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Errors & Fixes

SOLIDWORKS STEP and IGES import errors — how to fix them

A STEP or IGES file that arrives as loose surfaces, with faulty faces or missing parts, is usually not SOLIDWORKS' fault: the bad geometry is normally created when the other program exports it. SOLIDWORKS has two import engines and a repair wizard, Import Diagnostics. Knowing which engine you used decides which fixes are available.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Imported 3D part with highlighted faulty faces and gaps next to a STEP file icon
Import Diagnostics: faulty faces and gaps between faces found in the imported body.

Applies to: SOLIDWORKS 2017–2027, STEP, IGES and other neutral formats.

Most likely causes

  1. Bad surface geometry or trim curves written by the exporting program (most common)
  2. Neighbouring faces whose edges almost meet, leaving gaps (common)
  3. IGES rather than STEP — the format most likely to give errors (common)
  4. 3D Interconnect link that blocks repairs until it is dissolved (common)
  5. Units in the file header that do not match the model (occasional)
  6. Not enough RAM for a very large STEP assembly (large files)

Which engine imported your file?

Comparison of the 3D Interconnect import engine and the traditional import engine
Each engine handles some files the other cannot — try both.
3D Interconnect Traditional import
Switch Enable 3D Interconnect checked Enable 3D Interconnect cleared
Link to source file Kept until you break or dissolve it None
Import Diagnostics repairs Only after Dissolve Feature Yes
Topology errors in the tree Not shown Shown
Assembly ↔ multibody part Both directions Multibody part to assembly only

Engineers Rule found that neither engine is reliably better, and that a very large STEP import can crash simply because all of its data stays in memory. The settings you used last are reused on the next import.

Repair workflow

Import Diagnostics panel listing faulty faces and gaps with Attempt to Heal All button
Heal everything first, then repair what is left one face at a time.
  1. Import into a new, empty part — Import Diagnostics needs a tree with only the imported bodies.
  2. Let SOLIDWORKS run Import Diagnostics and click Attempt to Heal All.
  3. Repair what remains individually. Self-intersecting faces cannot be healed: delete them and rebuild them with surfaces.
  4. A clean result says that no faulty faces or gaps remain. Then Check the body and save it as a SOLIDWORKS part.
  5. Changed something and want to diagnose again? Save as Parasolid and import that file into a new part.

Ignoring the errors costs later: features may fail on the bad faces, edges can be lost in DWG/DXF export and the part may refuse to export to STEP again.

A specific error: "invalid record index"

Javelin traced the STEP message Encountered invalid record index to one entity type and fixed it by turning off 3D Interconnect, renaming that entity in the file with a text editor and importing again. Keep a copy of the original file before editing it.

Repairing surfaces is covered step by step in the surfacing course, starting with surfaces vs solids. Formats and their limits are in the file formats reference.

Fixes, in order

  1. 1. Ask for STEP instead of IGES

    Fictiv's experience is that IGES files give the most errors. Asking the sender to re-export as STEP — the same geometry in a more robust format — often solves the problem before you start repairing.

  2. 2. Try the other import engine

    Tools → Options → System Options → Import: Enable 3D Interconnect switches between the 3D Interconnect engine and the traditional import. In Engineers Rule's tests each engine failed on files the other handled, so import twice and keep the better result.

  3. 3. Run Import Diagnostics and heal

    Accept the offer to run Import Diagnostics after opening the file, or right-click the imported body → Import Diagnostics. Click Attempt to Heal All first, then repair the remaining faces and gaps one by one. It works only while the tree holds nothing but imported bodies, and not on a part still linked through 3D Interconnect.

  4. 4. Dissolve or break the 3D Interconnect link

    Right-click the inserted file → Dissolve Feature to turn it into native geometry so Import Diagnostics can heal it. This cannot be undone; the link to the source file is gone. Break Link keeps the body but stops updates from the original file.

  5. 5. Knit surfaces into a solid

    If the file arrived as surfaces, use Knit Surface with Create Solid checked. Unknitted edges show blue; the Gap Tolerance option finds small openings. Thicken (Create solid from enclosed volume) and Intersect (Create Internal Region) are alternatives. Missing faces can be deleted and refilled with a filled surface.

  6. 6. Find the bad geometry with Check

    Tools → Evaluate → Check reports invalid faces and edges far faster than Import Diagnostics, but does not fix them. In an imported assembly it shows which components need repair at part level.

  7. 7. Fix wrong units in IGES files

    A model 25.4 times too big usually has an inch header on a millimetre model. Javelin's fix is to correct the unit codes in the IGES header with a text editor, or to scale the body by 1/25.4.

  8. 8. Turn on automatic healing

    Under System Options → Import → General, PLM Group recommends Automatically run Import Diagnostics (Healing) and Perform full entity check and repair errors for the traditional engine.

Sources

Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.

Frequently asked questions

Why does my STEP file open as surfaces in SOLIDWORKS?

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The faces do not form a closed, watertight volume — usually because of gaps or faulty faces from the exporting program. Heal them with Import Diagnostics, then knit the surfaces with Create Solid checked.

Why is Import Diagnostics greyed out?

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It only works while the part contains nothing but imported bodies, and not while the body is still linked through 3D Interconnect. Dissolve the 3D Interconnect feature, or re-import into a new part.

What is 3D Interconnect?

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An import engine that inserts neutral and other CAD files with an optional link to the source file, so changes in the original can be updated. Turn it off under System Options → Import to use the traditional engine.

Should I use STEP or IGES?

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STEP. It carries solids and assembly structure, and import guides report fewer errors than with IGES.