Altium NEXUS Documentation

Incorrect Link in Project Variant

Modified by Jason Howie on Sep 30, 2019
All Contents

Parent category: Violations Associated with Others

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 compiler 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 recompile the project. 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 recompile the design project. 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).

Tip

  • Object hints will only appear provided the Enable Connectivity Insight option is enabled on the System - Design Insight page of the Preferences dialog. Use the controls associated with the Object Hints entry in the Connectivity Insight Options region of the page to determine the launch style for such hints (Mouse Hover and/or Alt+Double Click). 
Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

You are reporting an issue with the following selected text
and/or image within the active document:
ALTIUM DESIGNER FREE TRIAL
Altium Designer Free Trial
Let’s get started. First off, are you or your organization already using Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

In that case, why do you need an evaluation license?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You actually don’t need an evaluation license for that.

Click the button below to download the latest Altium Designer installer.

Download Altium Designer Installer

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Please fill out the form below to get a quote for a new seat of Altium Designer.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

If you are on Altium Subscription, you don’t need an evaluation license.

If you are not an active Altium Subscription member, please fill out the form below to get your free trial.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Why are you looking to evaluate Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

You came to the right place! Please fill out the form below to get your free trial started.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Great News!

Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

That’s great! Making things is awesome. We have the perfect program for you.

Upverter is a free community-driven platform designed specifically to meet the needs of makers like you.

Click here to give it a try!

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.