Task 8: Setting the Conductor Clearances

In this task, you will learn how to set conductor clearances. Conductor clearances define the minimum clearances that are required for a design. Multiple clearances can be set for different sections of the design, including inner layer clearances and differential pair clearances, for example. A design rule stack is also defined within this section. You can have many different stacks within your design rule.

Electric Objects

  1. Select the Conductor Clearance tab, and then select the Conductor tab.
  2. In the Design rule group section, specify a new design rule of "0.1mm" and click Add. The specified value is added to the Design rule group list.

Figure 1: Setting the Design Rule Group

  1. In the Basic settings section, enter "0.10000" in the first cell of the Track row, (also the first cell of the Track column).

Figure 2: Basic Settings

  1. Copy the contents of this cell (first cell of the Track row/Track column) by pressing Ctrl+C.
  2. Display the Basic Settings tab by clicking the Display basic clearance settings dialog button.

  1. Click the arrow next to the Track row and drag the cursor down to cover the whole of the table. Press Ctrl+V to paste the value "0.10000" into all selected cells.

    Figure 3: Basic Settings

  1. Close the Basic settings dialog by clicking X.
  2. In the Design rule stack section, create an entry of "0.1mm" and click Add. The specified value is added to the Design rule stack list.

    3. Figure 4: Setting the Design Rule Stack

  3. In the Design rule stack section, select 0.1mm for each conductor layer in the Design rule group column. The design rule stack is now ready to use.

Figure 5: Setting Unit Values for Conductor Layers

  1. In the Default design rule stack list, set all of the fields to be "0.1mm".

Figure 6: Default design rule stacks

  1. Now set the distance to first corner. In the Design rule group section, set the Distance to first corner to be ‘0.20000’ for both surface mount and through-hole pins.

 

Note
These values set the minimum distance a track must be from the edge of a pad before it can turn a corner. This is to prevent acute angles into pads that may cause manufacturing issues with the board.

 

Figure 7: Setting Distance to First Corner

Figure 8: Example of DRC result of routing pattern violating the Distance to First Corner rule

 

  1. Click Save. At this stage, ignore any warnings or errors.
    This task is demonstrated in the following video.
Next topic: Task 9: Configuring Hole/Area Settings