Overview#
Stitch combines separate surfaces into a single quilt by joining coincident edges. If the stitched faces fully enclose a volume with no gaps, Fusion turns the quilt into a solid body automatically. Unstitch does the reverse: it separates a selected body (or faces) into individual surfaces.
Stitch is the gate between "a pile of surfaces" and "a solid you can machine, 3D print, or assemble".
Where to find it#
- Surface > Modify > Stitch
- Surface > Modify > Unstitch
- There is also Merge in the same panel, but it only works within a single body and only when design history is turned off. For normal parametric work, use Stitch.
Step by step#
Stitch#
- Make sure the surfaces you intend to join share edges, either exactly (after trimming) or closely (within tolerance).
- Start Stitch (Surface > Modify > Stitch).
- Select the faces to stitch into a single body.
- Adjust the Tolerance if needed. Edges within the join tolerance display in green. The dialog shows the number of free edges and the number of edges to be stitched together, and you can expand the Unstitched Edges table and click through the entries to see the gaps. Keep the tolerance small unless you have a specific reason.
- Click OK. The faces are stitched into a single body; if they form a watertight body, Fusion creates a solid, otherwise the result remains a surface quilt.
Diagnosing a stitch that stays a surface#
- Read the free-edge count in the Stitch dialog and click through the Unstitched Edges table to see where the openings are.
- Zoom into each free edge. Common causes: a missing face, a gap larger than tolerance, edges that overlap rather than coincide, and faces trimmed slightly differently.
- Fix with Patch (to fill), Extend plus Trim (to close small gaps), or increase tolerance slightly as a last resort.
Unstitch#
- Start Unstitch.
- Select the faces or solid bodies to break into multiple surface bodies.
- Click OK. The faces are unstitched and display as separate bodies, which you can hide, delete, or modify separately.
- Re-stitch later or use the pieces as construction geometry.
Options reference#
| Option | What it does | Notes |
|---|---|---|
| Faces (Stitch) | Faces to stitch into a single body | Select multiple |
| Tolerance | Maximum gap between edges that still stitch | Edges within the tolerance display green |
| Free edge / edges-to-stitch counts | Show how many edges remain open and how many will join | Shown in the dialog |
| Unstitched Edges table | Lists the open edges; click an entry to see the gap | Expand it in the dialog |
| Faces or solid bodies (Unstitch) | What to break into separate surface bodies | Solid bodies are allowed |
Tips and pitfalls#
Tip: Increase tolerance in small steps. If it takes a tolerance of 1 mm to stitch a model that was designed to be exact, you have a modeling error, and the solid will carry that error into downstream geometry.
Tip: Stitch frequently, not just at the end. Stitching after each trim lets you confirm shared edges early and reduces the number of bodies you must track.
Tip: For a body that will not become a solid, use Stitch on just two neighbors and check which free edge remains. Bisecting the model this way finds the bad seam fast.
Warning: When faces have inconsistent normals, a stitched solid can end up inside-out, with negative volume or strange Boolean behavior. Check the volume in Properties and use Reverse Normal on the offending face before stitching.
Warning: Stitching surfaces that overlap along more than an edge (they intersect in the middle) will not form a valid quilt. Trim first.
Warning: Unstitching a solid loses the "solid" status. You must re-stitch with every face included to get it back. If you only wanted to modify one face, consider Split Face, Delete Face, or Replace Face instead.
Tip: If a stitched solid later fails in Fillet or Shell, there may be tiny sliver faces or edges from tolerance-merged seams. Rebuild the area with a cleaner patch.
Tolerance in numbers#
Stitch joins surfaces whose free edges lie within the Tolerance. If the gap between two edges is 0.02 mm and the tolerance is 0.01 mm, nothing happens; at 0.05 mm they join. Use the smallest tolerance that works, because a large tolerance can pull edges together across features that were meant to stay separate and distort geometry by up to the tolerance.
A practical ladder (general guidance, not Autodesk data; the default tolerance is shown in the dialog):
| Gap measured | Action |
|---|---|
| Under 0.001 mm | Likely within the default tolerance. |
| 0.001 to 0.05 mm | Increase tolerance to just above the gap. |
| 0.05 to 0.5 mm | Likely a modeling error: patch or rebuild rather than stitch. |
| Over 0.5 mm | Not a tolerance problem; geometry is missing or misplaced. |
Measure the gap with Inspect > Measure between the two edges before choosing a tolerance. That turns guessing into one number.
Worked example: stitching a six-sided box into a solid#
You have six planar surfaces for a 50 x 30 x 20 mm box, created by extruding sketches with a few of them offset slightly (0.02 mm) by a sketch constraint error.
- Select all six faces and run Stitch with the default tolerance shown in the dialog. If the 0.02 mm gap is larger than that tolerance, one face stays loose and the body remains a surface (check the free-edge count in the dialog).
- Use Inspect > Measure on the free edges of the loose face and its neighbor; the gap is 0.02 mm.
- Re-run Stitch with a tolerance of 0.03 mm. All six join and, because the body is watertight, it becomes a solid. Check with Properties: the volume should read 30,000 mm3 (50 x 30 x 20).
- If the volume is not 30,000 mm3, a face was inverted or a gap snapped incorrectly; undo and investigate rather than raising tolerance further.
Why a stitch stays a surface#
| Cause | How to tell | Fix |
|---|---|---|
| A face is missing | Free edges visible (shown differently) around a hole | Patch the hole, or add the missing face. |
| A gap larger than the tolerance | Measure shows a gap | Increase tolerance slightly, or fix the geometry. |
| Faces overlap | Duplicated surfaces at the same place | Delete the duplicate. |
| Non-manifold edge | Three faces meet on one edge | Unstitch and rebuild one branch. |
| Normals inconsistent | Some faces appear inside out | Use Reverse Normal on the inverted face, then stitch. |
Unstitch: when to use it#
Unstitch separates the selected faces, or whole solid bodies, into separate surface bodies. Use it to:
- Remove a face from a solid so you can replace it or patch it.
- Isolate a problem face to rebuild.
- Break a body into pieces for individual trimming.
After unstitching, the solid becomes a collection of surfaces, so you must stitch again to make it solid. Unstitching the whole body and re-stitching with a slightly larger tolerance is a classic repair for imported geometry that will not behave.
Failure modes and fixes#
| Symptom | Cause | Fix |
|---|---|---|
| Stitch succeeds but the body is still a surface | Still has free edges | Use the Unstitched Edges table to find them and repair each. |
| Stitch warps the shape | Tolerance too large | Undo, measure gaps, use the smallest working tolerance. |
| Volume is negative | Normals point inward | Reverse Normal on the faces, then restitch. |
| Unstitch gives hundreds of bodies | You unstitched everything including tiny faces | Undo and select only the faces you need. |
| Cannot select faces from different bodies | One body is hidden or in another component | Show them, activate the common component. |
| Result is a non-manifold edge warning | Three or more faces share an edge | Unstitch and rebuild the junction. |
Workflow advice#
- Run Stitch often, not only at the end; open edges are cheaper to find early.
- Keep one component per surface assembly so selection is simple.
- Use the free-edge count in the Stitch dialog, and note it before and after each fix; the goal is zero.
- For imported models, after Stitch check Properties for volume sanity and run a Section Analysis to look for internal faces.
- Keep a pre-stitch copy of the faces (hidden) until the solid is verified.
Stitching across components#
Autodesk's help does not describe stitching across components. As general guidance, if Stitch cannot select a face, check in the Browser whether that body lives in another component, and consider moving the faces into one component before stitching.
Stitching and design history#
Stitch is a timeline feature when design history is on, so editing an upstream surface re-runs it. If an upstream edit opens a gap larger than the tolerance, the Stitch feature fails and turns red. Roll back to just before it, fix the surface, and roll forward. Avoid raising tolerance as a response to a failure caused by an edit; the proper fix is to restore the geometry.
Practice exercise#
- Make a box from six surface rectangles: surface-extrude a 40 by 40 mm square 40 mm tall for four sides, then create top and bottom with Patch.
- Stitch all six. Check that the result becomes a solid and has a volume of 64,000 mm^3 in Properties.
- Unstitch the solid; observe six surface bodies.
- Hide the top surface and stitch the remaining five. The result is an open quilt with four highlighted free edges.
- Re-stitch with the top present at tolerance default; confirm it becomes a solid again.
Stretch challenge#
Build the six-sided box from separate surfaces, deliberately shift one face by 0.04 mm, and stitch with the default tolerance. Diagnose with Measure, repair with the smallest working tolerance, and confirm a volume of 30,000 mm3. Then Unstitch the top face, patch the hole with a new curved top, restitch and check the volume again. Expected result: a solid whose volume changes by the volume of the curved cap, with zero free edges, and a note recording the tolerance you needed.
Related#
- Thicken and Solid From Surface
- Surface Repair
- Trim and Untrim