d | FreePCB User Guide | Version 1.2

PREV | Table of Contents | NEXT

7. Tutorial (continued)

7.11 Checking Design Rules

Design Rules are a set of rules that establish lower limits for dimensions such as trace widths and clearances. They are necessary because the PCB manufacturing process is subject to certain limitations and tolerances, and the design has to allow for this. For example, you can't use trace widths of 1 mil in your layout, because it is physically impossible to etch them reliably.

If you are having your PCBs made for you, the board house should provide design rules based on their process. For example, Advanced Circuits recommends the following for their low-cost process:

Minimum trace width | 0.008 inch
Minimum clearance between copper features | 0.008 inch
Minimum distance from copper to edge of PCB | 0.014 inch
Minimum annular ring width (pins) | 0.007 inch
Minimum annular ring width (vias) | 0.005 inch
Minimum silkscreen line width | 0.008 inch

The Design Rule Checker (or DRC) is a tool that you can use to make sure that your project doesn't contain any violations of these rules. These are referred to as DRC Errors. Since your tutorial project may not actually contain any DRC Errors, I would suggest that you close your project and instead open C:\freepcb\tutorial\motor_drc_errors.fpc, as shown below. This contains several typical errors. See if you can spot them.

Now let's run the Design Rule Checker. You can launch it by selecting the Tools > Design Rule Check menu item. This will pop up the following dialog:

We will modify the fields in the dialog to match the Advanced Circuits values. Trace width should be set to 8 mils. The pad to pad, pad to trace, trace to trace and copper area to copper area values should be set to 8 mils. The annular ring (pins) values should be set to 7 mils, and the annular ring (vias) value should be set to 5 mils. The board edge to any copper field should be set to 14 mils. The hole to pad or trace, board edge to hole and hole to hole values are not given, so let's use 25 mils which seems reasonable. Your dialog should look like:

Now click OK to run the checker. A new dialog should pop up with a list of errors, as shown below.

Errors 0 and 1 are violations of the minimum clearance between pads and the board edge. Errors 2 and 3 are trace-to-pad violations. If you look closely at the layout window, you will see that symbols consisting of small orange rings have been placed at the site of each error, as shown below.

These small circles may be hard to see, but if you press the "d" key on the keyboard they become much larger solid circles, as shown.

Now zoom in on one of the errors, such as the one at U1.16.

Click on the DRC Error ring to highlight it. The PCB elements that caused the violation will also be highlighted, as shown. Also, a description of the error will appear in the status bar.

In this case, the error is a clearance violation between pad U1.16 and the trace segment passing through it, which are not on the same net. Oops! You can fix the error by rerouting the trace to avoid the pad, as shown. Note that the DRC Error symbol doesn't automatically disappear, but you can delete it by selecting it and pressing the "Delete" key, or by re-running the Design Rule Checker.

Now let's zoom in on the DRC Errors on the left side of the board, and select one of them.

In this case, the error is a pad-to-board-edge violation. Basically, JP6 is too close to the edge of the board. We can solve the problem by moving it further to the right, as shown.

I will leave it up to you to find and fix the last error. Then you can run the Design Rule Checker again, which should not find any errors.

You should reload your motor.fpc project before beginning the next section. When you close the motor_drc_errors.fpc project, I would suggest that you do NOT save your changes, so you or someone else can use it again.

PREV | Table of Contents | NEXT