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dnewman
Posts: 17
Registered: ‎12-06-2011
Message 1 of 48 (1,865 Views)
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Sweep Cut a solid

1865 Views, 47 Replies
12-06-2011 04:37 AM

Hello all, I hope you can help.

 

I would like to create a feed scroll.  I know this can be done in solidworks (see link). But can this be done in inventor.

 

Scroll Feed 

The Image is similar to what I'm after,  but my thoughts are that this is not possible in Inventor... yet.  Am I Right?

 

The Solid in the image wascreated as a rectangular pattern (1200-off) of a cylinder along a helix path that is then cut from the work piece. In essence this is exactly what im after but as you can see there are far too many surfaces and the resultant cut is jagged especially when viewed with the shaded with edges style not to mention its size the file size 11+ Mb and hence i cant attach it to this post.

 

Is my method the only method available out there at the moment or am I missing a trick?

 

Solid Works Sweep Cut

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Yes, I know that Inventor can't sweep solids, see my first post of this thread.

 

And I did say that the model I did is not 100% correct. Still, you will be able to accomplish the same as a solid sweep by sweeping a 2D section, since the cross-sectional geometry of the swept volume remains constant along the path. The trick is to figure out what that 2D section looks like. Whether the 2D section has a closed-form solution, I can't elaborate on that, my Calculus is too rusted.

 

The original SW part has a volume of 241.8, mine has a volume of 242.0 (error of 0.083%). I don't think that's too bad?

 

Anyway, I'm hoping someone sees something in the way I did it and comes up with a better solution or method.

Thanks.

 

I figured you have to take the 3D path into account somehow, and the easiest is just a silhouette of that 3D path/volume.

 

There's a 3rd, more terse approach, see attached.

 

Sadly, I'm working on a 4th method...

Another solution, this one develops the 2D shape to sweep along the helix. (IV 2012 format). As others have said it would be nice if solid sweeps were included. Solidworks tool is pretty limited and fairly confusing on its own, but at least they are trying.

 

The interference between the tool and shaft is about .00017 in^3, very evenly distributed, likely due to the surface approximation. If you have IV Pro, the simulation shown in the included video (mp4 format) is included.

 

Neil

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JDMather
Posts: 26,893
Registered: ‎04-20-2006
Message 2 of 48 (1,858 Views)

Re: Sweep Cut a solid

12-06-2011 04:40 AM in reply to: dnewman

Coil.

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dnewman
Posts: 17
Registered: ‎12-06-2011
Message 3 of 48 (1,854 Views)

Re: Sweep Cut a solid

12-06-2011 05:14 AM in reply to: dnewman

I'm sorry, my fault entirely, I haven't explained myself very well.

 

I wish to design somethis similar to the items from IAC http://www.iacplastics.com

06-12-2011 13-06-29.jpg

 

06-12-2011 12-47-45.jpg

 

 

The smaller cylinder needs to be cut from the workpiece as if the smaller cylinder (shown) is a mill tool and the work piece rotates as the tool traverses along the length of the work piece.  Such that the profile will allow a similar sized item to the 'Toolpiece' to fit snugly to the scroll so that it can stay at right anglesto the scroll

 

 

 

 

below is the coil method (left) and the pattern method (right)

notice the profile from the coil doesnt result in a regular circular arc

 

06-12-2011 12-59-15.jpg

06-12-2011 13-07-21.jpg

 

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JDMather
Posts: 26,893
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Message 4 of 48 (1,839 Views)

Re: Sweep Cut a solid

12-06-2011 06:12 AM in reply to: dnewman

Coil feature in itself does not start with profile perpendicular to path, therefore

Coil surface - sweep cut. (special settings required here as well)
Attach your SolidWorks file here.

 

Also - attach the Inventor file where you did pattern -

first

drag the red End of Part marker to the top of the browser rolling up all features.

Save the file with the EOP in a rolled up state.
Right click on the filename and select Send to Compressed (zipped) folder.
Attach the resulting *.zip file here.

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whunter
Posts: 200
Registered: ‎06-25-2009
Message 5 of 48 (1,799 Views)

Re: Sweep Cut a solid

12-07-2011 12:19 AM in reply to: dnewman

You're right, not possible in Inventor (the SW way).

 

If you add a 3D helix to the path to fit your 1200-off shaft's cut, and create a user plane on the end of that 3D helix, what does the cross-section (the cut on that plane) look like? What I'm after is, what does/would the 2D sketch look like if it were just a coil.

 

Can you attach a screesnshot here? It is a very interesting problem.

Contributor
dnewman
Posts: 17
Registered: ‎12-06-2011
Message 6 of 48 (1,793 Views)

Re: Sweep Cut a solid

12-07-2011 01:11 AM in reply to: dnewman

Sorry about not replying straight away had to go into a design review meeting that just stretched and stretched.

 

Attached is the Solid works version of the part that im trying to make in Inventor.

 

 

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Contributor
dnewman
Posts: 17
Registered: ‎12-06-2011
Message 7 of 48 (1,792 Views)

Re: Sweep Cut a solid

12-07-2011 01:24 AM in reply to: whunter

The image on the left is a cross section of the coil cut - the image on the right is a sweep-cut both cuts are made with the same diameter but the foot-print (shadow ?) profile are very different. you can see that a cylinder would nestle easily int the swept cut piece but not in the coil cut piece


coil-cut.jpg

sweep-cut.jpg

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sam_m
Posts: 598
Registered: ‎11-05-2003
Message 8 of 48 (1,781 Views)

Re: Sweep Cut a solid

12-07-2011 03:55 AM in reply to: dnewman

Is this what you're after?

 

originally tried by rectangular-pattern a surface extrusion but then realised I'd have to sculpt away EVERY bloody one so gave up on that...

 

so, this way, created a "notch" as an extrusion, patterned this around a coil (3d sketch helix) and this was a solid of all the cuts.  Use this as a toolbody with a combine-cut operation and Robert's your mother's brother...  (or at least I think it's what you're after).

 

Obviously increase the number of parts in the pattern to provide a smoother result (and bring your pc to its knees).

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sam_m
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Message 9 of 48 (1,780 Views)

Re: Sweep Cut a solid

12-07-2011 04:00 AM in reply to: sam_m

500 x pattern along the curve's length:

 

Part1.png

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JDMather
Posts: 26,893
Registered: ‎04-20-2006
Message 10 of 48 (1,773 Views)

Re: Sweep Cut a solid

12-07-2011 05:14 AM in reply to: sam_m

sam_m wrote:

500 x pattern along the curve's length:

 


 

I think the idea is to sweep with a Guide Surface rather than pattern which creates a large file and course surface.

 

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