Altium Designer Documentation

Violations Associated with Components – Нарушения, связанные с компонентами_AD

Created: 06.06.2015 | Updated: 08.10.2021

Parent page: Verifying Your Design Project

The Violations Associated with Components region on the Error Reporting tab of the Project Options dialog
The Violations Associated with Components region on the Error Reporting tab of the Project Options dialog

Logical, electrical, and drafting awareness in your schematic diagram can be verified during design project verification according to rules defined as part of the options for the design project – on the Error Reporting and Connection Matrix tabs of the Project Options dialog.

For a detailed overview of verifying your captured design, see Verifying Your Design Project.

The Violations Associated with Components region on the Error Reporting tab of the Project Options dialog allows specifying the severity level associated with check of component-related violations that can exist in source documents when validating a project. Use the following collapsible sections to access information on each violation available in this region.

Default report mode:

Summary

This violation occurs when at least one component has been deleted from a project design. Operating as a 'soft delete', deleted components are moved to a dedicated Trash location where they can be retrieved (Restore) or completely removed (Permanently Delete) from a deleted entry's menu options () in the browser interface of the connected Workspace.

Notification

Where a design project is using a component that has been deleted, 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:

ComponentName: Component has been deleted

where:

  • ComponentName is the name of the Workspace component.
Deleted components will also be marked in component access locations such as the Properties panel and the project's Item Manager.

Recommendation for Resolution

If the component was deleted by mistake, it can be restored by someone with appropriate access rights from the Trash page of the Workspace's browser interface. Otherwise, replace the component used in the design with another equivalent component that is available in the connected Workspace.

Default report mode:

Summary

This violation occurs when compiling an Integrated Library Package (*.LibPkg) and the pin mapping between the schematic component and the linked model is found to be invalid.

Notification

If 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:

ComponentName: Could not find port <ModelPinNumber> on model <ModelName> for pin <ComponentPinNumber> – PCB model related

ComponentName: Could not map port <ModelPinNumber> on model <ModelName> to a pin – simulation model related

where:

  • ComponentName is the name of the component in the source schematic library.
  • ModelPinNumber is the expected designator for the pin/pad that could not be found on the linked model.
  • ModelName is the name of the model that is linked to the component.
  • ComponentPinNumber is the designator of the pin on the source schematic component to which the erroneous pin of the model is mapped.

Recommendation for Resolution

Resolution involves accessing the mapping between the schematic symbol and the target domain model. To do this, you'll first need to be viewing the properties for the applicable schematic library component. Double-click on the entry for the component in the Components list of the SCH Library panel to access the Properties panel, with the properties for that component loaded.

If the PCB model related violation message is displayed, select the model in the Footprint section of the panel and click the button underneath the list to access the PCB Model dialog. Once there, click on the Pin Map button to access the Model Map dialog. In the Component Pin Designator column, find the pin number flagged by the message (ComponentPinNumber). The violation arises because the corresponding entry in the Model Pin Designator column points to a pad designator that does not exist in the PCB model. Amend the entry as required. Typically there will be a one-to-one mapping, with the designators on both sides the same.

If the simulation model related message is displayed, select the model in the Models section of the panel and click the button underneath the list to access the Sim Model dialog. Once there, click on the Port Map tab. This violation will arise when the model pin is not correctly mapped to a pin of the schematic component. This can happen when the entry for the model pin has been set to a pin that is already mapped, or to Not Connected. Amend the entry as required.

Tip

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 at least one placed instance of a Component Item Revision – placed from a connected Workspace – is detected to be in an inapplicable state. For example, the component is currently Depracated or Obsolete and should therefore have no place on the latest design spin. Applicability is determined through the Allowed to be used in designs option in the State Properties dialog. From within the Edit Lifecycle Definitions dialog, access this dialog for the required state, either by double-clicking on the state's entry within the parent lifecycle definition or by selecting its entry and clicking the edit icon that appears (). When this option is enabled, an Item Revision in this state is permitted to be used in a design. It is deemed to be Applicable. If this option is disabled, an Item Revision in this state cannot be validly used and is deemed Inapplicable (or non-applicable).

The Edit Lifecycle Definitions dialog is itself accessed from the Data Management – Servers page of the Preferences dialog, by clicking the Properties button for the Workspace to which you are actively signed in, then selecting Lifecycles from the drop-down menu.
When connected to an Altium 365 Workspace, note that configuration and use of lifecycle definitions is not supported with the Standard Subscription Plan. As such, this violation check will not be available with this level of access to Altium 365.

Notification

If 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:

Component <Designator> <Comment>: Component revision has inapplicable state

where:

  • Designator is the component instance's Designator.
  • Comment is the component instance's Comment.

Recommendation for Resolution

Use the Item Manager dialog to choose a replacement Component Item Revision that is valid for use in the design. Do this for each component that is in an inapplicable state. Alternatively, you can switch out an existing Component Item Revision for a different revision, or revision of a different Component Item at the individual component level. Select the component on the schematic to access its properties through the Properties panel. In the Properties section of the panel, either click the Update button to use the latest revision of the current Component Item, or click the button at the right of the Design Item ID field to access your Workspace, and browse for another Component Item Revision to use.

Use controls available through the Properties panel or Item Manager dialog to choose a later revision of the Item that is in an applicable state or, if this is not possible (the Item, in general, is not for design use), choose an applicable revision of a different Item.

Tips

  • 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).
  • If a placed component loses connection with its source Workspace – for example, the Workspace from which it was placed is disconnected or you are signed out from your Workspace – it will violate the Component revision has inapplicable state check. This will be reflected in the Messages panel with an entry in the form: Component <Designator> <Comment>: Can't perform revision status validation: Failed to get session: Access denied! User login required for this service.
  • You can also catch components that are being invalidly used within a design during the design release process. Add and configure Component State Checking to your overall release validation regemin.

Default report mode:

Summary

This violation occurs when a component – placed from a connected Workspace – is detected to be out of date.

Notification

If 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:

Component <Designator> at <Location>: Component revision is Out of Date

where:

  • Designator is the component instance's Designator.
  • Location is the X, Y coordinates marking the origin of the offending component instance.

Recommendation for Resolution

Use the Item Manager dialog to identify and update components that are not the latest revision. The Item Manager includes a Revision Status column, for any components that are not at the latest revision the component's status will be Out of Date. Select the out-of-date component(s), right-click and choose Update to latest revision from the menu. Once this has been done, Generate an ECO to apply these changes to the affected schematics.

Alternatively, you can switch out an existing Component Item Revision for the latest revision, at the individual component level. Simply select the component on the schematic to access its properties through the Properties panel. In the Properties section of the panel, click the Update button to use the latest revision of the current Component Item.

Tips

  • 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).
  • If a placed component loses connection with its source Workspace – for example the Workspace from which it was placed is disconnected or you are signed out from your Workspace – it will violate the Component revision is Out of Date check. This will be reflected in the Messages panel, with an entry in the form: Component <Designator> <Comment>: Can't perform revision status validation: Failed to get session: Access denied! User login required for this service.

Default report mode:

Summary

This violation occurs when the same part of a multi-part component instance has been placed more than once in a schematic design. For example, you have placed a 74HC32 component with designator U9, but have inadvertently placed two instances of part one of this component, resulting in two instances of U9A in the design.

Notification

If 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:

Component <ComponentName> has duplicate sub-parts at <Location1> and <Location2>

where:

  • ComponentName is the name of the offending component in terms of its designator and library reference.
  • Location1 is the X, Y coordinates for the first instance of the particular sub-part.
  • Location2 is the X, Y coordinates for the duplicate instance of the particular sub-part.

Recommendation for Resolution

Change the part number for the offending parts as required, using the Increment Part Number command – available from the main Edit menu or from the Part Actions sub-menu (when right-clicking over the part). The advantage of launching the command from the Edit menu is that you remain in increment mode, allowing you to cycle through the part numbers until you reach the desired one.

Tip

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 two or more pins in a component have the same designator.

Notification

If 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:

Duplicate pins in component Pin <Identifier1> and Pin <Identifier2>

where:

  • Identifier1 is the identifier for the first instance of the duplicated pin, represented by the part designator-pin designator pairing
  • Identifier2 is the identifier for the second instance of the duplicated pin, represented by the part designator-pin designator pairing.

Recommendation for Resolution

Change the designator of the offending pin(s) accordingly, so that each has a unique assignment. Pin designators can be edited from within the Schematic Editor for a component that has already been placed:

  • If the component pins are not locked, you can simply select the pin and edit its designator through the Properties panel.
  • Otherwise, edit the pin(s) using the Component Pin Editor dialog. With the component selected in the design space, access to this dialog is made from the Properties panel by clicking the  button, below the Pins section, on the Pins tab of the panel.

Typically, the duplication will reside in the library component, in which case you should edit the pin designator for that component in the source schematic library and then pass the change on to placed instances of the component, using the Update From Libraries (Schematic Editor) or Update Schematics (Schematic Library Editor) commands. Both commands are available from the main Tools menus of these editors respectively.

Tips

  • 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).
  • Only one violation instance will be listed in the Messages panel for each distinct component. A component may well have more than two pins with the same designator, but when investigating the violation using the Details region of the panel, only the first two duplicate pins (in alphabetical pin name order) will be listed.

Default report mode:

Summary

This violation occurs when at least two parts across source schematic sheets in a design have the same designator associated with them.

Notification

If 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:

Duplicate Component Designators <PartDesignator>

where:

  • PartDesignator is the offending designator.

Recommendation for Resolution

Assign different and unique designators to the duplicates as required. This can be done manually by editing each offending designator or through the use of the Annotate dialog (Tools » Annotation » Annotate Schematics).

Alternatively, reset the duplicate component designators first using the Tools » Annotation » Reset Duplicate Schematic Designators command then use the Tools » Annotation » Annotate Schematics Quietly command to annotate without launching the Annotate dialog.

Tip

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 if an extra pin has been detected in one of the display modes for a part.

Notification

If 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:

Extra Pin <Identifier> in <DisplayMode> of part <PartName>

where:

  • Identifier is used to identify the pin in question. When compiling a schematic library document, the identifier appears in the format PhysicalComponentName-PinDesignator (e.g., DIP14-15). When compiling the source schematic or project, the identifier appears in the format PartDesignator-PinDesignator (Inferred) (e.g., X1-1 (Inferred)).
  • DisplayMode is the specific graphical representation mode for the part in which the extra pin has been found. A part has a Normal mode and can have up to 255 defined Alternate modes.
  • PartName is either the physical component name or the designator for the affected part, depending on whether you are compiling the schematic library document or source schematic sheet/project respectively.

Recommendation for Resolution

This violation typically arises when an alternate graphical mode is defined for a component and either:

  • An extra pin has been added to the display that is not specified in the Normal display mode, or
  • A pin has been specified with a different Designator and/or Name to a pin specified in the Normal display mode.

Not only must there be an identical number of pins between graphical display modes, but the pins must be also identical in both Designator and Name.

In the source schematic library, display the offending display mode for the component and delete the extra pin. This can be performed directly on the schematic sheet for a part that has been placed already, however, you would typically tackle the problem from within the library, then push the change across (Tools » Update Schematics).

Tip

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 Generic Component has been included in a final design. Generic Components can quickly be placed in a design without the need to find and choose a specific manufacturer part from the available component sources and are intended as placeholders that are easily replaced by a suitable component.

The Generic Components feature is currently in closed Beta.
When connected to an Altium 365 Workspace, note that the Generic Components feature is not supported with the Standard Subscription Plan. As such, this functionality will not be available with this level of access to Altium 365.

Notification

If a design project is being finalized and contains a Generic Component, 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:

Generic Component <PartDesignator> is placed at <Location>

where:

  • Designator is the placed generic component instance's Designator.
  • Location is the X, Y coordinates marking the origin of the offending generic component instance.

Recommendation for Resolution

When a design has progressed to the point where a Generic Component can be replaced with a specific physical component, you may use the Replace Component dialog by selecting the ellipsis menu in the Design Item ID field of the Properties panel. Note this also can be done from the Item Manager or through the project's ActiveBOM document.

Tip

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 in multi-part components when a hidden pin common to more than one sub-part is connected to different nets.

Notification

If 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:

Mismatched hidden pin connections in Pin <Identifier> and Pin <Identifier>

where:

  • Identifier is used to identify the pin in question. The identifier appears in the format PhysicalComponentName-PinDesignator (e.g., U2-7).

Recommendation for Resolution

Reassign the offending pin(s) to the correct nets. A hidden pin is assigned to a net by entering the net name into the Hidden Net Name field in the SCHLIB List panel or the SCH List panel when the panel is displaying pin properties. If this is being done in the SCH List panel, right-click in the panel and enable the Show Children option to list the pins in the panel.

Tip

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 is related to the power pins (VCC and GND) of a multi-part component. Typically, these pins are associated with part 0, are automatically connected to the VCC and GND nets for the design, and are hidden. If for one of the component parts, you enable visibility of such a pin, it is no longer connected to the target power net and the error will be flagged.

Notification

If 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:

Pin is visible in one sub-part and hidden in another sub-part

Recommendation for Resolution

Either disable the display of the offending power pin(s) in the design space or, if keeping the pins displayed, ensure that a VCC and/or GND power port object is attached to the pin(s) accordingly.

Tip

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 compiling an Integrated Library Package (*.LibPkg) and a linked model for a component in the source schematic library could not be found.

Notification

If 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. When the linked model is a footprint model or simulation model, the message notification is also displayed in the Messages panel in one of the following formats:

<ComponentName>: Could not find <ModelName> – when the model search scope is Any.

<ComponentName>: Could not find <ModelName> in <LibraryName> – when the model search scope is Library Name.

<ComponentName>: Could not find <ModelName> in <Path> – when the model search scope is Library Path.

where:

  • ComponentName is the name of the component in the source schematic library.
  • ModelName is the name of the footprint, or simulation model, that is linked to the source component and which could not be found.
  • LibraryName is the name of the library file specified to contain the linked model.
  • Path is the absolute path to a library file specified to contain the linked model.

When the linked model is a signal integrity model, the message is displayed in the Messages panel in the following format:

<ComponentName>: Could not find 'GenericEntity' in <Path>

where:

  • ComponentName is the name of the component in the source schematic library.
  • Path is the absolute path to a library/model.

Recommendation for Resolution

When the problem is a linked footprint or simulation model

This issue is typically caused by one of the following scenarios:

  • The model name is incorrectly specified when defining the model link.
  • The linked model does not reside in the specified library file.
  • The library file containing the linked model has been moved or deleted.

The first port of call in resolving this violation is the associated setup dialog for the model type you are linking to – the PCB Model dialog, or the Sim Model dialog. In each case, check and ensure:

  • The name of the model to which you are linking is correct, and
  • The correct option is used to locate the library/model file in which that model resides.

The format of the displayed error message depends on the search scope you have enabled when locating the model, and can be of great help when tracking down the problem with the model link:

  • If the model could not be found in a specified path (search scope: Library path), ensure that the library/model file you have specified actually exists at that location and also check the library/model file to see if the model with the specified name exists within.
  • If the model could not be found in a specified library/model file (search scope: Library name), ensure that the library/model file has been added to the Available Libraries list (Project Libraries, Installed Libraries, Project Search Paths). Also, check to make sure the library/model file contains the model with the same name specified in the link.
  • If the model could simply not be found (search scope: Any), ensure that a library/model file – containing a model with the same name as that specified in the link – has been added to the Available Libraries list.

When the problem is a linked signal integrity model

Typically caused when the type of signal integrity model (e.g., diode, IC) is not specified, this is resolved in the associated setup dialog for signal integrity models. The easiest way to access this is through the Properties panel when viewing the properties for the selected component. Check that you are using the correct model in the Models section on the General tab of the panel and amend if necessary. The Add and  buttons can be used to create a new model (choose Signal Integrity from the list) or modify the existing signal integrity model. This will give access to the Signal Integrity Model dialog, where the Import Ibis button allows pins models to be imported from an Ibis model file.

You can add an Ibis model directly by clicking Add » Ibis model and using the subsequent Ibis Model dialog to define the link to the model and file.

Tip

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 if there is a different number of pins between graphical display modes for a part.

Notification

If 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:

Missing Pin <Identifier> in <DisplayMode> of part <PartName>

where:

  • Identifier is used to identify the pin in question. The identifier appears in the format PartLibraryReference-Pin Designator (e.g., DIP14-8).
  • DisplayMode is the specific graphical representation mode for the part in which the missing pin has been found. A part has a Normal mode and can have up to 255 defined Alternate modes.
  • PartName is the library reference for the affected part.

Recommendation for Resolution

This violation typically arises when an alternate graphical mode is defined for a component, but not all pins specified in the Normal mode have been specified for the Alternate (i.e. there must be an identical number of pins between graphical display modes).

In the source schematic library, copy the missing pins from an existing display mode into the offending display mode for the component. This can be performed directly on the schematic sheet for a part that has been placed already, but you would typically tackle the problem from within the library, then push the change across (Tools » Update Schematics).

Tip

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 sheet symbol contains two sheet entries possessing the same name.

Notification

If 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:

Sheet Symbol with duplicate entries Sheet Entry <Identifier> at <Location1> and <Location2>

where:

  • Identifier is used to represent the offending sheet entry. The identifier appears in the format SheetSymbolName-SheetEntryName(SheetEntryIOType).
  • Location1 is the X, Y coordinates for the first violating sheet entry.
  • Location2 is the X, Y coordinates for the second violating sheet entry.

Recommendation for Resolution

Change the name of the offending sheet entry object as required, either by editing the name in-situ or by double-clicking on the offending sheet entry and editing its Name in the Properties section of the Properties panel – which presents all properties for the selected sheet entry.

A sheet entry name can also be edited from the Sheet Entries section on the General tab of the Properties panel – when browsing the properties for the selected parent sheet symbol.

Tips

  • 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).
  • When you need to allow a specific point in the circuit not to report a violation of this type, you can place a Specific No ERC directive directly at the error location from the Messages panel – you can do this by right-clicking a message reporting the violation to suppress, then choosing the Place Specific No ERC for this violation command.

Default report mode:

Summary

This violation occurs when a component in the design is found to have a default designator (with a ? suffix), i.e. either it has yet to be annotated or the designator has been reset.

Notification

If 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:

Un-Designated Part <PartDesignator>

where

  • PartDesignator is the default designator for the un-designated part (e.g. U?, D?, C?, etc).

Recommendation for Resolution

Assign a unique designator to the offending component as required. This can be done manually by editing the designator or through the use of the Annotate dialog (Tools » Annotation » Annotate Schematics).

Alternatively, use the Tools » Annotation » Annotate Schematics Quietly command to annotate without launching the Annotate dialog.

Tips

  • Only one error instance will be listed in the Messages panel for each distinct designator type (U?, D?, C?, etc.). Multiple errors may exist.
  • 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 part of a multi-part component instance has not been used within the design. For example, three out of four parts for an instance of a 74HC32 component may have been placed and wired but the fourth has not.

Notification

If 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:

Component <Identifier> has unused sub-part(s) (<PartNumber>)

where

  • Identifier is the parent component, represented using the format Designator Library Reference (e.g., U11 74HC32)
  • PartNumber is an integer used to indicate which specific part is not being used (e.g., 1 represents part A, 2 represents part B, and so on).

Recommendation for Resolution

Place the unused part and connect its inputs to the ground. To ensure the same root designator, copy an existing part for that component's instance and, after pasting, increment its part number accordingly.

Tip

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).

Обнаружили проблему в этом документе? Выделите область и нажмите Ctrl+Enter, чтобы оповестить нас.

Связаться с нами

Связаться с нашими Представительствами напрямую

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
200 characters remaining
Вы сообщаете о проблеме, связанной со следующим выделенным текстом
и/или изображением в активном документе: