topic Re: Creating a loft from different 2D Sketches in seperate planes. in Inventor Forum

Creating a loft from different 2D Sketches in seperate planes.

Anonymous — Sat, 26 Jan 2019 21:24:20 GMT

Hi all,

I am trying to define a closed loop for a loft by selecting lines that appear on different sketches. This will mean that the closed loop is a 3D loop, not 2D. The lines should all intersect at nodes, so I'm hoping it will become a closed sketch. The problem is the loft function doesn't seem to let you select lines to build your loop.

I know the usual forum etiquette is to attach the file, but I'd rather share this privately if the solution requires more than just a nod toward the correct technique.

Thanks,

OLC

Re: Creating a loft from different 2D Sketches in seperate planes.

JDMather — Sat, 26 Jan 2019 21:41:13 GMT

Did you fully define your sketch (no lines or arcs can be dragged?

Did you Include Geometry into 3D sketch?
Where is your second loop?

What is special about that geometry (the profile sketches) that I could not simply recreate it in a new file?

Re: Creating a loft from different 2D Sketches in seperate planes.

johnsonshiue — Sat, 26 Jan 2019 23:41:38 GMT

Hi! I assume this should be done using Surface Loft instead of Solid Loft. Did you try Surface Loft?

Many thanks!

Re: Creating a loft from different 2D Sketches in seperate planes.

WHolzwarth — Sun, 27 Jan 2019 10:19:29 GMT

Hmm. Looks like loft is at weekend rest.

I've made some testing with a 2018 file. A basic loft could be done, but no tangent transitions were possible.

I was hoping to get better results with a fillet between the angled faces. But look, what happened.

2018 IPT attached

Some minutes later: Success with new attempt for lofting. Selection of solid body was needed before. But still no luck with tangency.

More Later: Success is no more reproducible. Again failure with new attempts, this time with an additional fillet at the last edge of the angled section

Re: Creating a loft from different 2D Sketches in seperate planes.

Anonymous — Sun, 27 Jan 2019 11:34:14 GMT

@JDMather wrote:

Did you fully define your sketch (no lines or arcs can be dragged?

Did you Include Geometry into 3D sketch?

Where is your second loop?

What is special about that geometry (the profile sketches) that I could not simply recreate it in a new file?

I've gone back into the sketches and they are now fully defined and the lines cannot be dragged.
No, but I've gone ahead and tried this idea. I started a 3D sketch and included the geometry - this was a step forward as I can now select the loop and get a preview of a loft (see picture below). When I OK this feature though I get : "Create loft feature failed / Pull Shock 3.3iv.ipt: Errors occurred during update / Loft54: Could not build this Loft / The input sections resulted in the creation of a non-manifold solid. Use Edit Sketch or Edit Feature to change the feature definition. Use the Surface option if a sheet body is acceptable." What does it mean by a non-manifold solid * ?
The second loop is just an oval directly above the loop (this image shows the preview happening based around JDMather's idea to use the lines in a 3D sketch):

4. The geometry is based around lots of projected geometries that form a model I'd like not to be in the public domain. But you are right, a similar design to the two sketches is easy to mock up for investigation purposes (thank you for doing so). I'm happy to share it to individuals if it helps, but the question is more about how to create a closed loop from two intersecting, non planar sketches - your idea to include geometry into a 3D sketch has gotten me further than I had.

* After a bit of investigation, I was able to use this thread to turn my surface loft into a solid. Thanks to JD Mather for suggesting the 3D sketch and included geometry.

Re: Creating a loft from different 2D Sketches in seperate planes.

johnsonshiue — Sun, 27 Jan 2019 14:33:11 GMT

Hi Walter,

This could be related to the fact that one of the sections has G0 continuity and the other one does not. Try adding a fillet to the G0 edge. It should work better.

Many thanks!

Re: Creating a loft from different 2D Sketches in seperate planes.

Anonymous — Sun, 27 Jan 2019 16:21:20 GMT

Maddeningly, this solution has drawn up a new problem. Originally, the loft that had been made to construct this solid had a strange surface anomaly that meant that Surface offset/thicken couldn't be made to work. The 3D loop has now given me apparently an artefact free body from which to offset/thicken - but now I'm getting this:

Create Thicken/Offset feature failed
Pull Shock 3.3iv.ipt: Errors occurred during update
OffsetSrf73: Could not build this Thicken
Could not attach to face: face could not be found.

A search for the problem 'face could not be found' hasn't brought up anything useful. Strangely, the tool body and all features combined with the new loft exhibits the same issue and I am now not able to offset/thicken anything combined with the new loft. Any advice appreciated, though the forum moderators might want this new problem in a new thread.

Re: Creating a loft from different 2D Sketches in seperate planes.

JDMather — Sun, 27 Jan 2019 16:52:02 GMT

Drag the red End of Part marker to the top of the feature tree.

Now drag it down the tree step-by-step.

(You might also do a Manage>Rebuild All.)

Do you get any errors/issues indicated at any step?

From the limited information you have provided in your image - I don't understand why you would be using Thicken rather than Sculpt.

Re: Creating a loft from different 2D Sketches in seperate planes.

Anonymous — Sun, 27 Jan 2019 20:12:34 GMT

@JDMather wrote:

Drag the red End of Part marker to the top of the feature tree.

Now drag it down the tree step-by-step.

(You might also do a Manage>Rebuild All.)

Do you get any errors/issues indicated at any step?

From the limited information you have provided in your image - I don't understand why you would be using Thicken rather than Sculpt.

Yes, I did get errors that were not being flagged up. I've gone through and corrected everything (they were mostly to do with tool bodies and base bodies in various combined features). I can now use thicken/offset on the new loft from the 3D loop - thanks very much (it has thrown up a new problem that I can't combine that with the rest of the solids, but that's for a new thread I think as the problem in the OP is now resolved).

As for your question - I've finished designing the geometry and the frame of a bicycle that I have been intending on producing as a sort of 'garage project' for a few years. The main aim of the CAD is to produce a mold, that will be part of the manufacturing process. I have not designed the mold, but the bicycle frame. I'm now deriving the mold from that by creating thicken features as new solids. The alternative; to use mold maker or to sculpt the frame as a negative from a cuboid, leaves me with a mold far larger than the frame. My mold only needs to be a very slightly larger version of the actual frame.

A huge thanks for your help.