2016 and 2018 loft issue

[jmackniak]

I have what i think is a simple loft problem and cannot seem to figure out whats wrong.  Using both 2016 and then trying to solve in 2018 but cannot.  The sketches should loft through the three plans.   

the file attached is 2016

[SBix26 · Accepted solution]

The immediate and obvious problem is that the middle sketch doesn't have a closed outer profile.  This is easy to check by just starting the Extrude command to see that there's no profile in that sketch.

But there are other issues, too.  Loft is known to have trouble with hollow profiles-- much better to do it in two steps, especially when the interior is just a cylinder.  But this can be created by a Revolve feature with much better control, followed by a sweep for one of the lobes on the outside, and then a polar pattern of that feature.  You're trying to do way too much in one step.

Sam B

Inventor Professional 2018.2
Vault Workgroup 2018.0
Windows 7 Enterprise 64-bit, SP1

[JDMather]

This is not a 2016 vs 2018 issue - this is a sketching issue.

You are doing too much work.

If I provide a better technique - do you want it as v2016 or as v2018?

[mikegreslick6607]

It appears at though the middle sketch (Sketch2) does not have a complete profile around the outside.  This sketch is also dangerously underconstrained.  You should try making Sketch2 in the same manner that you made Sketches 1 & 3.

[jmackniak]

I deleted the 1" center circle on all planes; was able to loft without issue; then placed 1" hole through the handle.  thanks

[JDMather]

Any time you see repeated dimensions - you should think, "I am doing too much work, maybe I should ask some questions."

[SBix26]

Here's a 2016 version the way I would approach it.  Not sure what your outer profile is supposed look like, but much simpler sketches and better control of the results this way.  Definitely not the only way to do it, either.  Curious to see what @JDMather comes up with...

Sam B

Inventor Professional 2018.2
Vault Workgroup 2018.0
Windows 7 Enterprise 64-bit, SP1

[JDMather]

Nice solution.

The only critique I would have is that you created an unnecessary dependency on the Solid Body.

Ideally all features could be deleted without the sketches "going sick".

2018 file attached.

[kelly.young]

@jmackniak if you want to stick with using Loft here's how you could set it up.

Open up the iLogic Browser > Customize Here Button

Some great examples here! Hope that helps.

Please select the Accept as Solution button if a post solves your issue or answers your question.

[johnsonshiue · Accepted solution]

Hi! For this case, I personally prefer Guide Rail Sweep solution better. Certainly, Loft can be used here but the geometry may not be unique. As long as any G2 continuous surface passing these sections, it is considered a valid solution.

Guide Rails Sweep has more strict definition. I will ensure the profile in each section consistent along the entire path.

Many thanks!