Issue with loft rail

[jphalip]

Hi,

I'm trying to create a loft between two profiles (a circle and a rectangle with rounded corners) using a spline centerline. My issue is that, even though I've selected a centerline, it still creates another rail on the side. And unfortunately I can't seem to move that rail to when I'd like.

Here's the issue:

I tried to edit the loft and drag the rail's position:

But then after clicking 'Ok', the rail returns to the wrong position:

How can I fix this? Please see the problematic Fusion 360 file attached.

Thanks in advance!

Julien

[etfrench]

It's not a guide rail, just where the face(s) meet.  Set Visual Style to Shaded to not show it.

Create an offset plane somewhere in the middle of the model, then Project/Intersect to a sketch on that plane.  You'll see there is no actual break on the side:

[HughesTooling]

If you really feel you need the seem in the middle of the edge you can get it done in the surface workspace. I think it does produce a slightly different shape, see attached file.

[HughesTooling]

@jeff_strater Any idea what's going on in sketch2 in this design? It shows fully constrained but doesn't show enough dimension for it to be constrained!

If you add a line this happens.

And if I break a line these dimensions appear.

[jeff_strater]

Hmm...  that is weird, @HughesTooling .  I'll have the sketch guys look at it.  Clearly not fully constrained at all.

[edit]  I assume you mean Sketch1.  Created FUS-129694 for this

[jphalip]

@HughesTooling @jeff_strater I figure the confusion about the constrained status might come from the fact that the example I've shared was exported from a component of a larger model into a separate f3d file.

[jphalip]

Thanks @HughesTooling. This is really odd. Even when I use the surface loft tool, the seam doesn't land in the middle of the rounded rectangle's side edge:

Also, the reason why I'm trying to lined those up is to guarantee that the resulting shape is symmetric. Otherwise, it looks skewed as you can see with this section analysis:

Am I missing something?

[etfrench]

The curvature comb doesn't look too good either:

[etfrench]

Starting with a rectangle, then filleting the corners after the loft appears to give a symmetrical body with a good curvature comb:

[jphalip]

Interesting. I'm not sure why it's not symmetrical by default with the rounded rectangle, or why that can't be corrected after the fact. Could that be a bug?

[etfrench]

I would vote for bug😊

[wersy]

Surface does it better.

[wersy]

I dug a little deeper.
If you make the base solid with rounded corners, it will be better.

However, the cross-section is twisted.

With two solids it will be even better.

[HughesTooling]

---

@jphalip wrote:

Thanks @HughesTooling. This is really odd. Even when I use the surface loft tool, the seam doesn't land in the middle of the rounded rectangle's side edge:

Am I missing something?

---

Strange, you did try dragging the seam to the midpoint?

Another thing I've tried that lets you pick any quadrant on the circles and midpoint on the obround is break the circles into 2.

Now you can use the solid loft and pick any quadrant on the circle.

The cross section look symmetrical with the seam here.

[wersy]

Both versions are not quite symmetrical.

Body loft

Surface loft

[TheCADWhisperer]

@jphalip 

Q1. Why are your sketches not lined up with Constraints? I can drag Sketch1 anywhere?

Q2. Why are you not making use of symmetry about the Origin?

Q3. Why are your sketches not fully defined (and did you move one of your sketches off of the original sketch plane)?

I can show the correct way to model this - but your true Design Intent is not clear to me.

Q4. And why did you use a complex Spline when geometrically simple arcs and line can define path well within (.04mm difference) manufacturing tolerance.  (And since your geometry is not fully defined - I suspect that .04mm difference isn't even known by you or have any significance other than to make the geometry more complex than necessary.)

Once my questions are answered I can continue discussion with correct modeling technique.

Maybe something like Attached is what you are after...

[wersy]

BTW, My examples refer to aligned sketches

[HughesTooling]

---

@TheCADWhisperer wrote:

@jphalip 

Q1. Why are your sketches not lined up?

Where did this come from? The sketches in the file in the first post are aligned. @jphalip answered in another post that this was exported from another design so probably explains why it's where it is and not fully constrained.

[TheCADWhisperer]

---

@HughesTooling wrote:

Where did this come from? 

---

@HughesTooling 

Hmm, good question.

I just downloaded file again and don't see that offset.

I guess that is one of the dangers of underdefined sketches - I must have accidently moved something.

Hope I didn't confuse @jphalip with this.

[wersy]

In the original, the centre point is shifted by 0.0095mm.