Is it possible to edit a Sculpt object in the Model workspace?

[bmwenze0]

I was working on an object in the Sculpt workspace and I wanted to edit it in the model workspace, but I'm not able to sketch onto any of the faces of the Sculpt object no matter what workspace I'm in. More specifically I want to extrude cut shapes through the body below which was made using thickened faces.

[TheCADWhisperer]

Are any of the faces planar?

Can you attach the file here?

[bmwenze0]

The faces are planar. I would post the file, but I don't have the permission to do so.

[TheCADWhisperer]

Can you start a new sketch on one of the origin Workplanes?

Have you tried closing Fusion, then reopen?  (I have had some cases where I didn't even bother with that, I just did a full reboot and everything started working again.)

[innovatenate · Accepted solution]

You cannot sketch on a face sculpt body. You also cannot edit a sculpt body from the Model work space. Whenever you finish form, the sculpt body automatically gets converted into a solid (B-Rep) geometry. This can be very powerful when combined with the Timeline since the model features will update when you make edits the sculpt body.

A couple of suggestions for a solution are below.

In the model environment, you can sketch on a planar (totally flat) face. One thing you may consider doing if you do not have a planar face to sketch, is to create a work plane in the position that you need to sketch on. Then use the extrude (cut) feature to remove material from the solid.

Another option is to create sketch on the default plane in the shape that you need a cut out in. Next, convert this sketch into a solid body by extruding the sketch into a solid body. Now, use the move command to position the body where the cut should be. Don't forget to use the reorient command in Move to help position the solid body. Once positioned, you may use the Model > Modify > Combine command to do a Boolean Cut and remove material.

You may also convert the "cut shape" body to a component and then use assemble > joints to position the component. After position, you may again use the Combine command to subtract one component from another.

Another option is to use the Project to Surface command to project a sketch onto a complex surface in the Model work space. Next, create a Patch in the patch work space and thicken the patch to remove material.

I've made a ScreenCast of these suggestions (below). Take a look and let me know if helps.

Cheers,

[bmwenze0]

Thank you very much - this helped me a lot! I really appreciated the screencast as well!