Help - Sweep Tool Not Working as Expected

[Anonymous]

I have just recently started using Inventor 2015, and I'm currently struggling with the Sweep tool. 

My goal is to design an oblong, dome-shaped part with a flattened side (imagine a cap for a finger tip, like in this image):

The previous part has been created using a tapered extrusion, and a subsequent fillet and shell - but it gives me very little control over the shape of the "dome" (since the extrusion is basically following a straight line, and the shape of the fillet is also fixed).

So I thought of using a sweep instead. The sweep path would be the cross section at the base:

I then sketched the sweep profile onto a plane perpendicular to the sweep path plane, like this (it's just a quarter of an ellipse for this example, the actual part would use splines, but the principle is the same):

 

Now, when trying to apply the sweep, I get two kinds of error messages:

• "Path does not intersect profile". Well, that's true... But why does it need to intersect? Isn't it sufficient for a sweep if the profile and the path touch along an edge? But anyway, even if I "fix" this (by artificially extending the profile sketch beyond the path plane), I always get:
  
  
• "The attempted Swep operation results in a self-intersection. Try with different options or inputs." I also understand that... But I don't get why the self-intersection is a problem here, if all I'm trying to obtain is a solid that is the union volume of all those slices (and I don't care if they intersect).

For my understanding, this seriously limits the usefulness of the Sweep operation.

For example, I can take my profile and Revolve it around the Z-Axis, but this would of course limit it to a circular cross-section (since there's no way to select a rotation path). OTOH, I can take my cross-section and extrude it, but again, that limits the profile to a linear path (since there's no way to select an extrusion path). That's where I thought the Sweep would come in - but I can't use it due to said limitations.

So my questions are:

1. Any hints on using the Sweep operation correctly to create a part of the desired shape?
2. Or... Is Sweep perhaps the wrong tool altogether? How would you guys go about creating a part from the above input? Lofts?

Any help is greatly appreciated. Thanks in advance.

[JDMather]

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gstercken wrote: 

Now, when trying to apply the sweep, I get two kinds of error messages:

• "Path does not intersect profile". ..., even if I "fix" this (by artificially extending the profile sketch beyond the path plane), I always get:
  

1. Or... Is Sweep perhaps the wrong tool altogether? How would you guys go about creating a part from the above input? Lofts? 

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"artificially extending the profile ..." is does not sound like the correct solution to solve that error to me.

Simple Project Geometry a single point from one sketch to connect the other sketch sounds like the solution to me, but without the file.....

Sweep does not sound like the right tool for this job.

Loft or Boundary Patch.

Model the portion that you can model as desired (it sounds to me like a good portion should be a simple Extrude) and then post the file here.

[Anonymous · Accepted solution]

If it were me trying to create that shape I'd use Loft with a base sketch and a sketch near the top of the shape, use a rail either side to control the curvature up the shape, then possibly a Delete Face with heal to finish off the top.

Screen shot attached. 

[Anonymous]

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@Anonymous wrote:

If it were me trying to create that shape I'd use Loft with a base sketch and a sketch near the top of the shape, use a rail either side to control the curvature up the shape

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Thanks Tim - actually, while waiting for replies, I had already started experimenting with lofts, and it looked like the way to go. However, the really helpful hint was about using rails, now I finally understood what they are for, and that they are the way to solve my exact problem. Your screenshot was also very helpful.

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@Anonymous wrote:

then possibly a Delete Face with heal to finish off the top.

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That part was a bit confusing to me... Where exactly do I find the "Delete Face"? In any case, I was able to approximate it now by making my top sketch sufficiently small.

Thanks again!

[Anonymous]

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@Anonymous wrote:

artificially extending the profile ..." is does not sound like the correct solution to solve that error to me.

Simple Project Geometry a single point from one sketch to connect the other sketch sounds like the solution to me, but without the file.....

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Okay, I get it now... I need to use "Project Geometry" between the perpendicular sketches in order to "connect" the geometries. 

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@Anonymous wrote:

Sweep does not sound like the right tool for this job.

Loft or Boundary Patch.

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Thanks, I'm trying Loft now, looks like the way to go. I'll also have a look at Boundary Patch.

[Bert_Bimmel]

I would appreciate an option within the sweep-feature to avoid self union upon intersection. In the example shown below, that would mean, that the red and green faces respectively the blue and the yellow one would remain single, uninterupted cylinders, and the highlighted edges won't exist

The point is: I cannot model a multi-layer wave spring without gap, because when the sweeping-profile's height matches the helical sweeping-path's pitch, the modeling kernel gets confused with self intersections it can't resolve. Thus, an "ignore"-option would be helpful here:

[WHolzwarth]

I didn't test it, but for the wave-spring I can imagine only a one-turn wave, and a rectangular pattern for the other waves. Melting together can be avoided by multibody creation or a tiny minor thickness of the section versus the pattern step.

[Bert_Bimmel]

I did try that, but the result was unsatisfactory too: in order to avoid Union-confusion, you'd need to create a multi-solid part (where bodies can intersect without union), plus the joint where the end of the first wire and the beginning of the second wire will etc. not perfectly match.

[WHolzwarth]

Can you upload your file?

[Bert_Bimmel]

Bitte schön!

[WHolzwarth]

Perhaps like that. Still a MBP, but looking not really bad.

2020 IPT attached.

[Bert_Bimmel]

Looks quite nice! That's probably as close as you can get without my proposed enhancement of the modeling kernel. Thanks!

[johnsonshiue]

Hi! Another approach is to split the path into multiple segments. Then create multiple solid bodies so that they don't merge together (see attached part).

A few notes worth mentioning.

- To split the path, the easiest way is to create a surface based on the original path. Then split the surface and use the edges as the path.

- Guide Surface Sweep is needed here so that the profile does not twist along the path.

Many thanks!

[Bert_Bimmel]

Hi. Sorry, but your approach busts the idea of a parametric model, where you can modify the parameter for the number of turns, and the model will update correctly without any further user interaction.

[johnsonshiue]

Hi! Here is another attempt without creating multiple solids (see attached part). In this one, I created one sweep body. Then use swept surface to split the side faces.

Many thanks!

[Bert_Bimmel]

Hi Johnson,

oddly, when increasing the parameter for the number of turns,  Inventor swaps the start end point of the sweeping path, so that the resulting solid extends to the opposite direction. I cannot find an option to control start and end point (which would anyway result in an incorrectly updating model without the user swapping it back):

3Turns - Sweeping counterclockwise

5Turns - Sweeping clockwise