Errors & Fixes
Corrupted SOLIDWORKS file — how to open and recover it
A part that suddenly reports an unknown error, or an assembly that will not open at all, is usually a file damaged while it was being saved or copied — most often over a network or in a cloud-synced folder. Work from the least to the most destructive fix: open a copy locally, let SOLIDWORKS repair it, look for AutoRecover and backup copies, and only then rebuild from the surviving geometry.

Applies to: SOLIDWORKS 2017–2027 parts, assemblies and drawings.
Most likely causes
- Network dropout while saving or copying across the network (most common)
- Cloud sync tool grabbing the file during a save (common)
- SOLIDWORKS crashing or being force-closed during a save (common)
- Power cuts and failing hardware (disk, memory) (occasional)
- Files sent by email or FTP, very old templates (occasional)
Messages that usually mean a damaged file
- An unknown error occurred while accessing the unnamed file. — the most typical one, according to Javelin.
- An error was encountered while trying to open your file. Contact Technical Support… — Hawk Ridge treats this as a corrupt file.
- SOLIDWORKS encountered a problem in the file… — GoEngineer links this, and unknown-error messages, to cloud sync.
An unknown error can also be a software bug, so try the file on another PC before writing it off.
Recovery after a crash

| Setting in Backup/Recover | Default | Notes |
|---|---|---|
| Auto-recover | On, every 10 minutes | Only for files saved at least once; local folder only |
| Backup | Off | Keeps copies after each save; set the number of copies |
AutoRecover files are deleted when you save and close normally — they only remain after a crash. Do not rely on them as your backup.
Assemblies and drawings

Assemblies: open the structure only, as described in the fixes, to find the corrupt component. Drawings: copy the sheets into a new drawing (drag the sheet tabs, or right-click → Copy sheet / Paste sheet) to leave a damaged sheet behind.
Prevention
- Open and save on a local drive, then copy back to the server. Short network dropouts cause bloat, crashes and corruption.
- Don't work inside OneDrive, Dropbox or similar folders — or pause sync while SOLIDWORKS saves. Move and rename with Pack and Go.
- Save before big operations, and never force-close SOLIDWORKS while it is saving.
- Teams sharing files: PDM keeps a local cache and the full version history.
If SOLIDWORKS itself crashes while saving, see SOLIDWORKS crashing. Files that will not save at all are covered in save errors.
Fixes, in order
1. Copy the file to a local drive and try again
Before anything else, copy the file from the server to your own disk and open it there, or open it on another computer. A file that fails on the network sometimes opens fine locally.
2. Accept SOLIDWORKS' offer to repair
Since SOLIDWORKS 2017 a corrupt file may trigger a prompt asking whether to attempt a repair. SOLIDWORKS then works on a copy, skips the damaged parts and reports what it fixed. Expect the geometry back without an editable feature tree — like an imported STEP file. For assemblies and drawings, open the referenced parts first.
3. Look for AutoRecover files
After a crash, recovered files appear under Document Recovery in the Task Pane. If not, open the AutoRecover folder shown in Tools → Options → System Options → Backup/Recover and look for files named AutoRecover Of … with the extension .SWAR. Remove the prefix and change .SWAR back to .SLDPRT, .SLDASM or .SLDDRW. You may need to show hidden files.
4. Restore a backup or an older version
If backups are switched on in Backup/Recover, the previous copies are in the backup folder. In PDM, right-click the file → History, choose an earlier version and Get it.
5. Find the bad component in an assembly
File → Open, choose <Advanced> in the configuration list and New configuration showing assembly structure only. Everything opens suppressed: resolve components one at a time until the error returns. Replace that component or rebuild it.
6. Rescue a damaged top-level assembly
If only the .SLDASM is bad, insert it into a new empty assembly as a subassembly, right-click → Dissolve Subassembly and save under a new name. The mates and components come with it.
7. Rescue the geometry of a part
Insert the part into a new part (Insert → Part), then List External Refs → Insert the features of original part(s) if references are broken → Break All. Or export the body as STEP or Parasolid from an install that can open it and import it back.
8. Send it to support as a last resort
Your reseller can pass the file to SOLIDWORKS technical support. It can take several business days, and success is not guaranteed.
Sources
- GoEngineer — Corrupted SOLIDWORKS Files FAQ (Aug 2018)
- Javelin — How to salvage data from a SOLIDWORKS File Corruption (Nov 2023)
- Javelin — Catch & Repair More Corrupt Files with SOLIDWORKS 2017 (Oct 2016)
- TriMech — How To Troubleshoot an Assembly in SOLIDWORKS That Won't Open (Aug 2020)
- Javelin — How to Fix Corrupt SOLIDWORKS Components in an Assembly (Sep 2026)
- Hawk Ridge Systems Support — Using Auto-Recover After SOLIDWORKS Crash
- Javelin — SOLIDWORKS Backup / Recovery Settings Explained (Jul 2019)
- Solid Solutions — How to recover SOLIDWORKS files after a crash
- Hawk Ridge Systems Support — How to Recover a Corrupt Part File
- Hawk Ridge Systems Support — Unable To Save File
- GSC — Common Causes of SOLIDWORKS File Corruptions (Feb 2021)
- SPK and Associates — Restore SolidWorks File Tutorial (Aug 2022)
- Javelin — How to Fix a Corrupt SOLIDWORKS Drawing (Sep 2022)
- GoEngineer — Cloud file management recommendations (Oct 2025)
Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.
Frequently asked questions
Can a corrupted SOLIDWORKS file be fixed?
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Often the geometry can be saved, but not always the feature tree. SOLIDWORKS' own repair, AutoRecover files and backups come first; after that you can recover the bodies by inserting or exporting the part.
Where are SOLIDWORKS AutoRecover files saved?
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In the folder shown under Tools → Options → System Options → Backup/Recover. The folder must be on a local drive; files end in .SWAR.
How often does SOLIDWORKS AutoRecover save?
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Every 10 minutes by default, and only for documents that have been saved at least once and changed since.
How do I stop files from getting corrupted?
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Work on a local drive and copy back to the server when you finish, do not edit files inside cloud-synced folders, use a UPS, and consider PDM for shared files.
Related
- SOLIDWORKS "Failed to save document" — how to fix itFix SOLIDWORKS 'Failed to save document' and unable to save errors: rebuild and save all, save locally, cloud folders, long paths, read-only files, antivirus.
- SOLIDWORKS keeps crashing — causes and fixesSOLIDWORKS crashing on start-up or while you work? Recover your file, read the crash logs, test with Rx safe modes and fix drivers, settings and installs.
- SOLIDWORKS STEP and IGES import errors — how to fix themFix SOLIDWORKS STEP and IGES import errors: faulty faces and gaps, surfaces instead of solids, 3D Interconnect vs classic import, wrong IGES units.
- SOLIDWORKS default file locationsDefault SOLIDWORKS folders for templates, sheet formats, the Design Library, BOM templates, profiles and materials, and how to point to shared folders.