Defining Rules for a PCB

You can keep working with your project or open it from the Workspace and continue from where the previous step is completed.

A printed circuit board is always designed according to certain rules. They are created in the PCB Rules and Constraints dialog accessed by selecting Design » Rules. More details about the PCB Rules and Constraints dialog can be found here.

Fig. 28 - PCB Rules and Constraints editor — **Fig. 28** - PCB Rules and Constraints editor

We are going to use the following rules:

Clearance from the Electrical section. Choose an existing rule and specify a value of 0.2mm for all objects. It is enough to enter it once in the Minimum Clearance parameter. Also select the Ignore Pad to Pad Clearances within a footprint option to ignore the minimum clearance rule between Pad belonging to the same Footprint.

Fig. 29 - Clearance settings — **Fig. 29** - Clearance rule configuration

Width from the Routing section. Three rules should be created here, namely Width_POWER, Width_Shell, and Width. They are used to assign track widths for the three different types of nets. Before creating rules for this category, let's first create Net Class Power, which will include power and GND nets. To do this, select the Design » Classes from the PCB editor main menus, and the Object Class Explorer dialog opens.

Fig. 30 - Adding a new class — **Fig. 30** - Adding a new class

Right-click on the Net Classes section and then select Add Class. Name the Net Class as POWER. In the left column, search for GND, VCC_3.3, and VCC_5V nets and move them to the right column using the button. The result should be as follows:

Fig. 31 - Moving nets — **Fig. 31** - Moving nets

Press OK.

In the PCB Rules and Constraints Editor dialog, create a rule named Width_POWER. In the Where The Object Matches region, select Net Class, set the value to POWER and specify the track width as shown below.

Fig. 32 - Width rule configuration for the Net Class — **Fig. 32** - Width rule configuration for the Net Class

Create the Width_Shell rule. In the Where The Object Matches region, select Net, set the value to NetJ1_Shell and specify the track width as shown below.

Fig. 33 - Width rule configuration for the Net — **Fig. 33** - Width rule configuration for the Net

Select All for the Width rule in the Where The Object Matches region. The width of these signal routes will correspond to a transmission line with an impedance of 50 ohms. Check the Use Impedance Profile option and select S50. The track width data will automatically fill in and will match data in the Layer Stack Manager. The result is shown below.

Fig. 34 - Width rule configuration for the All Nets — **Fig. 34** - Width rule configuration for the All Nets

Note: One of the most common mistakes made by beginners is the incorrect priority of created rules. For example, if there is a rule at the very top of the rule tree with "Where The Object Matches" set to "All", it means that it will deliberately exclude all the rules below it (lower in priority). You can check how many objects are covered by the rule by clicking "Test Queries". Use the "Priorities..." button to set the priority.

Routing Vias Style from the Routing section. The values should be set as shown below.

Fig. 35 - Routing vias rule configuration — **Fig. 35** - Routing vias rule configuration

Differential Pairs Routing from the Routing section. Check the Use Impedance Profile option and select D90. The data will automatically fill in and will match data in the Layer Stack Manager. The result is shown below.

Fig. 36 - Differential pair rule configuration using Impedance Profile

Polygon Connect Style from the Plane section.

Fig. 37 - PolygonConnect rule configuration — **Fig. 37** - PolygonConnect rule configuration

Minimum Solder Mask Sliver from the Manufacturing section. Set the value to 0,04mm.

Fig. 38 -Configured Solder Mask Rule — **Fig. 38** - Configured Solder Mask Rule

Component Clearance from the Placement section.

Fig. 39 - Configured component clearance rule — **Fig. 39** - Configured component clearance rule

Don't forget to click OK and save the project locally and to the Workspace.

Good job! Article is now completed!

Completed Completed

article Previous

article Next

CAPTCHA

Was this article useful?
Yes No

Thank you Glad to hear it