Fixing CATIA Data Errors with CATDUA

June 9, 2021 Iouri Apanovitch

Have you ever experienced a persistent “OK to Terminate” error when opening a CATIA file? Or the Desk command popping up telling you that the model has missing links, while you see none missing? Or the model failing to regenerate without any rhyme or reason?

If so, enter the CATDUA (CATIA Data Upgrade Assistant) utility.

CATDUA is a part of CATIA V5, and is a tool for repairing errors in CATIA files. Which means, yes, CATIA files, particularly from older CATIA releases, usually contain data errors, which may start manifesting themselves once you switch to a newer CATIA release.

CATDUA has many helpful uses, among those being:

  • Upgrading older models to a newer data format
  • Fixing broken links when opening CATProducts
  • Resolving update failures in sketches and other features
  • Cleaning document references (such as when the Links dialog appears)
  • Improving performance and reducing the file size

In general, we strongly recommend running the model through the CATDUA whenever you encounter any odd and inexplicable behavior when opening or editing a CATIA model. We also recommend using CATDUA before exporting a CATIA model to an external format, such as STEP or IGES.

For best results, use CATDUA at regular intervals as preventative maintenance to reduce the risk of CATIA data related issues.

CATDUA can be run in two modes: Desk mode and Utility mode. The differences between the two modes are summarized in this table.


Desk mode

Utility mode

Nb documents

Processes a single document

Processes multiple documents



Corrections are effective in the CATIA V5 session. Not automatically saved to hard drive or to PDM system

By default, cleaned files are saved to a local Temp folder. Must be moved to the workspace or to PDM system by the user



Does not check/clean links between documents (CATProduct, CATPart, CATDrawing, CATAnalysis, etc.)

Checks/cleans links between documents (CATProduct, CATPart, CATDrawing, CATAnalysis, etc.)



Can be reviewed immediately in the current CATIA session, before being saved

Must open the processed files into a CATIA session to view the changes after cleaning


To run CATDUA in Desk mode, open the document in CATIA and select File > Desk to start the Desk window. Select the document in the Desk tree, right-click and select CATDUAV5.


It is recommended that you run the check before you clean. Select Check and set all other options in CATDUA V5 dialog box as shown below.

Click Run and wait until the check report displays in your Internet browser, like shown below.

Note that detected errors are prioritized:

  • Priority 1: Cleaning action may lead to data deletion. Though very rarely, this may produce models that fail to regenerate geometry
  • Priority 2: Cleaning action may lead to data modification, i.e., may result in a change in model geometry
  • Priority 3: Unimportant errors, always safe to repair

To review the detected errors, click in the report on the models with the Detected codes.

Complete description of all error codes is available in CATIA Documentation in the following section: Infrastructure > Advanced Tasks > Using CATDUA V5 > Table of Detected Return Codes.

To clean the model after checking, select Clean and click Run. Once the processing finishes, review the report again to verify that the cleaning went successfully.

If any errors of Priority 1 or 2 are reported as fixed, do not save the model yet. Examine the model interactively to make sure there have been no other failures or unwanted changes introduced. If you see no unexpected changes, save the model to make the repair permanent.

To run CATDUA in Utility mode, select Tools > Utility and double-click CATDUAV5 to start the batch dialog.

In the CATDUAV5 dialog box that opens, select whether to Check or Clean, then the error codes, the files or folders to process, and the folder for the cleaned files, as shown below.

IMPORTANT: Since the processed models are not opened in CATIA session, you must click the Licensing Setup button and select the CATIA license configuration to use. Selecting a general use CATIA configuration, such as MD2, or HD2, or CAC, is usually sufficient for most CATIA models. However, you must select specific add-on licenses if you intend to process files that contain technological data, such as SMD for sheet-metal design, CD3 for composites, TUB for tubing design, etc.

Click Save button if you want to save the batch parameters and run it later. Otherwise, select Run to execute the batch. Note that this may take considerable time, depending how many files are processed and how large the files are.

Once processing is complete, select the  icon to review the report. If any errors of Priority 1 or 2 are reported, open and examine the repaired models directly from the Target Directory.

If no undesired results are found in the cleaned models, close the CATDUAV5 dialog box and move the files from the Target Directory to your workspace or to the PDM system.

If you need more information or assistance with the above, please contact us: 

About the Author

Iouri Apanovitch

Senior Technical Training Engineer<br><br>As a senior member of the Rand 3D team with a doctorate degree in Finite Element Analysis (FEA) and over 35 years of experience, Iouri provides design, consulting, and training services to those in the aerospace, automotive, electronics, and consumer goods industries. Iouri is a seasoned pro in 3D parametric design and prototyping using knowledge-based engineering methods, and has worked on a wide range of projects including BOM automation, CMM points generation, automated 3D annotation creation, and die tooling automation design. He is also a sought-after instructor and holds the designations of both CATIA Certified Professional (Expert level) and CATIA Certified Instructor.

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