How to revolve a surface

[Anonymous]

So, I made a propeler and now I want to build a perfect case for it.

I was thinking to do this steps:

1) revolve de fin and save

2) open a new fil, derive and scale bigger the object resulted of the revolveing

3) use the shell comand to make a cavity in the object to make it the right size

The problem is that I think inventor doesn't let me revolve the fin. So I have 2 questions:

1) how can I revolve the surface?

2) is there a better way to do this case?

I would really appreciate if someone could help me because I am just learning about Inventor.

I am not a native english speaker so I am sorry for my mistakes

PS: The .ipt is attached

[WHolzwarth · Accepted solution]

Right now, Inventor has no quick solution for that task. But it can be done. Some iterations with projected cut edges will do it.

It's a matter of patience, doing more sections than I did.

2017 file attached

[johnsonshiue · Accepted solution]

Hi Guys,

There is a better approach here. I don't have access to Inventor 2017 at the moment. But, I can describe how to do it. This needs to be done via Guide Rail Sweep.

1) Make Sketch9 and Sketch10 visible. These two sketches are very important.

2) Edit Sketch10 -> create a concentric circle touching the start of the spline in Sketch9.

3) Create a straight vertical path (2D or 3D) from the top straight down. The length should be equal to the vertical length of the spline in Sketch9.

4) Sweep -> Surface -> Guide Rail Sweep -> pick the big circle created in step2 as the profile -> pick the straight path as path -> pick the spline in Sketch9 as guide rail.

You will get a surface covering the blades.

Many thanks!

[WHolzwarth]

Hmm, Johnson. Perhaps I didn't go the right road.

But look at my result.

[johnsonshiue]

Hi Walter,

The path has to be at the center. It should start from the center point of the circle and straight down vertically. Try it. It should work. I tried it on 2018 and it worked. I think it should work on 2017 also.

Many thanks!

[WHolzwarth]

Good evening Johnson,

I took another look, and I think, that following your way gets a surface, but not the solution. You could get a surface with Sketch 9 acting as guiderail, but IMO 3DSketch9 should be used instead. And trying to get this Sweep is failing.

See picture, and new attachment.

[Anonymous]

Johnson Shiue, thanks for your answer

So I tried what you suggested, and at the beggining I thought it worked perfectly but then I noticed that the surface didn't match because its not the same if you use the rail of the 2d sketch or the 3d sketch produced.

It would be great if you could be able to use the 3d sketch as a rail, but inventor doesn't allow it.

Can you think in a way to use the 3d sketch as a rail, or another way to solve this problem?

Thanks!!

[johnsonshiue]

Hi Guys,

I am sorry that talk was cheap. I forgot to mention about the need to create the Loft using Guide Rail Sweep also. The original may Loft look nice but you will see undesirable high curvature area within the Loft. It is better to use Guide Rail Sweep. Attached is the solution I was talking about on 2017. Please take a look and let me know if any additional information is needed.

Many thanks!

[Anonymous]

I think I did what you just said and this is the result.

The issue is that it doesnt actually match the fin. If you look closely you could see a space between the loft produced and the fin

PS: I attached the .ipt

Thanks so much for the answer.

[johnsonshiue]

Hi! You need to take closer look at my solution. I did not use any Loft. The Loft2 surface was deleted and recreated using Guide Rail Sweep. I think that is a main difference. Please take a look at the part I attached and let me know if more information is needed.

Many thanks!

[WHolzwarth]

Hmm, Johnson. This is one of the rare cases, where I don't agree with you.

Try this with your latest file:

- Create a half section view in modeling window

- Look at the interior and see the gap between the surface and the fins

At least at one point they should meet. But there's no such zone

[johnsonshiue]

Hi Walter,

Unfortunately, I don't have a better solution than I have presented.

Many thanks!

[WHolzwarth · Accepted solution]

You're not alone, Johnson.

Just now I've stumbled about another way: Rotational pattern of the existing solid.

Calculation takes some time, and the result's quality depends on the number of instances.

[johnsonshiue]

Hi Walter,

I believe this is another case which will benefit from sweeping a solid. Revolve is essentially sweeping along a circle.

Many thanks!

[WHolzwarth]

Normally I don't worry much about my inputs being accepted as solutions. But sometimes it's time for raising a hand ..