Loft Issues

[Tim-Peruchini]

I am modeling a complicated piece of a pedestrian bridge concrete structure and am having difficulties creating a Loft.  See attached model file.

My original attempt for modeling this structure was to use a guided Sweep, which resulted in geometry that was close but not perfectly accurate along the entire path (despite being guided, it still twisted a tiny bit).  So I'm trying a Loft to see if that makes the geometry more accurate.  The issue I am having is the usual "guide curve does not intersect profile".  Here has been my workflow:

1. Import path Points from an Excel file.  Use the "Create Spline" feature between all points.
2. Create two workplanes normal to the path; one at the start point, one at the end point.
3. Import CAD profile on both sketch planes, using the start/endpoint of the path as the shared origin with the profile.
4. Create Patches on both profiles so the Loft command recognizes them.
5. Select the path guide curve.

A really confusing part of this is that sometimes the Loft works and sometimes it doesn't, even when I follow the exact same steps.  The times that I have been successful, the geometry is not accurate; the loft necks down and is too skinny near the middle of the path.  I tried adding more guide curves connecting multiple vertices of the profiles to constrain it more, but the issues I had originally only seem to be amplified and I can never get this to work.

Any thoughts?

[JDMather]

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@Tim-Peruchini wrote:  The issue I am having is the usual "guide curve does not intersect profile".  

1. Import path Points from an Excel file.  Use the "Create Spline" feature between all points.

Any thoughts?

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It is quite easy to drag the (connections to the guide curve and observe that it is not in fact connected to the profiles.

Wayyy too many points, contrary to popular belief - more points does not equate to better curve.

Do the cavity separate operation.

I probably would have done the 3D spline as the intersection between a side profile and a top view profile.

[johnsonshiue]

Hi! I could be wrong but I don't believe Loft is the right tool to use in this case. You can create Guide Surface Sweep easily. Make XY plane visible. Start Sweep command and select the profile in the middle and the 3D path -> Guide Surface Sweep -> select the visible XY plane in the graphics window. XY plane helps keep the profile rotation minimum in this case. Please take a look at the attached part.

I am not sure if you are aware of a tool called Autodesk Infraworks. I believe it has extensive workflows helping design infrastructure like this.

Many thanks!

[Tim-Peruchini]

Can you explain what you mean by dragging the connections to the guide curve?  I still don't understand how the sketch was not connected to the guide curve.  If my sketch plane uses a point on the curve as the origin and I am importing a sketch origin-to-origin (and the sketch is connected to its own origin), how is it not inherently connected?  Is that just a quirk in Inventor that you can't trust import placements?

Also, I have Inventor 2020, so I can't open the file you posted.  Can you post a downgraded version?

[Tim-Peruchini]

@johnsonshiue, thank you for your reply.  I have tried doing sweeps and was dissatisfied with the resultant geometry.  I did your method of constraining it to the XY plane to reduce twist, but there is still an unacceptable level of twist that was generated, hence why I am trying a loft.  The final model also needs to be a solid, not a bunch of surfaces.

[JDMather]

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@Tim-Peruchini wrote:

Can you explain what you mean by dragging the connections to the guide curve?  ...how is it not inherently connected?  

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Connections should have Coincident Constraints.

Attempt to drag Sketch54 lines that are "connected" to the spline.

What do you observe?

[Tim-Peruchini]

When I drag the lines, they freely move.  So even though points may actually be coincident, Inventor requires a coincident constraint be placed on intersecting lines?

[TheCADWhisperer]

It might solve without the Coincident Constraint, but for the most robust behavior you should have them.

The other thing I did was create Sketch Blocks of the profile - that way it can be moved as one unit.

I will try to get you a 2020 file tomorrow.

[JDMather]

See Attached file.