Combine, Split, Offset, and Boundary Fill

Overview#

Once you have multiple bodies, you need to combine them, cut them apart, and extract new volumes. This page covers the tools that do that:

• Combine: Join, Cut, or Intersect two or more bodies (Boolean operations).
• Split Body: divide one solid body into two using one or more splitting tools.
• Split Face: divide faces using a sketch, face or workplane, to isolate changes to an area (for Draft or Press Pull) without separating the body.
• Silhouette Split: split a body at the silhouette outline seen from a view direction, to create parting lines.
• Offset Face: shift faces on a solid body in a positive or negative direction.
• Boundary Fill: create solids from the enclosed volume (cells) bounded by surfaces, planes, and bodies.

Where to find it#

• Workspace: Design.
• Tab / panel: Solid tab > Modify > Combine, Split Body, Split Face, Silhouette Split, Offset Face.
• Boundary Fill: Solid tab > Create > Boundary Fill.
• Shortcut: none listed in Autodesk's shortcut reference.

Step by step#

Combine#

1. Have at least two separate bodies that overlap.
2. Choose Modify > Combine.
3. Select the Target Body (the one that is kept and modified).
4. Select one or more Tool Bodies.
5. Choose Operation: Join (combines the solid bodies into one), Cut (removes the tool volume from the target), or Intersect (keeps the overlapping volume).
6. Check Keep Tools if you want the tool bodies to remain after the operation (useful for reusing a cutter). Check New Component if the result should be placed in its own component.
7. OK.

Split Body#

1. Modify > Split Body.
2. Select the Body to Split.
3. Select the Splitting Tool(s); they display in the canvas.
4. Leave Extend Splitting Tool(s) checked so the tool extends across the whole body; Autodesk notes you can uncheck it if the tools already intersect the body.
5. OK. The solid splits into two bodies, shown in the canvas, browser and timeline.

Split Face#

1. Modify > Split Face.
2. Select the Faces to Split.
3. Click the Splitting Tool field and select a sketch, face or workplane.
4. Choose Split Type: Split with Surface (projects the splitting face onto the face), Along Vector (projection direction defined by an edge, face or axis; can produce several divisions), or Closest Point (projection direction is the closest distance between the tool and target faces).
5. Optionally check Extend Splitting Tool so the tool fully intersects the faces, then OK. Hold Ctrl (Windows) or Command (macOS) to select multiple faces.

Offset Face#

1. Modify > Offset Face.
2. Select the faces.
3. Drag the manipulator or enter an exact Offset distance (positive or negative; check the preview for which way the face moves). Adjoining curved tangent faces offset when geometrically possible. Committing creates an Offset Face feature in the timeline that you can edit by double-clicking.

Boundary Fill#

1. Position the tool bodies and surfaces so they enclose a volume.
2. Create > Boundary Fill.
3. Select the bodies and surfaces as the tools.
4. Select the cells that make up the enclosed volume or volumes.
5. Choose the operation: Join, Cut, Intersect, New Body, or New Component (Hybrid Design type only).
6. OK.

Worked example: casting core and cavity#

1. Model a part body and a larger "stock" box around it.
2. Combine with Cut, target = box, tool = part, Keep Tools on. You now have a cavity block.
3. Split Body the cavity block with the XY plane to get two mold halves.

Options reference#

Tips and pitfalls#

Tip: Use Combine > Intersect to carve shapes from two projected silhouettes. Extrude the front view and the side view, then Intersect.

Tip: Split Face is a quick way to isolate an area of a face for Draft or Press Pull without creating a separate body.

Warning: Unless Keep Tools is checked, the tool bodies are not retained after the combine. If you will need them again, enable Keep Tools or copy the bodies first.

Note: Autodesk says that when join, cut or intersect operations meet complex or near-coincident geometry, Fusion may automatically use a mesh-assisted fallback, with no settings to change.

Warning: Combine may fail or give an unexpected result when bodies only touch at a face or edge without volume overlap (general experience). Move them slightly into each other, or use Extrude Join from the start.

Warning: Boundary Fill produces nothing if the surfaces leave a tiny gap. Trim and extend the surfaces so they close, or add a plane.

• Check New Component if the combined result should live in its own component.
• Offset Face is what Press Pull opens when you pick a face.
• A Split Face result can be used as a parting line for Draft, or edited with Press Pull (Autodesk's suggestion).
• Silhouette Split can split a shelled body at its silhouette; its Split Solid Body option requires a planar parting line.

Choosing the right tool#

Several of these tools overlap, and the wrong choice shows up later as a fragile timeline.

Combine in depth#

• The Target Body takes the result and keeps its name, appearance and position in the browser. Select the part you care about as the target, not the cutter.
• Join combines solid bodies into a single solid body. If the tools do not touch the target (even a tiny gap), expect the operation to fail (general experience).
• Cut with several tools subtracts all of them at once and appears as one timeline item.
• Intersect keeps the overlapping volume. If one tool misses the target, expect an empty result and an error (general experience).
• When you create a cut, visible bodies participate and hidden ones do not.

Worked example: a mold cavity with numbers#

You have a 40 x 30 x 20 mm housing and want a two-part mold block.

1. Create a stock box 70 x 60 x 50 mm centered on the housing (extrude a rectangle Symmetric, 50 mm total). That leaves 15 mm wall on each side in X and Y and 15 mm top and bottom.
2. Scale the housing for shrinkage: Modify > Scale, Uniform, factor 1.006 (a 0.6 percent shrink allowance is a common general figure, not Autodesk data; use your resin's value). Do this on a copy so the original stays intact.
3. Combine: target = stock box, tool = scaled copy, Operation Cut, Keep Tools on. The box now holds a cavity.
4. Split Body the box with the XY plane at the parting height. Two bodies appear; rename them Core and Cavity.
5. Add a 5 mm sprue: sketch a circle on the top face, Extrude Cut down to the cavity.

Check the result: the sum of the two halves plus the cavity volume equals the original box volume (read each body's volume from its properties). Any discrepancy means a leftover sliver.

Split Body and Split Face details#

• With Extend Splitting Tool(s) on, the tool is extended across the whole body. Turn it off when the tools already intersect the body.
• Split Face with Along Vector projects the tool along a direction you define with an edge, face or axis, and may make several divisions if the vector hits the face in several places. Closest Point uses the closest distance between the tool and the target faces.
• After Split Face the new faces are independent, so you can use the split as a parting line for Draft or push one patch with Press Pull.
• To repeat Split Face, right-click and choose Repeat Split Face.

Offset Face with numbers#

Offset Face on a 10 mm bore by 0.15 mm in the direction that enlarges the bore gives a 10.3 mm bore: the face moves by the offset, so the diameter changes by twice the value. Whether a positive value enlarges or shrinks a bore depends on the face normal, so confirm the direction in the preview and with Inspect > Measure. Autodesk notes adjoining curved tangent faces offset when geometrically possible; fillets next to the face can still fail if they cannot adapt.

Boundary Fill in practice#

Boundary Fill creates cells from the selected bodies and surfaces; you then select cells to generate solid bodies. Typical uses are making a plug from a cavity or building a solid from surfaces crossing a body (general examples). Partial overlaps create several cells; try selecting one at a time and watch the preview.

Failure modes and fixes#

Practice exercise#

Model a ball-and-socket test piece and a two-part mold for it, with numeric checks.

1. Create a sphere of 40 mm diameter and a cylinder 20 mm diameter, 80 mm tall, through its center (axis along Z, midpoint at the sphere center).
2. Copy both bodies (Move/Copy with Create Copy). On the originals run Combine Cut (sphere target, cylinder tool, Keep Tools off) to get a drilled ball. Check Properties: the volume should be sphere volume (33,510 mm3) minus the cylinder section inside the sphere.
3. On the copies run Combine Intersect to get the plug (a cylinder capped by sphere surfaces). Verify drilled ball volume plus plug volume equals the original sphere volume of about 33,510 mm3.
4. Split Body the drilled ball with the XY plane. Confirm two equal-volume halves.
5. Split Face the sphere surface of one half with the XZ plane, then give one patch a different appearance.
6. Offset Face the bore wall by 0.2 mm in the direction that enlarges the bore and measure the new bore diameter (expect 20.4 mm).
7. Make a 70 mm cube, subtract a 1.006 scaled copy of the drilled ball with Keep Tools on, then Split Body the cube at the ball's equator. Finish by using Boundary Fill on three planes crossing a small box to extract one octant.

Expected result: volumes that add up, two matching ball halves, a bore of 20.4 mm, and a two-part mold block. If the volumes do not add up, look for a leftover sliver body in the browser.

Related#

• Extrude (Join/Cut/Intersect operations built in)
• Construction geometry (splitting planes)
• Press Pull and direct modeling
• Shell, Draft, Scale (mold-related)