Electronic Design - Set up new design rules for PCB board design

Setting up new design rules for the introduction of PCB design: The PCB editor is a rule-led environment, which means that when users change the design, such as drawing lines, moving components, or automatic routing, Altium Designer will monitor Every action, and check whether the design still fully complies with the design rules. If it does not meet, it will immediately warn, emphasizing that an error has occurred. Setting up design rules before designing allows users to concentrate on designing, because the software will prompt if there is an error.

There are 10 types of design rules, which are further divided into types of design rules. Design rules, including electrical, wiring, process, placement, and signal integrity requirements.

Now let's set up a new design rule, specifying the required width of the power cord. Specific steps are as follows:

1. Activate the PCB file and select Design>>Rules in the menu.

2. The PCB Rule and Constraint Limit Editor dialog box will appear. Each rule class is displayed under the Design Rules folder on the left side of the dialog box. Double-click the Routing extension to see the related wiring rules. Then double-click Width to display the width rules.

3. Click to select each rule. When the user clicks on each rule, the upper part of the right dialog box will display the scope of the rule (the target of the rule that the user wants), and the lower part will display the rule's restrictions. These rules are not only preset values, but also include the information set in the PCB Board Wizard when a new PCB file is created.

4. Click the Width rule to display its scope and constraints. This rule applies to the entire board.

Setting up new design rules for the introduction of PCB design

A powerful feature of Altium Designer's design rule system is that multiple rules can be defined for the same type, and each target has a different object. The exact setting of the target of each rule is determined by the scope of the rule. The rule system uses a pre-defined hierarchy to determine the target of the rule.

For example, a board can first set a width constraint rule, and then set the second width constraint rule for the ground line, and set the third width constraint rule for some lines connected to the ground (independent of the first two rules). The rules are displayed in order of priority.

There is already a width constraint rule that applies to the entire board (width = 12mil). Now a new width constraint rule (width = 25mil) will be added for the 12V and GND network. To add a new width constraint rule, the steps are as follows:

1. Find the Width under the Design Rules folder, right-click and select New Rule to add a new width constraint rule, and only set the 12V network. A new rule named width_1 has appeared. Click on the new rule in the Design Rules folder to modify the range and constraints of the line width.

2. Type 12V or GND in Name. When you click Back, the name will be automatically updated in Design Rules.

3. In the next step, use Query Builder to set the scope of the rule, or you can directly type in the scope at any time. If users feel that Query is more complicated, they can select the Advanced option and click the Query Helper button to use the Query Helper dialog box.

4. Click the Query Builder button to open Building Query in the Board dialog box.

5. Click Add first condition and select Belongs to Net from the drop-down menu. In Condition Value, click and select Network 12V from the list. Query Preview now reads InNet ('12v').

6. Click Add another condition to increase the width of the defined GND. Select Belongs to Net and GND as Condition Value.

7. Click AND and select OR from the drop-down menu. Check the preview shows InNet('12v') OR InNet('GND').

8. Click OK to close Building Query from the Board dialog box.

9. At the bottom of the PCB Rules and in the Constraints Editor dialog box, click the constraint value (10mil) and enter the new value to change the Min Width, Preferred Width and Max Width to 25mil. The new rule has now been set, you can choose to set other rules or save and close the dialog box.

10. Finally, click to edit the original rule named width (the range is set to all), and confirm that Min Width, Preferred Width and Max Width are all set to 12mil. Click OK to close the dialog box. When wiring manually or automatically, all first will be 12mil wide, except for GND and 12V which are 25mil wide.