Trouble creating a surface

[fritter63]

Getting pretty frustrated trying to figure out how to do this or even if I'm taking the right approach.

See attached picture. I need to have a t-spline surface between the arc and the solid body so that I can create a smooth

transition.

I *think* what I need to do is to *patch* a surface using all the connecting lines? say for instance, half of the arc, the spline from the apex of the arc to the solid body, half of the curve on the solid body, the line going down the solid body, and lastly the spline curve from the solid body back to the arc edge.

However, when I try do to patch and select all of these (and why do I have to de-select chaining to able to select multiple?), then the patch dialog won't let me select OK to create the patch surface.

Is this even the right approach? I get ZERO errors from Fustion 360. Is this a problem with the segments not connecting  correctly?

While we're at it, why am I unable to edit a sketch that was copied from another drawing (and there in a "base feature")?

Also, can someone tell me how to do screen casts so I can share the video to help solve the problem? Is this built into Fusion or is it a seperate app to record? (Mac OS X).

Thanks.

[jeff_strater · Accepted solution]

I think that you want to use a Loft here.  Assuming that you want a solid body result, I would just use solid loft.  Select the half circle as one profile, and the body face as another, then use Rails to select the 3 guide curves (I turned off chain select to make sure I only got those curves).

Here is a screencast showing how I did it on a model similar to yours:

For screencasting, go to https://screencast.autodesk.com/, and you can download the free screencast tool.  It works pretty well, in my opinion

Jeff Strater (Fusion development)

[TrippyLighting]

You could try to do a loft with three rails.

The rails would be the two curves on the corners of the arc and one curve on the apex of the arc that connect to the main body.

The first loft profile would be the arc-sketch. Select the yellow inside, not the arc or line.

The second surface - I am not sue if this works as it is curved and I can't try from my iPad - would be the curved surface of the main body that you are trying to connect to. It has a solid black line vertically and you may want to convert that into a construction line so you only get one surface offered for the second profile selection.

The screencast tool is an extra but free download from the Autodesk website. Once installed you'll find an extra red button in the upper right corner of Fusion 360. When done recording and accept the upload it will automaticaly upload the video to your A360/Fusion account and will send you an email when the video is available for watching with a link that you can copy into a post.

[fritter63]

Thanks for your help guys! I think that would work (and much simpler too). But I'm having troubles doing it locally and I think it's due

to that vertical line on the solid body surface for the second loft profile. 

When I select and right click, it won't give me the option to either delete it or convert it to a construction line, in fact I"m not even sure

why it is there. Any ideas? It also won't let me select those two surfaces to stitch together.

Thanks

[TrippyLighting]

How was that line created. Is it part of a sketch or is it some form of split line ?

[fritter63]

OK, I think I almost have this, except that I get an error "the rails must intersect every profile". I think is because my rails at the corner

of the arc are actually two lines (a line and a and arc). Is it possible to select two lines like that? Or can you "join" them together somehow?

The reason they are like that is that I need it to an arc for most of the distance, then for the last 3/16" it just needs to be a straight line down to the arc corner.

Maybe I just have to create the original profile with a spline?

[fritter63]

ok, got it to work! Just needed to make sure those splines were actually connecting to the body vertices, overlaying the 2D drawing was not doing that 

apparently.

Picture Attached.

This at least shows me how to get it done, and now I can play with getting the exact shape I want.

Thanks guys (esp for "working" on a Sunday).