Can i select more than one profile for sweep ????

[tis07282015]

See attached file. I have sketch 9 (1.25'' dia) and sketch (.625'' dia)

What have I done wrong to complete sweep ? It allows me to select only one circle.

Thanks

Sam

[Cadmanto]

A sweep will only allow you to do one profile.

A loft can do multiple profiles.

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[tis07282015]

I knew loft can do multiple profiles, how about path ? Can it be curved as I have in my file ? Solidwork does.
So my question is Loft or sweep can I do as in my file ?

Thanks

[Cadmanto]

Your part came in with no features.  As in my screen shot in my last posting, if that bent piece is what you are trying to sweep, doesn't look like it needs multiple profiles.

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2018

[tis07282015]

Forget about anything

In my file I have two circles(sketch 9 and sketch 10) and a path(sketch 13)

Can I do whatever you call loft or sweep ?

thanks

[jtylerbc]

I can't see your part's features (including any sketches you have) either.  I assume it may be because you're on a newer version than I am.

Since I can't see your actual geometry, I may be heading the wrong direction a bit.  But it sounds like what you want may be a Loft with Center Line (which would be your path). 

Could you post a screenshot of your sketches?  Since @Cadmanto and I don't seem to be able to see them in your model due to software version or something, that might help clarify what you are trying to do.

[JDMather]

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@tis07282015 wrote:
Solidwork does.

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Can you Attach your SolidWorks file?

Your sketches are not fully constrained (this would be poor practice in SolidWorks or Inventor).

Your path is not constrained to the center of the circles (this would be poor practice in SolidWorks or Inventor).

Your path is not perpendicular to one of the profiles (I would expect that this does not return the results that you are after in SolidWorks).

Is this a class assignment?

Inventor error message tells you that the Profiles and Path are not connected.

[tis07282015]

[cid:image001.png@01D4BA29.84DF01E0]

[tis07282015]

I used to have Solidworks 10 years ago. I don't have it now.

[JDMather]

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@tis07282015 wrote:
I used to have Solidworks 10 years ago. I don't have it now.

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I have used SolidWorks everyday (including this morning) for 17 years.

I always fully define my sketches.

It would make logical sense to constrain the beginning and end of path to the centers of the circles.

[tis07282015]

Can you help me fully define
Sketch 9, sketch 10, sketch 13 ?. After that will it work ?
Thanks

[Cadmanto]

I am flying blind here seeing I don't have a visual of what you are describing, but back in the day when I created ergonomic type geometry, I did it by first creating a series of surfaces shaped and contoured the way I needed them, then trimmed surfaces to ultimately convert them through the thicken command to get the geometry.

Thinking you might have to do this.  So a couple of sweeps using the two different profiles, trim them to get what you are looking for.  It is a shot in the dark, but might be worth exploring.

Looking at your images above, you can have multiple guide curves in the loft.

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2018

[JDMather · Accepted solution]

Edit the path sketch.

Drag the arc away from the circles.

Project Geometry (SWx Convert Entities) the center points of the two circles into your path sketch.

Add Coincident Constraints between the projected center points and the ends of the arc path.

(I already attached solution in previous response above.)

[tis07282015]

Thank you

It worked. I just did not realize that when I created path it did not snap center point.

Thanks again

[JDMather]

In Inventor you have to Project the Geometry. 

There is a way to autoproject similar to SolidWorks, but I prefer to have more control.

But just like in SolidWorks - you can observe color change of sketch geometry when it is fully defined.

If you don't see color change, or thumbtack in browser (-) in SWx, then start dragging endpoints and observe.

This is perhaps the single most important diagnostic technique in both softwares.

[tis07282015]

Great tip.

Thanks again

[johnsonshiue]

Hi! This is fairly easy. Please take a look at attached part. Loft with Centerline rail is the way to go. The issue with the original part is in Sketch13. The arc does not intersect the big circle. Just project the center of the big circle. And, add a coincident constraint between the end point of the arc and the projected center. Then, the Loft should work.

I would be surprised if the exact same geometric condition works in SWX.

Many thanks!