Wrap to Surface

[alexander.blomqvist8WGL5]

Hi,

Long time user, first time caller!

I want to project a 2d sketch on a cylinder, and then use the feature " Solid Sweep", using my projected 3d sketch as path, I've been doing this for years in Inventor.

In Inventor, I do a 2d sketch of the toolpath, then in 3d sketch i use the feature "Project Curve to Surface" selecting Output "Wrap to Surface". Below you can see an example (I know my sketch is not fully constrained).

In Fusion I can't find the corresponding function, i can only find "Project Along Vector" and "Project to Closest Point", and none of those give a desired result.

Will the function I'm missing be added or is there another way I can do this? Do not suggest "Emboss" because it does not give the desired result.

Excuse the spelling and grammar, English is not my native language.

[davebYYPCU]

Do not suggest "Emboss" because it does not give the desired result.

Please describe why this is not giving the required result.

Please describe the shape of the solid Sweep object.

(Toolpath? for a ball nose cutter or endmill of some description?)

Without further information, I would use Sheetmetal > Unfold / Refold if as you say Emboss is not working.

Might help.....

[alexander.blomqvist8WGL5]

Emboss does not give me walls parallel to the roller that is going roll in the groove and Emboss roll's over in the end positions of a Wrapped grove, "Solid Sweep" gives me just what i need.

It's for an endmill.

Thanks for the tip about the sheetmetal, I've seen a guy dong it that way on youtube and it probably works, the thing is that it is really easy to do this in Inventor and it would be really easy in Fusion as well, if "Wrap to Surface" existed.

The "Solid Sweep" feature in Fusion works as expected.

[johnsonshiue · Accepted solution]

Hi! It will be great if "Wrap To Surface" is available on Fusion. In the meantime, Emboss can be used as a workaround. You may make a copy of the main cylinder. Create a closed profile in the 2D sketch (use Offset command and connect the both ends with lines). Next, use Emboss command to cut the cylinder with the profile. Then the cut edges can be included as the Sweep path.

Many thanks!

[laughingcreek]

fusion doesn't have dedicated cam follower tools like inventor.  but there are a ton of post here about how to get the right geometry with the tools that are available.

before emboss, the primary tool was to wrap a sheetmetal part.  this was just to get a surface representing the center of the path.  the surface is then thickened, which achieves the parallel faces you are looking for.  in some cases emboss can now be used to get the path surface.

now we have solid sweep, which should simplify things  a bit more.  but you still have to create the path.  if the path is super simple you can do it manually.  if not then use either the sheetmetal or emboss work around to get your path.

do a search for "cam follower"

[alexander.blomqvist8WGL5]

Thanks for your reply!

I accept this workaround as a temporary solution, and I will cross my fingers that "Wrap To Surface" will appear in a future update. There are quite a few extra steps to get the desired result compared to if only "Wrap To Surface" had existed.