How to sweep vertical or horizontal profile?

[Anonymous]

Here's another situation that seems impossible in Fusion 360.

Or... I don't know how to do it.

I have a T-spline plane, two corners rounded and sculpted in three dimensions, of which I want to use the 3D edge as path for a sweep. The profile to sweep is supposedly a simple rectangle, but there's material needed above the sweep path and much more below it, so I've centered a rectangle on the starting point of the T-spline edge corner and drew another tall one below it. Select both to sweep.

Problem:

Parallel mode keeps verticality okay, but does not go all the way around to completion. And worse, it keeps the profile (rectangles) parallel to the sketch plane, which is not what I want.

Perpendicular mode oddly angles the sweep inward below the T-spline, which again is not what I want.

I want to keep the rectangle vertical like a curved architectural wall where the wall thickness remains consistent. Yet have the top (of wall) slope down gradually along the length of the wall according to the height of the T-spline edge. Technically, this is probably called perpendicular to the normal angle only in XY plane with Z angle zero. I have Z axis up.

Possible?

Alternatively it can be a boolean subtraction of solids (Cut command in Fusion), but the "top of wall" still needs to be horizontal in cross section where any perpendicular section view of the wall shows top of wall as level. This means some kind of  horizontal sweep using the T-spline edge is still needed.

Any other solution?

[fritter63]

If i'm understanding you correctly, on the last one, can you "cut" the wall after the sweep, using the t-spline as the cutting tool? And just have it "extend" that out so it gets the whole thickness of the wall?

[Anonymous]

Almost.

As I had mentioned, the T-spline, if used as cutting body, is still not "horizontal" at the cutting edge across the wall thickness. The T-spline has been sculpted in three dimensions. It's a surface sloping in all directions.

Imagine a vertical section view of the wall where the wall thickness is always consistent in your section view. The top of wall, though at different height for where you put the section view, has to be horizontal (parallel to XY plane where my Z axis is up).

[Anonymous]

The problem is evident just for rough prototype 3D printing. The unwanted angle of the sweep causes an unnecessary overhang.

[fritter63]

@Anonymous

I got it to work. Gotta eat dinner then I'll post the solution.

[fritter63]

@Anonymous

https://knowledge.autodesk.com/community/screencast/d844c7f4-47e3-4328-89a6-4db3a5706b8f

[Anonymous]

Thank you for the ideas and the screencast!

I think I understand. The Guide Rail method might help.

However, my cutting tool is a sculpted T-spline plane instead of a flat sloped plane. And the "wall extrusion" also came from the edge of the same T-spline instead of a radius arc.

So now I've gone as far as duplicating the Body that is the T-spline plane, moving the duplicate in the Z direction, and using the upper one to cut.

But I'm still stuck.

How to find the intersection between the T-spline and the "wall extrusion" body — to use as Guide Rail reference? I'm thinking this type of 3D spline is not possible in Fusion, especially not for use as path in a sweep or to pick as Guide Rail. True?

[fritter63]

But I'm still stuck.

How to find the intersection between the T-spline and the "wall extrusion" body — to use as Guide Rail reference? I'm thinking this type of 3D spline is not possible in Fusion, especially not for use as path in a sweep or to pick as Guide Rail. True?

Sorry, thought it was clear in my vid. What I did was to create sketches on the two parallel work planes, and then I did sketch->project include-> intersection, and on the popup I selected "bodies" as the selection type. Then I selected the wall body, and it created a line which is the intersection of the sketch plane and the body. This is the line(s) you select for the path and rail.

But, you can't create a sketch on your t-spline. So no, I don't think you can do it with the t-spline. But why do you need the t-spline? If you are just trying to create a sloped wall, using a straight plane should work.. unless it is not a linear reduction in height?

[Anonymous]

Surely a cut using a flat sloped plane is easy. But again, I have a sculpted T-spline plane — and it's sculpted in three dimensions. Imagine an amusement park water slide or roller coaster. There are abrupt changes in direction in both height and left-right to make the ride interesting. Just imagine it. That's what it is. Perhaps my screenshot is visually deceptive. It may look equivalent to a flat sloped plane from your angle.

So your solution to the T-spline form in my design is simply to NOT use a T-spline form in my design?

[fritter63]

Ha, yah. "Don't do that" !

Maybe there is another way to get a couple rails that are lined up vertical, but I don't know how to do it. Hopefully someone from the fusion team will chime in here? 

Sorry, I thought you were just trying to create a sloped garden wall like the one I just finished in our yard.

[Anonymous]

But there seems to be a solution.

Because I cannot find a way to "thicken" the outer faces of a T-spline-cut extrude in Fusion, I've exported it into Vectorworks...

But upon importing back to Fusion, it's now hanging in "translating the *.stp" after the upload. Progress bar seems forever orange.

[Anonymous]

Yes you could 3D print that garden wall design.

Article from Business Insider:

3D Printer creates house in 24 hours.

But now we digress.

[TrippyLighting]

I believe this is possible with Fusion 360 when combining tools from the Model and Patch environments.

The trick seems to be to project the T-spline edge into a 3D sketch.

1. Make T-Spline
2. Create new sketch and project with "Include 3D points> This will leave you with the 3D edge from the T-Spline in this new 3D sketch.
3. Change to the Patch environment
4. Select Create->Extrude and select the 3D sketch curve as the profile. This extrudes into a surface.
5. Change back into the Model environment
6. Select  "Create->Thicken" and thicken symmetrically to otherwise as desired.
7. Trim the bottom with a another sketch and a extrude-cut.

[fritter63]

---

@Kenhain wrote:

Yes you could 3D print that garden wall design.

Article from Business Insider:

3D Printer creates house in 24 hours.

But now we digress.

---

Yeah, those 3D house printers are exciting ,but they've been promising them for years! We just went with Concrete CMU's and a couple (very talented) local guys.

[Anonymous]

Thank you for the tip on Project / Include -> Include 3D Geometry and Extruding in Patch mode. It seems to be the direct solution.

However [ kick me punch me shoot me NOW ],

the Extrude does not perfectly align with the 3D Sketch.

I've followed your screencast step by step. The extrude patch body for some reason does not match the 3d sketch.

It's a curious aberration. Or am I still doing something wrong?

If they align perfectly, then it would indeed be the complete solution using the Thicken command in Model mode.

[TrippyLighting]

It's a perfect fit here:

[Anonymous]

Attached is mine. Something is wrong. I don't know what.

[davebYYPCU]

Your so close, don't despair,

the "3D spline" handles just need a small edit, to pull the curve to match each other.

i was able to make a ramp fitting your description this morning, but being away from my system till Monday, didn't get time to share it.  The same workflow as Trippy did, so no need to double up.

Browny

[TrippyLighting]

Yeah, you did not follow either my screencast, to the written process.

You created a second T-SLine to create your surface. That's not what I wrote 😉

Once you have your projected 3D curve , you need to change into the Parch mode and extrude that curve into a patch/surface.

Then you change back not the model environment and use Thicken to thick that surface etc..

[Anonymous]

Yeah, what are you talking about now?

Attached is the same curve but drawn from scratch. Same procedure. Same problem.