Failed 3D Sweep

[t.bennett]

I am trying to generate a cam plate, the idea for manufacturing this would be to place it on a rotary head on a mill and move the endmill to centerline and rotate the part while moving the endmill away from it when needed to generate the profile.  I can not seem to replicate this in Inventor and my sweep is producing very odd (or no) results.  What am I missing here?

[ampster40]

I'm still studying this part, but am curious if you attempted to create that 3D sketch for the path outside of any existing solids?  Looks like the path sinks down into the solid and without testing it I suspect this may be what the problem is.  The path itself may not actually sink into the solid, but the sweep that will be made using that 3d sketch will cause the swept body to sink down into the existing solid. 

[WHolzwarth]

This will do. Basic problem seems to be the tangential run of the 3D path versus the planar surface of the cylinder. It's always better to have both sides thickness left.

Walter

[t.bennett]

The 3D sketch is Sketch3 wrapped to the face of the solid.  I've gotten this to work on another part but that has different issues that I'll look into once I know what is causing this one to fail.

Is there another way to generate a profile like this that wraps around?  The one in the picture is close to what I want but does not match the manufacturing process as the flats are the same width at the OD and ID.

[JDMather]

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@t.bennett wrote:

...but does not match the manufacturing process....

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There is far more complication to this than you might expect.

What diameter end mill are you going to use?

[t.bennett]

The endmill diameter is not important as long as the radius is less than that of the lead-in to the cam sections.

Wh - A problem with yours I noticed is that the swept surface raises towards the center of the part, if I modify that to use the top face as a guide it seems to maintain the height across the entire part.

One last thing I am confused about is if this part was made on a rotary head like I have said, I should be able to place an axis on the highlighted face in this picture.  That radius is .625" from sketch3 so if a 1.250" endmill was used that should just be a partial arc but Inventor does not allow an axis to be placed so I still do not think the profile is matching how it would be if made.

[JDMather]

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@t.bennett wrote:

The endmill diameter is not important as long as the radius is less than that of the lead-in to the cam sections.

 ...

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Why do you think I would ask the question if it wasn't important?

[t.bennett]

That would be a programming issue, not anything to do with modeling unless I am missing something.

[WHolzwarth]

Jeffrey is right. Tool diameter has big influence on the shape of the cam surface.

See sample. The blue face is the guiding surface for the tool axis. Only this surface can be used as guide, all other surface offsets (depending on tool diameter) are distorted. You can see the influence by looking at the other surfaces. Though the tool axis is always moving on the same path, you're getting different shapes, depending on the tool diameter.

[t.bennett]

The profile I had drawn was the surface I wanted, not a guide for the tool so tool diameter is not relevent unless the radius is smaller than the tool.  You can make the blue profile with any endmill smaller than 1.25" because of the .625 radius

Edit:  When I said centerline before I did not mean the endmill being on the center of the 3D sketch but the center of the endmill because on the center of rotation of the rotary head.

[WHolzwarth]

You can't get this surface. No matter what tool diameter of a cylindrical tool you're using.

[t.bennett]

So why can you not make that surface?  You rotate the ring with the endmill cutting it, not that difficult.

[WHolzwarth]

Sure. But you won't get what you modeled.

I'll come back in a few hours. Shortly before New Year now here.

[WHolzwarth]

Here we go again. Happy New Year to all forum members.

As mentioned before, expected surface shape and tool shape are interacting. Additionally the diameter of the cylinder tube (external and internal) has influence.

If you want to follow a 3D path on the outside diameter of the tube, do this:

- Create the 2D contour like in Sketch3

- Offset this contour in 2D with tool radius

- Create two 3D curves on the outside of the tube. The upper curve is path for the tool axis

- Sweep the tool axis along the upper curve and create the leading surface for the tool axis

- Offset this surface with the tool radius. That's the shape, which results after machining

That's it, and it's true.

But why couldn't I offset a 0.5 in tool radius back? It's an Inventor self intersection limitation. You can see an upcoming sharp point at the interior tube region. I didn't test it, but IMO an increase of the inner tube diameter would solve it.

Here's room for improvements. Autodesk, are you listening? No Idea Station entry is provided.

Walter 

[wilkhui]

Hi Walter,

Happy New Year to you as well!

Thanks for reporting the failed offset at 0.5 in, we're tracking this using case tfs47028.

Indy