Issue with Shell command after the sweep through a spline

[ultimatejugadee]

I have recently started learning Inventor. I am using Inventor 2020.

When I try to use Shell command on an object created after sweep command it does not work. Interestingly this sweep was created after sweeping a circle through a spline. When I tried to do the same by using an arc (through the arch button) instead of a spline it works without an error.

Would you please able to tell me what I am doing wrong? Is spline which is also used to create an arc and much more easier to use cannot be used here?

Thank you very much in advance!

[Yijiang.Cai]

@ultimatejugadee , could you attach the model here for more investigation? Maybe you can also try the workaround below -

1. Create surface sweep

2. Create thicken using sweep surface

[ultimatejugadee]

Hi @Yijiang.Cai 

Thanks for your time! 🙂

Sorry for late replay.

Here is the file which shows error when applying shell command. I have also included the screenshot of the error.

[johnsonshiue · Accepted solution]

Hi! I believe it is a bug. The behavior does not make sense. The issue here is that the profile plane is not normal to the path. As a result, the Sweep body is more complicated than necessary. However, there is a way to make it work. Simply define a normal to path workplane and create a circle on a sketch based off the workplane. Then the Shell will work (see attached part).

Many thanks!

[Yijiang.Cai · Accepted solution]

@ultimatejugadee it looks like an issue related to shell here. We will track this in our system. Anyway there is an workaround to leverage thicken to get the result. Please see the attached model for more details.

[lennypop]

It appears the problem still exists.  The weird thing is that a visible seam will appear on one side when you sweep using a spline as the guide.  The seam is as if the guide is projecting itself out perpendicular to the plane it was created on.  BUT IT IS ONLY ON ONE SIDE.  

[johnsonshiue]

Hi! DO you mind elaborating the issue you are seeing? Are you talking about the seam edge along a closed spline face? If yes, that is the way Inventor works. The edge is there when a spline surface becomes closed. I believe it may have something to do with how to keep topology unchanged when a spline face changes from open to closed. I don't think this is a bug. I am not aware of a plan to change the behavior.

Many thanks!

[lennypop]

I made this as simple as possible, and swept a circle over a spline.  You can see that the line can be seen on one side, but not the other.
When you export this to a drawing, the iso view also has the line.
It is awesome that you responded.

[johnsonshiue]

Hi! In the drawing, you can edit the view and hide "Tangent edges." The faces along the seam should be tangentially continuous. So, the seam can be hidden.

Many thanks!