SOLIDWORKS Assembly Validation Tools – Part 2 – Interference Detection

Interference Detection identifies interferences between components, and helps you to examine and evaluate those interferences. Interference Detection is useful in complex assemblies, where it can be difficult to visually determine whether components interfere with each other.

With Interference Detection, you can:

  • Determine the interference between components.
  • Display the true volume of interference as a shaded volume.
  • Change the display settings of the interfering and non-interfering components to see the interference better.
  • Select to ignore interferences that you want to exclude, such as press fits, interferences of threaded fasteners, and so on.
  • Choose to include interferences between bodies within a multibody part.
  • Choose to treat a subassembly as a single component, so that interferences between the subassembly's components are not reported.
  • Distinguish between coincidence interferences and standard interferences.

To check for interferences in an assembly:

  1. Click Interference Detection (Assembly toolbar), (Evaluate toolbar) or Tools > Interference Detection.


  2. In the PropertyManager:
    1. Make selections and set options.
    2. Under Selected Components, click Calculate.


    The detected interferences are listed under Results. The volume of each interference appears to the right of each listing. Under Results, you can:


  • Select an interference to highlight it in red in the graphics area.
  • Expand interferences to display the names of the interfering components.
  • Right-click an interference and select Zoom to selection, to zoom to the interfering components in the graphics area.
  • Right-click an interference and select Ignore.
  • Right-click an ignored interference and select Un-Ignore

Excluding Hidden Bodies and Components

You can exclude interferences involving hidden bodies and hidden components from Interference Detection results.

Excluding Selected Components

You can exclude selected components from Interference Detection results. Optionally, you can specify to remember components to exclude from session to session. SolidWorks


  • Treat coincidence as interference Reports coincident entities as interferences.
  • Show ignored interferences Select to show ignored interferences in the Results list, with a gray icon. When this option is cleared, ignored interferences are not listed.
  • Treat subassemblies as components When selected, subassemblies are treated as single components, so interferences between a subassembly's components are not reported.
  • Include multibody part interferences Select to report interferences between bodies within multibody parts.
  • Make interfering parts transparent Select to display the components of the selected interference in transparent mode.
  • Create fasteners folder Under Results, segregates interferences between fasteners (such as a nut and bolt) into a separate folder named Fasteners. See Interference Detection with Fasteners.
  • Create matching cosmetic threads folder Under Results, segregates interferences between components with properly matched cosmetic threads into a separate folder named Matching cosmetic threads. Interferences due to mismatched threads, misaligned threads, or other interfering geometry are still listed as interferences.
  • Ignore hidden bodies/components Excludes the following from the results:
    • Interferences involving components that are hidden, including those hidden by the Isolate command.
    • Interferences between a multibody part's hidden bodies and other components.


Non-interfering Components

Displays non-interfering components in the selected mode:

Use current Uses the current display settings of the assembly.


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When you run Interference Detection, the interferences between the threads of fasteners are reported. Generally, you want to ignore these interferences.

You can create a Matching cosmetic threads folder to segregate interferences between components with properly matched cosmetic threads. You can create a Fasteners folder to segregate all interferences involving fasteners.

A custom property named IsFastener, with its value set to 1, designates a part as a fastener for interference detection.


To designate a part as a fastener for interference detection:

  1. In the part document, click File > Properties, and select the Custom tab.
  2. In the first blank cell under Property Name, choose IsFastener from the list.
  3. Select Number in Type.
  4. Under Value / Text Expression, type 1.
  5. Press Tab or Enter.

    The value 1 appears under Evaluated Value.

  6. Click OK.

    The part now has a custom property IsFastener with a value of 1. Now when you run Interference Detection (with Create fasteners folder selected), if the part is involved in an interference, the interference appears in the Fasteners folder.

    By default, fasteners provided with the SOLIDWORKS Toolbox add-in are designated as fasteners for interference detection (they have an internal IsFastener flag set in the file by default a special tool is required to add/remove this type of flag from a component. This also shows the part as a fastener in the component tree).

We hope this has given you a better understanding of the capability available in the Interference Detection command.  Please check back for the rest of the series as we continue to take a deep dive into the SOLIDWORKS assembly validation tools that are available and how they work.  Please check back to the CATI Blog as the Dedicated Support Team will continue posting new series of articles every month that go further into the details of many of the SOLIDWORKS tools. All of these articles will be stored in the category of Daily Dose…..of SOLIDWORKS Support and links to each article with their release date are listed below:



John Van Engen
Senior Technical Analyst
CATI Technical Support

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