| FreePCB User Guide | Version 1.2

PREV | Table of Contents | NEXT

7. Tutorial (continued)

7.12 Making Gerber and Drill Files

The final step in this tutorial is making the Gerber files and Drill file which you would send to the PCB manufacturer. You might want to review Section 5.18: Exporting Gerber and Drill Files before proceeding.

Select Generate CAM files... from the File menu. "CAM" is an acronym for "Computer-Aided Manufacturing". The following dialog should appear.

In the Files section, select the files that you wish to create by checking or unchecking the boxes next to them.

In the Gerber file options section, you can select:

- Include board outline - add the board outline to each Gerber file

- Add moires - add moire patterns (also called "targets") to each Gerber file

- Add layer description text - add a text string describing the layer to each Gerber file

- Add pilot holes - add pilot holes to pads and vias on the top and bottom layers

- Use thermal reliefs for pins - use thermal reliefs to connect through-hole pins to copper areas

- Use thermal reliefs for vias - use thermal reliefs to connect vias to copper areas

- Make cutouts in solder mask for vias - make openings for via pads in the solder mask layers

The Gerber file dimensions section allows you to set numeric parameters for the Gerber files. When you make a real board, you would get these from the PCB manufacturer. The values shown above are fairly typical of a low-cost, multilayer process.

- Copper to copper-fill clearance - the clearance that will be created around traces and vias that pass through copper areas.

- Hole-edge to copper-fill clearance - the clearance that will be created around holes through copper areas.

- Solder mask clearance - the clearance that will be created around pads and vias in the solder masks.

- Pilot hole diameter - the diameter of pilot holes in pads, if you chose to include these.

- Minimum silkscreen stroke width - the minimum line width that will be used for items on the silkscreen layers.

- Thermal relief line width - the width of the lines in thermal reliefs, which connect pads to copper areas.

- Board outline line width - the width of the lines used to draw the board outline.

- Annular ring width (pins) - the width of annular rings placed around inner layer pin holes for thermal relief connections.

- Annular ring width (vias) - the width of annular rings placed around inner layer via holes for thermal relief connections.

The Output folder is the destination folder for the files which will be created. By default, this is a subfolder of the project folder named "CAM". You can change it if you like. The folder will be created if it doesn't already exist (although its parent folder must exist).

Now click Create files to make the files. The following dialog should appear.

If there were any errors, messages will appear in the dialog. Usually, an error will result in FreePCB aborting that file and going on to the next one. Click OK to dismiss the dialog.

Now you can view your Gerber and drill files using a Gerber Viewer such as ViewMate by PentaLogix (which is free, and available here). ViewMate can also print check plots on your printer. You should ALWAYS check your files before using them to make a PCB. Also, read Section 5.173: Drill Sizes for important information about the drill file.

Screenshots of the Gerber files for the top silk-screen, top copper and inner 1 copper layers of our tutorial project are shown below. These look pretty crude in the screenshots. To appreciate just how precise they really are, you should open your own files in ViewMate and zoom in on some of the smaller features.

Well, that's the end of the tutorial. I have tried to cover most of the major features of FreePCB. Now you should be ready to create a board of your own.

PREV | Table of Contents | NEXT