Sweep inside a triangle

[tripleSheva]

I've Googled long and wide, watched videos, but still can't figure this out. I have a triangle of "absolute size" that I want to trace a profile along its inner perimeter. When I use the Sweep command, if the profile is located inside the perimeter I get the following:

If I move the profile so that it is touching the perimeter from the outside, it works as expected, and I get a nice looking profiled triangle:

However, this makes the overall size of the profiled triangle larger than it should be, as it's adding the width of the profile to the body.

The triangle's size (from shortest "base" to opposite point) is meant to be controlled by a user parameter, so that I can create N triangles of varying sizes, with the same profile and "thickness", which is why the profile must be on the inside of the perimeter.

I've even tried coming up with a way to have the profile on the outside, and use a formula to size the triangle based on the profile's width (E.g.: triangleSize - profileWidth * 2), but that screams wrong to me. Can anyone help me?

And while I'm at it, is there no easy way to snap things to one another" I get that F360 is "parametric", but editing the sketch just to add a guide line/point that I can then use to snap to the triangle's outline is stupid and cumbersome. I miss SketchUp's inference system so much!

This is the profile itself, BTW:

[jhackney1972]

Please attach your model.  If you do not know how to attach your Fusion 360 model follow these easy steps. Open the model in Fusion 360, select the File menu, then Export and save as a F3D or F3Z file to your hard drive. Then use the Attachments section, of a forum post, to attach it.

[davebYYPCU]

A set of nested triangles, a Radial pattern if such a thing was implemented?

I think you will be needing to break the system into smaller parts.

editing the sketch just to add a guide line/point that I can then use to snap to the triangle's outline is stupid and cumbersome.

Is required but hardly cumbersome.

Might help...

[etfrench]

No reason to use a sweep.  Just model one leg.  Circular pattern the leg.

[Warmingup1953 · Accepted solution]

I dont appear to get the same issue.

Well, I think I understand the question at least.

[davebYYPCU]

No one said it was equilateral.

[etfrench]

The centroid formula is just a little more complex for non-equilateral triangles.  Sweep is still not necessary.

[davebYYPCU]

Like this one?

The triangle's size (from shortest "base" to opposite point) is meant to be controlled by a user parameter,

Ok, - the Path works inside or outside.

Might help...

[tripleSheva]

Thanks for chiming in, Dave! So my assumption that a sweep can only work with the profile on the outside of the path is correct? It's not a lack of knowledge that is preventing me from achieving this?

>> editing the sketch just to add a guide line/point that I can then use to snap to the triangle's outline is stupid and cumbersome.
> Is required but hardly cumbersome.

I'd argue the opposite; you have to do the following steps every time you want to snap a point/line/surface of one object to another point/line/surface:
1. Edit the sketch
2. Add guide point/lines
3. Finish (close) the sketch
4. Enter Move/Copy mode
5. Select the sketch
6. Select the plane/axis
7. Make the alignment/positioning
8. Finish the move/alignment
9. Edit the sketch
10. Delete the guide point/lines
11. Finish the sketch
Are you saying there's an easier way to do that? Because that would be awesome!

In SketchUp, for comparison, this would take 3 steps (and no focus shifting):
1. Click-drag on the point/line (edge)/surface
2. Move-drag to the reference point/line/surface
3. Release the mouse

In extreme cases, you'll have to add a guide line for reference, but even that doesn't require adding/editing an object, and can be easily deleted afterwards without having to switch object focus either.

[tripleSheva]

Thanks! This helped me understand the issue... It all depends on where your profile is located on the path it is meant to sweep. If you position the profile on one of the triangle corners, the sweep works as expected. If the profile is located along the path (as it was centered in mine), it doesn't work, and breaks in unexpected ways. 🧐

[etfrench]

If you used a formula in Parameters, you don't need to do anything other than editing one of the parameter's input value.

You also don't need guide lines when snapping to a point or a line.  Just use the Coincident constraint or the Trim tool.

Why, and what direction, are you moving the sketch plane?

[davebYYPCU]

Download my file, 

It is not cumbersome to get the. result  you want.  Change the value for my parameter called Adj

somewhere from 1.5 to 2.5 until you get what you want.

Sweep works best when the path penetrates through the profile, but it’s not mandatory.

my list of steps, make sketch 1. Make sketch 2, Sweep,, Cut into 3 parts.

You are new - do  you know the power of the Origin?

In my case, sketch 1 has the origin in the middle of the channel opening, most obvious place to have it.  If extruding / patterning, it might go somewhere else.

You might want to add driven dimension to call out the mitre angles, or 

rearrange the sketch to be driven by the angles, not base lenght.

Sketch 2 the origin is mid point of the base of the triangle.  No drama.  I think you had that.

Both sketches have the same point to work from.

If you don’t use the origin in that way, then you would need Project > Intersect, as the first step of every sketch made after the first one.  Collect the common point from previous data you need.

Might help….

[tripleSheva]

That only works if there's already a point/line to snap to. The beauty in SketchUp is that it has a lot of inferred points that you can take advantage of, like a mid-point of a line, or a center of a surface/component. In Fusion 360, you would need to create those beforehand/on-demand, and then delete those; if you want to retain a clear-looking model.

[tripleSheva]

My apology. I was referring to the cumbersome process of snapping things. Not the setting of dimensions and origins.

[tripleSheva]

Thanks to everyone, I was able to make some progress. 🎉

But now when I try to use a parameter to control the model - after sweeping the profile, and splitting the result into 3 bodies - it fails and throws some errors. My understanding of how Fusion works made me think that this is doable. What am I doing wrong?

I believe I mentioned this earlier, so for context, my goal is to be able to clone these triangles and be able to control each of their profiles separately, along with having their individual sizes controlled via dedicated user parameters.

[davebYYPCU]

It's supposed to work as you are thinking it should.

I had some trouble finding the problem.

You persist in building the sweep to keep the profile inside the Path, (not best practice)

causes self-intersections / errors, and primary cause of failure due to the path intersections being so acute, but we can't change the path. 

I had all sorts of weird until I put the profile on the outside of the path, (best practice) and the file doesn't break for me between 40 and 80 long.  

Might help...

I didn't understand the Capture Positions, at the time you create the Component - Ground it. (best practice)

See if this one breaks.

[tripleSheva]

The reason why I'm keeping the profile inside the path is because I need the final assembly to be no larger than the user parameter. Creating a formula for the triangle dimension to calculate its size based on the parameter and the profile's current width (which might change from triangle to triangle) seems like an overkill to me. Is there a better way to constrain the final assembly to a certain size, without having the profile and other components scale down as a result?

As for the Capture Position, since it was present in so many modification interfaces, I assumed it simply means "update the object's position (origin) to its new position", but google it now it seems like that's not what it does, and that it should be mostly avoided...? 🤔

How else can I move the sketch to the corner of the triangle, without using Capture Position? Using Sweep after the Move, prompts me to capture or revert the position.

[davebYYPCU]

Capture Position only involves Components.

I have no clues from your files, as to why you would move anything. 

Document Origin cannot be moved and sets up file stability. 

Attaching the profile and path to the file origin is best practice.  

Profile inside the Path produces reliable errors, but Profile outside the Path has not so far.

Changing Parameters, requires fully constrained sketches.

The distance between your external path and the working inside path is currently 19.456 mm, 

can be registered as a parameter and used in formulas to suit.

I get it - that you want alternate Paths, with the same profile, editing each path as required.  

My most recent file calls out the length of the base member.

Might help..

[g-andresen]

Hi,

---

@tripleSheva wrote:

How else can I move the sketch to the corner of the triangle, without using Capture Position? Using Sweep after the Move, prompts me to capture or revert the position.

---

this way

günther

[davebYYPCU]

Fine so far, now change the path with Modify > Change Parameter, 

for me I lost one body - poof! gone - and no corner mitre in the corner, yellow Sweep Icon and Red Split Body - same as Pic 1, Post 1, top of this thread.

It does not happen with inside Path.