Working with imported files in SOLIDWORKS

The amount of technical support questions related to working with imported files in SOLIDWORKS has increased a lot within past years. It is obvious that people are more and more working with different CAD file formats.

SOLIDWORKS has luckily responded to this challenge and developed a feature called "3D Interconnect" that helps with working with files coming from other CAD systems.

Here is some information about working with imported files and "3D Interconnect" feature.

What is 3D Interconnect?

3D Interconnect is a feature that was originally introduced in SOLIDWORKS 2017 but it has been developed all the time and new supported file formats have been implemented constantly. Feature can be used to open files from other CAD systems in their own native file format (Autodesk Inventor, PTC Creo, CATIA, NX etc.). That way file is not imported but just opened in SOLIDWORKS. Created SOLIDWORKS file is also linked to original file and file can be updated if the original CAD file in other file format is changed. User can always break the link between SOLIDWORKS file and original file if needed.

How 3D Interconnect feature is turned on or off?

3D Interconnect feature is turned on by default in SOLIDWORKS.

The setting for 3D Interconnect is this: Tools > Options > Import > "Enable 3D Interconnect".

What are the supported file formats?

3D Interconnect supports multiple file formats. See the table below. Please note that importing CATIA files requires SOLIDWORKS Premium license. Importing CATIA files is not possible with SOLIDWORKS Standard or Professional license.

What's the difference if setting "Enable 3D Interconnect" is on or off?

When setting "Enable 3D Interconnect" is on when opening a file from one of its supported file formats, SOLIDWORKS opens that file in its native file format. So the file is then not imported but just opened. By default, the file is also linked to original file. For example in the picture below you can see that STEP file is opened and it is linked to original STEP file. Feature tree has is showing 3D Interconnect symbol in front of the component name, indicating that the file is linked to original STEP file.

When setting "Enable 3D Interconnect" is off, all files supported by SOLIDWORKS importing (file types that are available in "File > Open" window) are imported by using "traditional" SOLIDWORKS importing procedure. Files are then not linked to original imported file. So for example STEP files are then imported as static imported solid or surface bodies (depending on the import settings and the source data format).

What happens in SOLIDWORKS if original file has been modified?

When file has a link to original file, it is possible to use "Edit feature" (with imported part) or "Edit Part" (when imported into assembly) option to re-import the file. By default, SOLIDWORKS remembers the original file name and the directory where the file was imported from. But it is also possible to select the file to be re-read from another directory. To re-import the file, just press the green checkmark to re-import the model.

When working directly with file types of other CAD software (Creo *.prt files, CATIA *.catpart/*.catproduct files etc.) it is also possible to use "Update Model" function, according to picture seen below. In the picture it is also seen that there is a tiny "refresh icon" seen on top of the import feature. When working with updates of the file, it has to be remembered that "Update Model" command requires that the original filename has not been changed and the file is in the same folder as when the file has been imported. "Update Model" command is not visible for neutral file types such as *.STP, *.IGES, *.SAT etc. When working with these file types, it is always needed to use "Edit feature" (part) and "Edit part" (assembly) commands.

How can you break the link between SOLIDWORKS file and the original file (*.STP file for example)?

The link between SOLIDWORKS file and the original file is broken by selecting the option "Break Link" according to picture below.  Note: This option was called "Dissolve feature" in SOLIDWORKS 2020 and previous versions. After breaking the link, file is treated as static imported file that has no relation to original CAD file.

SOLIDWORKS 2021 SP1.0 version also brought some additional options that gives user more power to decide what to do with imported parts and assemblies. These settings below don't have any effect on importing part files:

"Create 3D Interconnect feature in parts only" - When setting is enabled, imported assemblies are always imported with broken link to original file. Imported parts will be imported with active link to original file.

"Break component links as external files" - When setting is enabled, imported assemblies and their components will be imported as external files. Otherwise assembly components will be imported as virtual components (they only exist in the assembly and they don't have physical file).