How to make a sweep follow a path around a corner?

[sgoelzerI2E]

I am stuck.

I am trying to add a molding profile to perimeter of an extruded body. This is equivalent to the "follow me" tool in Sketchup. 

It will work in one dimension (as shown), but I need to wrap the profile around the body. 

It fails with a profile tangent error

As shown in the screenshot, I can make the sweep function wrap around a box created as form. 

How do I cut a profile from around a body when there are 90* angles? 

Thanks

Scott

[DDMFGCOINC]

There is no tangency at those 90° corners. That is the reason for the tangent error. I don't believe you can sweep along a path with sharp corners (90° or otherwise). I have only ever swept a profile around tangent arcs, however, so I may learn something here as well!

If you create the sketch and extrude it, the process would work. You'd have to extrude all four edges though.

[davebYYPCU]

Sweep can do that, very common workflow,

I think you are getting the error, due to the tick in the chain select box, unclick that,

then select each leg sequentially, the path should build as you go,

you may need to hold Shift key, if editing the Path.

Might help....

[DDMFGCOINC]

Didn't realize that. Just tried it and it worked with and without the chain selection.

Interesting... 

[DDMFGCOINC · Accepted solution]

An addendum; if you select the path first, then select the profile, it works much better. Selecting the profile first seems to make Fusion go loopy and not allow additional selections in the path. 

However, as I said, I don't typically work with swept profiles on sharp corners, so I may be doing something wrong as well!

I did crashed F360 playing around with it, so I must have done something right.

[sgoelzerI2E · Accepted solution]

OK,

this almost seems like a bug in fusion, (how do I report this?)

but combining the hints and help above produced a workflow that gets it done:

-Fusion will want to select profile by default. This does not work.-

-Click on path and use the shift key to select the components of the path. EDIT (another bug-like behavior: using a selection set does not seem to work; have to do the hard way)

THEN

-select the profile to cut. 

screenshot attached shows success

Thanks everyone,

Scott

[jeff_strater]

@sgoelzerI2E,

Can you share the model and a screencast of the behavior you are seeing?  I have not been able to reproduce the behaviors that you report in this thread, and would like to understand if there is a bug here.

thanks

[DDMFGCOINC]

@jeff_strater

If you draw a cube and sweep a cutting profile along one of the faces (in this case select the profile first, then select the path as an edge of the face) Fusion will not allow you to select all four edges of the face, either through chained connections or selecting each edge individually.

If, on the other hand, you select the path first (chained or not) then select the profile, you can sweep the cutting profile around the entire face.

(Sorry, cannot post a model or video from here)

[jeff_strater]

Ah, thanks for the explanation, @DDMFGCOINC.  I see the difference now between what I was doing and what you were doing.  The difference is:  The sweep preview is destructive of the path geometry.  Sweep generates a preview as soon as it has enough information to do so.  In this case, it's as soon as you select the first segment of the path.  So, when you select the path, a preview is generated, and that wipes out the edge you just selected.  So, Fusion does not recognize that the second edge is actually connected to the first one you selected.  You can select the path by holding down CTRL (CMD on Mac), which will suppress the preview, and let Fusion see that the edges are connected.  See the screencast below.  You are right that if you select the path first, then the profile, Fusion has the path already cached, so it can do it all at once.

Hope this makes some semblance of sense.

Jeff

[DDMFGCOINC]

Awesome, did not realize CTRL would suppress the preview!

Glad I could learn something new out of this. Thanks for the explanation, it makes perfect sense!

[sgoelzerI2E]

I recorded demo with SnapXpro, but I cannot upload it to this forum. If you want it I can sent it to you. 

[sgoelzerI2E]

Thanks,

I understand now,

but that feature is completely not obvious. Would have never figured it out without help. 

A constructive suggestion: A checkbox in the sweep dialog (like the chain one) that duplicates the cmd key hold down. Titled something like 'Suppress Preview'