topic Re: Inventor - Sweeping geometry, incorrect taper in Inventor Forum

Inventor - Sweeping geometry, incorrect taper

Anonymous — Sat, 07 Aug 2021 17:21:56 GMT

I am trying to sweep a geometry across a path with a negative taper and it seems to be scaling the taper incorrectly. When I scale the geometry, it shrinks up and down fine, but the sweep taper seems to collapse an arc at the bottom. Is this just something to do with constraints? Because of the arc collapsing I cant taper it without a self intersection error.

https://imgur.com/a/M0Kw6ya

Re: Inventor - Sweeping geometry, incorrect taper

JDMather — Sat, 07 Aug 2021 20:23:44 GMT

Everything looks normal and logical to me.

Can you Attach your file here?

(There is currently an issue with Attachments - you must Reply and then Edit Reply to see the Attachments button.)

Re: Inventor - Sweeping geometry, incorrect taper

Anonymous — Sun, 08 Aug 2021 17:10:47 GMT

Thank you very much for taking a look. As you can see in the attached part, when this profile is swept across the path, it does not scale down properly to make a negative taper. The bottom radius collapses too much.

Re: Inventor - Sweeping geometry, incorrect taper

JDMather — Sun, 08 Aug 2021 18:10:21 GMT

@Anonymous wrote:

...it does not scale down properly

How are you making this determination - there are no dimensions on Sketh24 and I suspect that you are missing intended Tangent constraints? Where are your dimensions?

What is your Design Intent?

Re: Inventor - Sweeping geometry, incorrect taper

WHolzwarth — Sun, 08 Aug 2021 20:19:49 GMT

I didn't look at the initial sketches of the sweep, and regarded them as fixed.

But doing a tapered sweep along 3DSketch15 is only possible with a limited taper angle. In this special geometry it's possible up to -1.3 deg.

2021 IPT attached.

Re: Inventor - Sweeping geometry, incorrect taper

JDMather — Mon, 09 Aug 2021 13:25:49 GMT

@Anonymous

Examine the attached file.

I laid out your Sweep Path arc as a straight line.

What do you observe?

Re: Inventor - Sweeping geometry, incorrect taper

Anonymous — Mon, 09 Aug 2021 16:01:10 GMT

Thank you all for your comments. JDMather, the file you attached for some reason only showed a semicircle, but what I did is I scaled my geometry on the same plane as the sweep geometry ends in. In the image, my goal is outlined in green, a smooth linear scaling of the whole profile. What happens is overlaid and the bottom curve collapses strongly. It seems like this has something to do with constraints but I cant figure it out.

Image here: https://imgur.com/a/3q4YnDi
New IPT attached.

Re: Inventor - Sweeping geometry, incorrect taper

JDMather — Mon, 09 Aug 2021 17:49:36 GMT

@Anonymous wrote:

JDMather, the file you attached for some reason only showed a semicircle,

It seems like this has something to do with constraints but I cant figure it out.
New IPT attached.

I reduced the geometry to only the arc to help illustrate the problem - this is basic geometry - you scale something it gets smaller (or larger).

It has nothing to do with constraints. Simple geometry. Not sure why you Attached a second file - same problem.

Are you a student?

Is this a class assignment?

I know the solution to your problem - but I am trying to help you arrive at the solution in a logical manner.

Re: Inventor - Sweeping geometry, incorrect taper

Anonymous — Tue, 10 Aug 2021 04:04:06 GMT

Thanks, I still cant understand while the SCALE function drops the size linearly while the SWEEP function drops the size of the bottom radius more rapidly compared to the larger radius. I am a hobbyist, I would appreciate any tips for how to draw this geometry so it scales properly. I have tried using arcs instead of circles, etc. Same result.

The new file I attached has the overlay of the goal shape compared to the taper, same as the image in my last post.

Re: Inventor - Sweeping geometry, incorrect taper

BDCollett — Tue, 10 Aug 2021 04:19:50 GMT

@Anonymous wrote:
Thanks, I still cant understand while the SCALE function drops the size linearly while the SWEEP function drops the size of the bottom radius more rapidly compared to the larger radius. I am a hobbyist, I would appreciate any tips for how to draw this geometry so it scales properly. I have tried using arcs instead of circles, etc. Same result.

The new file I attached has the overlay of the goal shape compared to the taper, same as the image in my last post.

I believe what you actually want is a Loft using the 3D sketch as a center rail.

Sweep is only using the one shape and your taper is too much to achieve the result you want.

To do this you will need to fix your sketches up first. They are broken and unconstrained. Try and make sure all sketches are constrained before creating features. You can see in the bottom right corner how many dimensions are needed.

Re: Inventor - Sweeping geometry, incorrect taper

Anonymous — Tue, 10 Aug 2021 15:23:55 GMT

The loft will not work because it is swept across a 3D line and seems to twist in a strange way, that is why I switched to sweep.

The core issue is that during the taper, the profile does not scale linearly (bottom radius scales more than the top radius). It must be because of the way I drew the profile, but not sure how I could do it better.

Re: Inventor - Sweeping geometry, incorrect taper

JDMather — Tue, 10 Aug 2021 15:25:31 GMT

Loft will work if done correctly.

Re: Inventor - Sweeping geometry, incorrect taper

johnsonshiue — Tue, 10 Aug 2021 21:03:12 GMT

Hi Nikita,

What you are asking cannot be done by using Taper Sweep. What Taper Sweep does is to taper the sweep face inward (or outward depending on the taper angle) along the path. So the arc profile segment with a smaller radius may convert to a point sooner than an arc with larger radius.

You may need to increate the profile radius. Or, simply remove the rounds from the profile. Next, create the Taper Sweep. Apply desirable fillets afterwards.

Many thanks!