select Tools → CAD/CAM → Export Gerber. The window for options will appear, this time just check one more option than the first time:
Check Plot pads only (this will only generate the top and bottom soldermask instead of the copper patterns)
Click OK button to generate the files.
We now have the following files in the project folder.
Rename .gb1 to .GBS (bottom soldermask)
Rename .gb2 to .GTS (top soldermask)
Delete .gb0 and .gb3
These are the files we get at the end:
Fix the drill file
If we open the .drl file with a text editor (Excellon files are plain text files), we can see something like this:
The problem of this file is that the tooling information between M48 and % sign is not included. In fact the tooling information (the size of all used drill bits) is a .inf file.
We can just add this tooling information into the drill file manually (please note the Tnn lines after M48 in the screenshot below). The syntax is simple:
nn in Tnn are tooling numbers.
After Tnn is a letter C.
After letter C, is the size of this tool.
Verify the files
Before uploading your Gerbers and drill file to JLCPCB for production, it’s highly recommended to cross-check the generated files with a 3rd-party Gerber viewer.
If you find any issues, fix them and export the Gerber/Drill files and check them in the Gerber viewer again.
There are some nice Gerber viewers here and there, just use the one you feel handy.
If everything is OK, now you can move the production files into a folder (include the .inf file), zip it, upload it to JLCPCB to place the order.