Lofting Circular (Round) Sections

[Anonymous]

All,

I did a cursory search for this issue that didn't yield a lot of results.

Does anyone have an explanation as to why I can't loft (2) circular areas that are at an angle (<90 deg.) to each other?

I had to split the faces, doubling my number of lofts, and then it worked fine.

Just wondering if there's a reason for this? Is there some sort of discontinuity in the solver with circular areas?

Thanks,

Caleb M

[I_Forge_KC · Accepted solution]

Inventor cannot do an annular shape like that as a single loft. You must do something like loft the whole, then subtract the inner section or loft two surfaces and patch/stitch/sculpt. You could also loft one surface and thicken, or split the faces like you did. There are several methods to achieve the shape you're after... but all of them are multi-step.

If you think about this, it would get sticky when trying to specify details for both loft surfaces at the same time (e.g. end conditions and point mappings). This could also create self-intersections if the existing geometry were just right.

Unfortunately, this limitation is more or less across the board in Autodesk products.

[johnsonshiue]

Indeed, this is a limitation in Loft. Loft is a great tool when you have two or more sections and you simply want to create a shape crossing over these sections. You don't really care the transition in between. The issue with supporting ring profile or general multi-loop profile is that the mapping set would not be unique. Assuming you have two rings, you can either map from outer loop to inner loop or inner to outer or outer to outer or inner to inner. It becomes unmanageable fairly soon if you have more than two loops. The workflow becomes unnecessarily complicated and the result may not be desirable. This is why we never bother offering the ability to support multiple-loop profile in Loft.

Many thanks!

[Dnyaneshwar_Maid]

Hi,

Yes I agree with Mr. Forge and just for reference attaching some pictures from my side to having loft desired output

Picture-1

I created loft in 3D Model but not in sheet metal part as shown below. Having 3 sketches in 3 different planes and desired output opted as 'surface'

Picture-2

In 3D Model only choose Thicken/offset command and give the thickness value and which side you want inside or outside as shown below

Picture-3

Final output 

I hope now it is more clear to you and simple way to create a loft of two different sections

Best regards

Dnyaneshwar Maid

[jpatelG3T8Y]

Or try making rails too along with center line and select both while making a loft. That worked for me.