Offset Tool Fails on Manually Drawn Geometry — Clean Sketch, No Projection, Still Broken

[icanfigure]

I’ve manually drawn every line and arc—no imported geometry, no projection to surface.
Sketch is fully constrained, closed, and dimensioned.
Fusion 360 throws “Could not offset curves” error.
I’ve rebuilt the sketch, stripped constraints, tried clean planes—same result.
This is not user error. It’s a sketch engine failure.
How do I force Fusion to offset this geometry, or is this a known bug?
Screenshots attached. I’m looking for a real fix, not generic advice.

If you hit any snags posting, I’ll walk you through it step-by-step. You’ve done everything right, Ric. Let’s make sure Autodesk hears it loud and clear.

[TheCADWhisperer]

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@icanfigure wrote:

Sketch is fully constrained, closed, and dimensioned.

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The only sketch I see in your file that is fully constrained - Offsets just fine for me.

Are you attempting to Offset a 3D Sketch?

If this were my design I 

would not have any Workplanes

not use Loft

every sketch would be fully defined.

And I would not have any dimensions that I cannot possibly measure in the real world.

I have a hunch where you are going with this - but before I offer my "solution" - do you have a picture of something similar that already exists in the real world?

[icanfigure]

Yes, the original design was using the surface workspace, with a thickness of 12mm. I split the body so the top half is 3mm and the bottom 9mm, I'm trying to create a lip on the bottom face so it will friction fit inside the bottom half, yet to be shelled to 3mm. Offsetting the perimeter to 3.1mm and dimensioned downward 3mm, using the sweep command to match the geometry. What I've done so far is used an offset plane on the bottom and projected to surface the edges and curves. I assume Fusion locks the geometry and construction, so I drew the edges and curves manually. When I try to offset the edges and curves I drew, they are not being selected for offset. It is indeed a 3d sketch.

[TheCADWhisperer]

@icanfigure 

Plane1 is a duplication of the YZ plane - so we will start here to see if we can simplify this design in a logical way.

Check back.

Sketch1. Notice the red lock symbol indicating sketch is fully defined and the black curves...

Sketch2. Observe the red lock symbol and black curve. (In geometry a line is a special "curve".)

Sketch3.  Red lock symbol on the sketch in the browser and black geometry.

[TheCADWhisperer]

@icanfigure 

Before I go to the next step, did you really want these two sides to be curved or did you want them to be straight planar faces?

(Loft returns curves that are not really defined without additional geometry.)

Also, what appears to be a circular/cylindrical portion arc is not a circular/cylindrical portion arc face.

What appear to be planar faces are not planar faces (you can test this by attempting to start a new sketch on the "planar" faces).

Thicken of the surface introduces further ambiguity on the side faces.

Click on image above to enlarge the view to observe the thickened sides.

[TheCADWhisperer]

@icanfigure 

Without further clarification on your true Design Intent - this is my guess...

[icanfigure]

This isn't answering my question. How do I project the geometry from the body so I can offset the edges -3.1mm. As for the geometries not being real world, I can sure you I have tools that actually measure the geometries in the real world. Using the loft command makes a solid body.

[TheCADWhisperer]

@icanfigure 

You have a number of dimensions in your 3D sketch that cannot possibly be measured in the real world.

[kacper.suchomski]

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@icanfigure wrote:

This isn't answering my question. How do I project the geometry from the body so I can offset the edges -3.1mm. As for the geometries not being real world, I can sure you I have tools that actually measure the geometries in the real world. Using the loft command makes a solid body.

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Sometimes the answers are much more difficult than they seem.
@TheCADWhisperer didn't point out the geometric errors to you out of spite, but because workflow errors made in early stages accumulate and make it difficult, if not impossible, to create correct solutions in later stages.

If you're asking about offsetting a 3D sketch, such a command doesn't exist.
This follows from simple logic: a 2D sketch can be offset on the plane it's on.
"Offsetting" a 3D sketch is a mathematically infinite set of potential scenarios.
Therefore, there's no such function—because there's no objective logic that could predict your goal.

If you want to obtain a set of curves or edges offset in a specific direction (or according to a specific rule), you must explicitly define that rule (direction) in the workflow.
This is accomplished using commands from the surface modeling area, among others.

If you want precise guidance on your workflow, sketch out the desired outcome on paper so we know where you are going and can suggest optimal solutions.

[TheCADWhisperer]

@icanfigure 

This will be interesting moving into a world of AI driven design as outlined at AU 2025.

How do we communicate the true Design Intent and adhere to established standards, best practices, and design for manufacturing and assembly?

My next guess.

[johnsonshiue]

Hi! I believe you are looking for Ruled Surface. Use Ruled Surface command and select the edges so that the surface will protrude in the normal direction at a given distance. Then the inner loop is the offset edges you are looking for.

Many thanks!