Using an edge or a line as a profile for the Loft feature

[gamelife4dns]

We can use the Loft feature and select a point (vertex) as a profile.

Make for example a pyramid : start from a rectangle, end to one apex point. It works.

What about making a tent ? We can't select an apex line in place of the point.

So, the question is not how to make a tent, but how so select a line as a profile for the Loft feature in the general case. Or how to mimic that.

Thanks.

Steve

[davebYYPCU · Accepted solution]

Change to Surface > Loft and you can select open profiles / rails (within reason)

Might help....

[TrippyLighting]

What tools are the best to use depends on the specific geometry of the specific tent you want to create.

If you can share a picture of what you want to create, we can use that specific case to explain the concepts behind lofting starting from there.

[gamelife4dns]

I think I need the solid Loft feature because in only one operation I get a lofted solid joined to another main solid. Then I can invoke the circular pattern of the Loft feature to still obtain a single body. All of this is done parametrically with user parameters. Not value is used.

The actual case is a bevel gear tooth. More precisely a Klingelnberg tooth type.
Standard and Gleason tooth fades out to the gear cone apex, that is one point. The Loft feature works well for this case. But the Klingelnberg tooth is constant height, so it stretches to a line on the apex, not to a point.

So yes, I can obtain the desired tooth going in surface mode, lofting twice, then patching three times, then stitching, then combining. OK, that's one tooth joined to the main cone body, but Fusion 360 refuses to invoke the circular pattern with all those features as inputs. Keep in mind that I want it parametric. AFAIK there is not way to select bodies parametrically for a final Combine feature, so bodies must be joined while featuring them.

Thank you.

Steve

[TrippyLighting]

---

@gamelife4dns wrote:

Keep in mind that I want it parametric. AFAIK there is not way to select bodies parametrically for a final Combine feature, so bodies must be joined while featuring them.

Thank you.

Steve

---

That, unfortunately is a limitation of the pattern tools in Fusion 360. No auto-stitch or combine!

Not sure when we'll see that implemented.

Certain geometries simply cannot be created with the solid loft tool. It might just be the case that this cannot be done fully parametrically. 

[gamelife4dns · Accepted solution]

I think I found a solution. Selecting faces for the circular pattern instead of features.
So I built one tooth (through multiple features of surface mode) combined to the main cone. From there selecting tooth faces for the circular pattern seems to work, parametrically as I wanted.

Thanks.

Steve

[TrippyLighting]

Just FYI, asking for help, but then not sharing any detail, and then marking your own answer as the solution is considered very bad style

[gamelife4dns]

Well, I'm sorry. I thought I was clear and complete enough.

So, I needed to loft from a profile to an edge using the Solid Loft feature because it allows joining to an existing solid body. From there, a circular pattern of the loft feature was needed to complete the design (a bevel gear, and the body I want to loft is one gear tooth which needs to be replicated to obtain one final gear body).
All this parametrically.

Given there is no way to Solid Loft to an edge, @davebYYPCU suggested to use the Surface Loft feature, which indeed solves partially my purpose. And I selected his answer as a solution too.

But I still needed to Circular Pattern the result to one unique body, and this failed when selecting features as Pattern Type. Maybe because the feature list was too long: 2x Loft, 3x Patch, 1x Stitch, 1x Combine.

Then, I found myself that selecting faces instead of features as Pattern Type was successful.
So, I made one solid gear tooth using 6 features from the Surface mode, I combined the tooth to the main gear body, and then I Circular Patterned the flanks and the top face of the gear tooth to obtain the final gear body.
It works.

Thanks.

Steve 

[davebYYPCU]

This information indicates that you have combined the single tooth to its partner, before the pattern.

I would develope the single tooth as solid new body with some overlap to the partner,

pattern that body, then Combine all to the partner.

Might help....

[gamelife4dns]

The key is being "parametric".

Combining all bodies as a final operation is not parametric unfortunately (or I did not succeeded to it).

The number of teeth (bodies) is set in a User Parameter which I can not use in the Combine feature.

Steve

[TrippyLighting]

---

@gamelife4dns wrote:

The key is being "parametric".

Combining all bodies as a final operation is not parametric unfortunately

---

I’ve asked  for that for a number of years, but unfortunately it has not happened yet. I personally would consider this core functionality, as a opposed to costly (for the end user) extensions , for example.

[davebYYPCU]

I need an example, to assist further, otherwise it word pictures.

[steveETUVA]

I found myself with the same question but found a way around it the issue of not being able to loft a profile to a line (in Solids.)

Instead of lofting from a profile to a line - if an approximation is acceptable - you may want to consider simply lofting to a very narrow rectangle instead of a line. This way it is just a normal profile to profile loft. E.g. rectangle width of .001mm.

When selecting the narrow profile it requires a little zooming in to be able to select the narrow portion.

[TheCADWhisperer]

@steveETUVA 

Doesn't sound like something that I would do.

[davebYYPCU]

Agreed. Would be a few of us in that boat.

[steveETUVA]

Not sure about the value of your reply. Somebody may find it of use as a workaround, where an approximation is acceptable.