Sweep Cut a solid

[Anonymous]

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.

 

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

[JDMather]

Coil.

[Anonymous]

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

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

[JDMather]

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.

[whunter]

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.

[Anonymous]

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.

[Anonymous]

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

[sam_m]

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).

[sam_m]

500 x pattern along the curve's length:

[JDMather]

---

@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.

[Anonymous]

The old addage is true... you really do learn something new everyday!

I didnt know that you could reduce the size of a file by rolling up the EOP... excellent! Thanks for that one

any way heres my solution the same idea as sams but its way way too large due to the many surfaces id imagine.

BTW Warning its a resource muncher once you scroll down that EOP.

[sam_m]

---

@Anonymous wrote:

---

@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.

---

ahh, I get you.  I was reading the 1st post as the way he had created it in Solidworks was with a pattern and that's what he was after here.

[JDMather]

---

    

ahh, I get you.  I was reading the 1st post as the way he had created it in Solidworks was with a pattern and that's what he was after here.

---

SolidWorks has a Sweep function whereby you can sweep one solid feature (cylinder) on a path on a second solid feature resulting in the intersecting volume being removed (just like the manufacturing process.
Inventor is supposed to accomplish the same thing with a Guide Surface sweep, but I will have to experiment to see if it actually works with this geometry.

[JDMather]

---

@Anonymous wrote:

I didnt know that you could reduce the size of a file by rolling up the EOP... excellent! Thanks for that one

---

SolidWorks (later versions) works the same way in reducing file size by saving with the feature tree in a rolled up state.

There is supposed to be a way to get the geometry in Inventor - but I will have to experiment a bit.  Check back later - or tomorrow.

[Anonymous]

Thanks

Sorry its taken a a while to explain but its not so easy to explain what im trying to accomplish.

[whunter]

Gents, take a look at the attached, I don't think it is 100% correct, but the method might have some merit. I was playing with this the whole afternoon while I was supposed to be doing real work...

The IPT is attached (rolled up).

[kakaboo]

Nice, but no - that's not what customer ordered. To put it simply, Inventor do not provide options for sweeping solids. Only flat geometry figures can be sweept along path, with option of additional guidance by surface.

[whunter · Accepted solution]

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.

[SBix26]

Looks very good to me.  I, too, wish that Inventor could sweep solids, but since it can't, that doesn't mean that it's simply impossible to achieve the desired result.  The profile resulting from a swept solid has a consistent cross section, which means that if we can do the math (or get Inventor to do it for us), we can sweep a 2D profile and achieve the same results. 

[kakaboo]

I'm afraid sweeping of 2D profile - no matter how shaped and positioned in relation to 3D path curvature - will not produce results identical to sweeping 3D solid. The idea is to emulate cutting action of milling end, commonly employed in modern 5-axis milling machines. Please note that the material is removed by rotating profile of the tool, therefore 3D solid (cylinder, cone, sphere, whatever), not by forcing flat surface thru solid, like - say - tap dies do. 

cherrs.