Violations Associated with Others when Validating a Design in Altium Designer

Default report mode:

Summary

This violation occurs when an Alternate Part – chosen to be used for a component in a defined Variant of the active design project – cannot be added. This happens when a part with the same name, but resides in different libraries, is used across different Variants for the project. The .PrjPcbVariants file, which stores the information for the alternate parts chosen, cannot store multiple parts with the same name, and so references to the other instance(s), resident in different libraries, will not be added. For example, consider the situation where the following variants of a design project have been defined with an Alternate Part chosen for a placed capacitor:

• Variant 1 – Alternate Part Cap chosen, that resides in library Lib1.SchLib.
• Variant 2 – Alternate Part Cap chosen, that resides in library Lib2.SchLib.

Default report mode:

Summary

This violation occurs when there is a floating Parameter Set directive, NoERC directive, Differential Pair directive, or Probe object.

Notification

If a design project is being finalized and contains a floating Parametric Set directive, NoERC directive, Diff Pair directive, or Probe object, this is indicated during project Validation by demonstrating the warning in the Messages panel.

A notification is displayed in the Messages panel in the following format:

Floating <Parameter Set directive, NoERC directive, Differential Pair directive, or Probe object> at <Location>,

where:

• Parameter Set directive, NoERC directive, Differential Pair directive, or Probe object is the floating object located in the design space.
• Location is the X, Y coordinates for the floating object.

Recommendation for Resolution

Attach the floating Parameter Set directive, NoERC directive, Differential Pair directive, or Probe object to their intended location.

Default report mode:

Summary

This violation occurs when a single-part component has been chosen as an Alternate Part for a multi-part component – in a defined Variant for the active design project – and there is more than one part of the original base design component placed within the design. For example, consider a base design with multi-part component R1 – an isolated resistor network with 8 sub-parts. Also consider that four of those parts have been placed (R1A, R1B, R1C, R1D). Now, consider a defined variant of that base design, where an alternate part has been chosen to be used in place of that original base part. The chosen part should also be a multi-part component that can easily accommodate switching out the four sub-parts currently used in the design. However, if by mistake, a single-part resistor component is chosen as the alternate, it does not have the capacity to facilitate the switching-out of existing sub-parts R1B, R1C, and R1D. The Compiler, therefore, flags this as an incorrect link.

Notification

If validation errors and warnings are enabled for display on the schematic (enabled on the Schematic – Compiler page of the Preferences dialog), an offending object will display a colored squiggle beneath it. Hovering over the object will display a pop-up hint that summarizes the violation. A notification is also displayed in the Messages panel in the following format:

Incorrect link between project variant "<VariantName>" and schematic component Component <ComponentPhysicalDesignator> (<ComponentLogicalDesignator>) <BasePartComment>

where:

• VariantName is the name of the design variant in which the erroneous alternate component has been defined.
• ComponentPhysicalDesignator is the physical designator for the affected component (the designator as displayed on the compiled tab view of the relevant schematic document on which the component in question resides).
• ComponentLogicalDesignator is the logical designator for the affected component (the designator as displayed on the Editor tab view of the relevant schematic document on which the component in question resides). If the logical and physical designators are identical, this entry will not be displayed.
• BasePartComment is the value for the Comment parameter for the affected component as defined in the base design.

Recommendation for Resolution

Use the Details region of the Messages panel to cross probe to the component in question. If only one part of the original multi-part component is being used, then you can simply delete any other placed instances and validate the project again. Since the alternate part is a single-part component, it is sufficient for replacement for the single used part of the original multi-part component.

However, this approach, while effective, is not entirely desirable. It is more like a band-aid rather than resolving the underlying issue. A far better approach is to choose a better alternate part for the component in the relevant design variant. To do this:

1. Make the relevant variant the current variant from the Variants folder for the parent project in the Projects panel. Switch to the Compiled tab for the document, right-click on a part of the base multi-part component, then choose Part Actions » Variants. This opens the Variant Management dialog with only the offending component in only that chosen variant presented.
2. Use the Component Variation field to open the Edit Component Variation dialog.
3. With the Alternate Part option still selected, use the other options in the dialog to browse to and choose a more suitable replacement component to be used in that specific variant of the design.
4. Click OK to close the dialogs and validate the design project again. The incorrect link violation should have been resolved and no longer appear (unless, of course, there are multiple components with this issue, in which case repeat the previous steps).

Note

Use the controls associated with the Object Hints entry in the Connectivity Insight Options region (the System – Design Insight page of the Preferences dialog) to determine the launch style for object hints (Mouse Hover and/or Alt+Double Click).

Default report mode:

Summary

This violation occurs when a design object resides beyond the extents of the schematic sheet.

Notification

If validation errors and warnings are enabled for display on the schematic (enabled on the Schematic – Compiler page of the Preferences dialog), an offending object will display a colored squiggle beneath it. Hovering over the object will display a pop-up hint that summarizes the violation. A notification is also displayed in the Messages panel in the following format:

Off sheet <ObjectIdentifier> at <Location>

where:

• ObjectIdentifier identifies the specific object that currently does not reside completely within the boundary defined by the sheet. The identifier is composed of the object's type and its name/designator (e.g., Port <PortName>).
• Location is the X, Y coordinates for the object's electrical hotspot.

Recommendation for Resolution

When placing or pasting objects onto a sheet, you are prevented from placing/pasting beyond the extents of the sheet's border. This issue typically arises when the size and orientation of the sheet are changed after object placement. Consider the following to resolve the problem:

• Change the sheet orientation.
• Choose a larger sheet size.
• Move the offending objects back within the sheet boundary.

The first two options are carried out from the Page Options section on the General tab of the Properties panel (accessed when no objects are currently selected in the design space). Changing sheet size is the simplest way to resolve the issue. Moving objects manually may require layout changes to the circuit to provide enough space to accommodate the offending objects.

Note

Use the controls associated with the Object Hints entry in the Connectivity Insight Options region (the System – Design Insight page of the Preferences dialog) to determine the launch style for object hints (Mouse Hover and/or Alt+Double Click).

Default report mode:

Summary

This violation occurs when an object is not aligned to the current Snap grid.

Notification

If validation errors and warnings are enabled for display on the schematic (enabled on the Schematic – Compiler page of the Preferences dialog), an offending object will display a colored squiggle beneath it. Hovering over the object will display a pop-up hint that summarizes the violation. A notification is also displayed in the Messages panel in the following format:

Off grid <ObjectIdentifier> at <Location>

where:

• ObjectIdentifier identifies the specific object that is currently off-grid. The identifier is composed of the object's type and its name/designator (e.g., Pin <PinDesignator>).
• Location is the X, Y coordinates for the object's electrical hotspot.

Recommendation for Resolution

Ensure that the Snap grid is defined as required and enabled in the General section on the General tab of the Properties panel (accessed when no objects are currently selected in the design space). The offending object can be moved back onto the grid manually or by using the Align To Grid command.

Note

Use the controls associated with the Object Hints entry in the Connectivity Insight Options region (the System – Design Insight page of the Preferences dialog) to determine the launch style for object hints (Mouse Hover and/or Alt+Double Click).

Default report mode:

Summary

This violation occurs when, for a given variant of a multi-channel design, different Alternate Parts have been used for a component across channels.

Notification

If validation errors and warnings are enabled for display on the schematic (enabled on the Schematic – Compiler page of the Preferences dialog), an offending object will display a colored squiggle beneath it. Hovering over the object will display a pop-up hint that summarizes the violation. A notification is also displayed in the Messages panel in the following format:

There are alternate items for multi-channel item "Component <ComponentLogicalDesignator> <ComponentName>" in variant "<VariantName>". Please, check your variant configuration. Alternate parts aren't fully supported in multi-channel designs and can lead to inconsistent data

where:

• ComponentLogicalDesignator is the logical designator for the affected component (the designator as displayed on the Editor tab view of the relevant schematic document on which the component in question resides).
• ComponentName is the name of the component in violation.
• VariantName is the name of the design variant for which Alternate Part choices have been chosen across channels for the component in violation.

Recommendation for Resolution

Use the Details region of the Messages panel to cross-probe to the component in question. To resolve this type of violation, either choose the same Alternate Part for all affected channels or set the component to Fitted or Not Fitted for a channel so that there are no longer different Alternate Parts in use. To do so:

1. Make the relevant variant the current variant from the Variants folder for the parent project in the Projects panel. From the Editor tab for the document, right-click on the part in violation and choose Part Actions » Variants. This opens the Variant Management dialog with only the offending component presented (across all channels).
2. For each offending channel, use the Component Variation field to access the Edit Component Variation dialog.
3. With the Alternate Part option still selected, use the other options in the dialog to browse to and choose the same (required) part already used in another channel. Alternatively, choose to make the component Fitted or Not Fitted for that particular channel.
4. OK out of the dialogs and validate the design project again. The violation should now have been resolved and no longer appear (unless there are multiple components with this issue, in which case, repeat the previous steps).

Note

Use the controls associated with the Object Hints entry in the Connectivity Insight Options region (the System – Design Insight page of the Preferences dialog) to determine the launch style for object hints (Mouse Hover and/or Alt+Double Click).