Setting the New Standard in Electronics Design.

Efficiency. Collaboration. Accuracy.

Switch and Get the Power to Design Without Limits

Get 50% off when you switch to Altium Designer before April 26, 2024

Create Your Own PCB / Configuring the Basic Rules Completed Sign In To Save Your Progress
Click if you find this content useful

Create Your Own PCB

Configuring the Basic Rules

Correct rules definition is a very important step in the PCB design process. These rules describe to CAD the restrictions for manufacturing, impedance control, and routing parameters, and what can and cannot be done within the design. These rules cover everything from the minimum width of the conductor to the maximum height of the component in a particular area of the PCB. Any mistake or failure to comply with the rules can lead to problems, up to and including the complete inoperability of the PCB or the impossibility to manufacture or assemble it. Rules in Altium Designer are presented in the form of a hierarchy - from the fundamental rules covering the entire board to the rules of individual net classes. The rules in Altium Designer are set up using the PCB Rules and Constraints Editor dialog, which is a modern and powerful tool for design rules management.

You can access the PCB Rules and Constraints Editor dialog at any time your PCB is open by selecting Design > Rules from the main menus. You will soon see that setting even the most complicated rules in Altium Designer is incredibly easy and clear. Let’s set the design rules for our drone PCB.

First, we need to configure a basic rule for net-to-net clearance for all nets in our PCB.

Open the PCB Rules and Constraints Editor dialog. In the left pane of the dialog, there is a list of the types of rules you can set. Expand the Electrical region then expand the Clearance sub-region. There is a single Clearance rule, which we will configure.

Default rule to set up Clearance values
Fig. 1. - Default rule to configure Clearance values

Select Clearance. On the right side of the dialog, the current rule settings are displayed. Under the Constraints region, set the Minimum Clearance to 0.1mm for Different Nets Only

Clearance rule configuration
Fig. 2 - Clearance rule configuration
Tip: To configure a single clearance rule for different objects, update the cell where the objects intersect in the table near the bottom of the dialog.

Click Apply at the bottom-right of the dialog to save the settings. In addition to the clearance rules, the Electrical region allows you to configure the rules for Short-Circuit, Un-Routed Nets/Pins, Modified Polygons, and Creepage Distance. These rules are not required within the scope of this guide.

Now we will configure the mandatory Routing rules.

Expand the Routing region. Let’s configure the Width rules. Expand the Width sub-region then select Width.

Default Width configuration
Fig. 3 - Default Width configuration

The constraint manager for all traces of our project is displayed. You can set minimum, preferred and maximum widths for every layer of your PCB. Common traces of our drone PCB should be routed with 0.15mm width and shall not exceed 1mm and be less than 0.1mm, so set Min Width to 0.1mm, Preferred Width to 0.15mm and Max Width to 1mm as shown below.

Width rule configuration
Fig. 4 - Width rule configuration

Previously, we created a separate Net Class containing power nets. Now it’s time to add another width rule that will only work on the Net Class we created. Right-click on the default Width rule then select New Rule from the context menu.

New width rule for power nets is created
Fig 5 - New Width rule for power nets is created

Open Width_1. We need to limit the rule to the Net Class we created earlier. Click the drop-down menu in the Where The Object Matches region then select Net Class. In the right-hand drop-down, select Power. This selection limits the applicability of the rule to one net class.

Restriction of the rule for one net class
Fig. 6 - Restriction of the rule for one net class.

Currently, default values are set for Min Width, Preferred Width, and Max Width. Set Min Width to 0.2mm, Preferred Width to 0.4mm and Max Width to 1mm

Configured widths for a new rule
Fig. 7 - Configured widths for a new rule

Our rule has the default name Width_1. Since we have only two rules, we can remember that this rule is responsible for the width of a separate net class, but how do you keep track of the rules when there are several more? Renaming the rules at this stage will significantly increase the understanding of the rules in the future. You can specify the rule name in the Name field when the rule configuration window is open. Enter the name Width_Power in the Name field. Click Apply at the bottom of the dialog to save the rule.

Tip: You also can add a comment for your rule in the Comment field if desired.
Rule for power nets now has a clear name.
Fig. 8 - The rule for power nets now has a clear name

Now we need to set the range of allowed vias for our PCB. Expand the Routing Via Style sub-region then select RoutingVias.

Default rule to setup vias configuration
Fig. 9 - Default rule to configure vias 

Let's assume the company that will manufacture our PCB can execute the minimum via hole size at 0.15 mm and via pad at 0.1 mm (0.15mm/0.35mm), however, the main via size will be 0.2mm/0.4mm. Define the Minimum Via Diameter as 0.35mm, the Preferred Via Diameter as 0.4mm, the Minimum Via Hole Size as 0.15mm, and the Preferred Via Hole Size as 0.2mm. Click Apply to save the rule.

Routing vias rule configuration
Fig. 10 - RoutingVias rule configuration

Our PCB design implies the use of a differential pair. It is known that separate requirements to impedance are applied to a differential pairs routing, so we need to configure it. There is only the USB_P/N differential pair so our rule will be set for all differential pairs. Expand the Differential Pairs Routing sub-region then select the DiffPairsRouting rule.

Default rule to setup differential pairs routing configuration
Fig. 11 - Default rule to configure differential pairs routing

As part of the creation of the PCB stackup, we created an impedance profile for differential nets with 90 ohms impedance. Now we can use it for instant differential pairs configuration. Enable the Use Impedance Profile option in the Constraints region. The width values will be updated based on the specified impedance. That’s all there is to it! Quick and easy, right? Click Apply to save the rule settings.

Quick differential pair rule configuration using Impedance Profile
Fig. 12 - Quick differential pair rule configuration using Impedance Profile

The next mandatory step is to specify the size of the solder mask expansion and the solder paste indent.

Expand the Mask region, expand the Solder Mask Expansion sub-region then select SolderMaskExpansion.

Default rule for Solder Mask Expansion definition
Fig. 13 - Default rule for SolderMaskExpansion 

Set Expansion top to 0.1mm. Make sure that the link between the Expansion top and Expansion bottom expansion is enabled as shown below (click to enable/disable). Click Apply to save the rule configuration.

Configured Solder Mask Rule
Fig. 14 - Configured SolderMaskExpansion rule

Expand the Paste Mask Expansion subsection then select PasteMaskExpansion.

Default rule for Paste Mask Expansion definition
Fig. 15 - Default rule for PasteMaskExpansion 

Set Expansion to -0.05mm. In order to improve the solderability of the components, it is recommended to set the paste expansion smaller than the pad size. Click Apply to save the rule configuration.

Configured Solder Paste Rule
Fig. 16 - Configured PasteMaskExpansion rule

The last step in configuring the mandatory basic rules for the current project is to specify the component placement rules, specifically, the rule of vertical and horizontal clearance between the components. Our PCB is a part of a multi-board assembly and any miscalculation in the design of a single part of the device endangers the final assembly and operability of the entire unit. Let's create the rule.

Expand the Placement region. Expand the Component Clearance sub-region then select ComponentClearance.

Default rule to setup vertical and horizontal clearance between components
Fig. 17 - Default rule to configure vertical and horizontal clearance between components

Set Minimum Horizontal Clearance to 0.05mm and the Minimum Vertical Clearance to 0.1mm. Click Apply to save the rules. Close the PCB Rules and Constraints Editor dialog. Our work is done here.

Configured component clearance rule
Fig. 18 - Configured ComponentClearance rule
Good job! Article is now completed!
Sign In To Save Your Progress

Read Again

Was this article useful?
Yes No
Thank you Glad to hear it