Tutorial - Verifying Your Board Design in Altium NEXUS

Parent page: Tutorial - A Complete Design Walkthrough with Altium NEXUS

Main pages: PCB Design Rules Reference, Design Rule Checking (DRC)

The PCB editor is a rules-driven design environment in which you can define many types of design rules that can be checked to ensure the integrity of your board. Typically you set up the design rules at the start of the design process. The online DRC feature monitors the enabled rules as you work and immediately highlights any detected design violations. Alternatively, you can also run a batch DRC to test that the design complies with the rules and generate a report that details the enabled rules and any detected violations.

Earlier in the tutorial, you examined the routing design rules, adding a new width constraint rule targeting the power nets, as well as an electrical clearance constraint and a routing via style rule. As well as these, there are a number of other design rules that are automatically defined when a new board is created.

Configuring the Display of Rule Violations

Preferences page: PCB Editor – DRC Violations Display

Before checking for rule violations, it is important to understand how violations are displayed.

Altium NEXUS has two techniques for displaying design rule violations, each with its own advantages. These are configured on the PCB Editor – DRC Violations Display page of the Preferences dialog:

• Violation Overlay – violations are identified by the primitive-in-error highlighted in the color chosen for the DRC Error Markers (configured in the View Configuration panel; press L to open). The default behavior is to show the primitives in a solid color when zoomed out, changing to the selected Violation Overlay Style as you zoom in. The default is Style B – a circle with a cross in it.

• Violation Details – as you zoom further in, Violation Detail is added (if enabled), detailing the nature of the error. Violation Detail can include:

  • Information at the site of the violation
  • Where appropriate, an icon to indicate the type of violation, for example, thin lines that cross over, indicating a short circuit.
  • A numerical value showing the rule setting that is failing, for example, <0.25mm.

  
  Violations can be displayed as a colored overlay and also as a detailed message, with different symbols being used to show different detail of the error type.

     
  Violations are shown in solid green (the first image), as you zoom in this changes to the selected Violation Overlay Style (the second image); as you zoom in further Violation Details are added (the third image).

Configuring the Rule Checker

Dialog page: Design Rule Checker

The design is checked for violations by running the Design Rule Checker. Run the Tools » Design Rule Check command to open the dialog. Both online and batch DRC are configured in this dialog.

DRC Report Options

• By default, the dialog opens showing the Report Options page selected in the tree on the left of the dialog (shown below).

• The right side of the dialog displays a list of general reporting options. For more information about the options, press F1 when the cursor is over the dialog. These options can be left at their defaults.

  
  Rule checking, both online and batch, is configured in the Design Rule Checker dialog.

DRC Rules to Check

• The testing of specific rules is configured in the Rules to Check section of the dialog. Select this page in the tree on the left of the dialog to list all of the rule types (shown below). You can also examine them by type, for example, Electrical, by selecting that page on the left of the dialog.
• For most rule types, there are checkboxes for Online (check as you work) and Batch (check this rule when the Run Design Rule Check button is clicked).

• Click to enable/disable the rules as required. Alternatively, right-click to display the context menu. This menu allows you to quickly toggle the Online and Batch settings. Select the Batch DRC - Used On entry, as shown in the image below.

  
  Checking is configured for each rule type. Use the right-click menu to enable the Used design rules.

Running a Design Rule Check (DRC)

Click the Run Design Rule Check button at the bottom of the dialog to perform a design rule check. When the button is clicked, the DRC will run, then:

• The Messages panel will open and list all detected errors.
• If the Create Report File option was enabled in the Report Options page of the dialog, a Design Rule Verification Report will open in a separate document tab. The report for the tutorial is shown below.
  • The upper section of the report details the rules that are enabled for checking and the number of detected violations. Click on a rule to jump to and examine those errors.
  • Below the summary of violating rules are specific details about each violation.
  • The links in the report are live. Click on a specific error to jump back to the board and examine that error on the board. Note that the zoom level for this click action is configured on the System – Navigation page of the Preferences dialog. Experiment to find a zoom level that suits you.

The upper section in the report details the rules that are enabled for checking and the number of detected violations. Click on a rule to jump to and examine those errors.

The lower section of the report shows each rule that is being violated, followed by a list of the objects in error. Click on an error to jump to that object on the PCB.

Locating the Error Condition

When you are new to the software, a long list of violations can initially seem overwhelming. A good approach to managing this is to disable and enable rules in the Design Rule Check dialog at different stages of the design process. It is not advisable to disable the design rules themselves if there are violations, just the checking of them. For example, you would always disable the Un-Routed Net check until the board is fully routed.

• When a batch DRC is run on the tutorial board, there are:
  • 4 Minimum Solder Mask Sliver violations – the minimum width of a strip of solder mask is less than allowed by this rule. This typically occurs between component pads.
  • 4 Clearance Constraint violations – the measured electrical clearance value between objects on signal layers is less than the minimum amount specified by this rule.
• To locate a violation:
  • Click the link in the report file, or
  • Double-click in the Messages panel,
  • Click on a violation in the PCB Rules And Violations panel.
• Using the Violation Details, you can establish the error condition.

• The image below shows the Violation Details for one of the clearance constraint errors, indicated by the white arrows and the 0.25mm text, indicating that this gap is less than the minimum 0.25mm allowed by the rule. The next step is to work out what the actual value is so you know how much it has failed. You can then decide how to resolve this error.

  
  The Violation Details show that the clearance between these two pads is less than 0.25mm; it does not detail the actual clearance.

Understanding the Error Condition

So you've found an error. How do you know how much it has failed? As the designer, you need this essential information to be able to decide how best to resolve the error.

For example, if the rule says the allowable minimum solder mask sliver is 0.25 mm and the actual sliver is 0.24 mm, then the situation is not that bad and you may be able to adjust the rule setting to accept this value. But if the actual sliver value is 0.02, then that is probably not a situation that can be resolved by adjusting the rule setting.

Apart from actually measuring the distance, there are a number of approaches to finding out how much a rule has failed by. You can use:

• The right-click Violations submenu, or
• The PCB Rules And Violations panel, or
• The detail included in the Messages panel; the actual value is detailed along with the specified value (for example, 0.175 mm < 0.254 mm).

The Violations Submenu

The right-click Violations submenu was described earlier in the Existing Design Rule Violation section.

The image below shows how the Violations submenu details the measured condition against the value specified by the rule.

Right-click on a violation to examine what rule is being violated and the violation conditions.

The PCB Rules And Violations Panel

Panel page: PCB Rules And Violations

The PCB Rules And Violations panel is an excellent feature for locating and understanding error conditions.

• Click the button then select PCB Rules And Violations from the menu to display the panel. It will default to show [All Rules] in the Rule Classes list. Once you have identified a rule type of interest, select that specific rule class so that only those violations are shown at the bottom of the panel.

• Click once on a violation in the list to jump to that violation on the board; double-click on a violation to open the Violation Details dialog.

  
  The panel details the violation type, the measured value, the rule setting, and the objects that are in violation.

Resolving the Violations

As the designer, you have to work out the most appropriate way of resolving each design rule violation. Let's start with the solder mask errors as they are related, and both error conditions may be affected by the changes you make to solder mask settings.

Minimum Solder Mask Sliver Violations

Design rule reference: Minimum Solder Mask Sliver

The solder mask is a thin, lacquer-like layer applied to the outer surface of the board, providing a protective and insulating covering for the copper. Openings are created in the mask for components and wires to be soldered to the copper. It is these openings that are displayed as objects on the solder mask layer in the PCB editor (note that the solder mask layer is defined in the negative – the objects you see become holes in the actual solder mask).

During fabrication, solder mask is applied using different techniques. The lowest cost approach is to silkscreen it onto the board surface through a mask. To allow for layer alignment issues, the mask openings are typically larger than the pads, reflected by the 4mil (~0.1mm) expansion value used in the default design rule.

There are other techniques for applying solder mask, which offer higher-quality layer registration and more accurate shape definition. If these techniques are used, the solder mask expansion can be smaller or even zero. Reducing the mask opening reduces the chance of having solder mask slivers or silk to solder mask clearance errors.

A solder mask sliver error. The purple represents the solder mask expansion around each pad.

Errors such as these solder mask issues cannot be resolved without consideration of the fabrication technique that will be used to make the finished board.

For example, if this was a complex, multi-layer board for a high-value product, then it is likely that a high-quality solder mask technology would be employed, which would allow a small or zero solder mask expansion. However, a simple, double-sided board like the board in this tutorial is more likely to be fabricated as a low-cost product, requiring a low-cost solder mask technology to be used. That means resolving the solder mask sliver errors by reducing the solder mask expansion for the entire board is not an appropriate solution.

Like many aspects of PCB design, the solution lies in making thoughtful trade-offs in a focused way to minimize their impact.

Clearance Violations

Design rule reference: Clearance Constraint

There are two ways of resolving this clearance constraint:

• Decrease the size of the transistor footprint pads to increase the clearance between the pads, or
• Configure the rules to allow a smaller clearance between the transistor footprint pads.

Since the 0.25mm clearance is quite generous and the actual clearance is quite close to this value (0.22mm), a good choice in this situation would be to configure the rules to allow a smaller clearance. This can be done in the existing Clearance Constraint design rule, as shown below.

• The TH Pad – to – TH Pad value is changed to 0.22mm in the grid region of the rule constraint. To edit a cell, select first it then press F2.

• This solution is acceptable in this situation because the only other component with thruhole pads is the connector, which has pads spaced over 1mm apart. If this was not the case, the best solution would be to add a second clearance constraint targeting just the transistor pads, as was done for the solder mask expansion rules.

  
  Edit the Clearance Constraint to allow a TH Pad to TH Pad clearance of 0.22mm.

• Click OK to accept the changes and close the PCB Rules and Constraints Editor dialog.

Silk to Silk Clearance Violation

Design rule reference: Silk to Silk Clearance

The last error to resolve is the silk to silk clearance violations. These are usually caused by a designator being too close to the outline of an adjacent component. Your design may not have any of these violations – it depends on how close you placed the components, or if you have already repositioned the designators. Click, hold and drag a designator to move it – all objects will dim apart from the objects in the component whose designator is being moved; move that designator to a new location.

Designator movement will be constrained by the current snap grid. If it is currently too coarse, press Ctrl+G and enter a new grid value.

Reposition any designator that is causing a silk to silk violation.