How to model this?

[sbmathias]

I need to model a groove around a cylinder. The catch is that the groove will not go all the way around the cylinder; it only goes about 190 degrees. It will physically be machined by bringing a rotating end mill squarely into the curved side of the cylinder to the depth of the groove, then rotating the cylinder 190 degrees around the cylinder's axis, then retracting the end mill.

I've made the initial plunge cut hole that the end mill would make, but can't seem to figure a way to now revolve that 3-dimensional cut around the cylinder axis.

Is there some way to do it with a Sweep or a Spiral or ??

 

[EEnd]

Could you just add another hole like your plunge cut at the other end and revolve cut a rectangular profile from the center of the entry cut to the center of the exit cut?

Eric

 

[MadMango]

You could also add a curve on the surface of the tube and do a Sweep-cut.

[green]"I think there is a world market for maybe five computers."[/green]
Thomas Watson, chairman of IBM, 1943.
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[sbmathias]

EEnd:
Yes, I suppose that would work. It does end up being several features instead of 1 (to maintain and modify), but it should work. Given the geometry, I think I have to create several reference planes, etc, but that may be the best way.

I'll see if anyone else comes up with a more sophisticated solution.

MadMango:
I'm not sure I follow how your solution would work. Adding a curve on the surface does give me a path to sweep along, but I think you can only sweep a 2D profile along, and I need a 3D "solid" to remove material.

Would it somehow work to create a solid to remove from my cylinder? That may end up being the same problem, though.

 

[ctopher]

Pick a plane thru the center of the part, create a sketch of the groove on one side with centerline thru the center, revolve-cut to angle you want.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[sbmathias]

ctopher:

As I understand your solution, I would only get a groove with squared-off ends. I didn't specifically say so, but I need to have full-radius ends, like the end mill would make. Did I misunderstand?

Again, my problem seems to originate in the fact that I need to sweep or revolve a 3D solid in order to cut my groove, and as far as I can tell SW only lets you sweep or revolve 2D sketches.

 

[Heckler]

I would follow Chris's idea and then just add a full radius fillet. This would work unless you plan to make this cut with a ball endmill.

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 4.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
o
_`\(,_
(_)/ (_)

"There is no trouble so great or grave that cannot be much diminished by a nice cup of tea" Bernard-Paul Heroux

 

[Heckler]

I'm not sure SWx can do this but I remember doing this a while back in Pro/e but model the cut then position it in the part and do a simple subtract thus getting the groove.

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 4.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
o
_`\(,_
(_)/ (_)

"There is no trouble so great or grave that cannot be much diminished by a nice cup of tea" Bernard-Paul Heroux

 

[Heckler]

Another way would be to create a mold base cavity.

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 4.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
o
_`\(,_
(_)/ (_)

"There is no trouble so great or grave that cannot be much diminished by a nice cup of tea" Bernard-Paul Heroux

 

[MadMango]

I uploaded an image that might help clarify things.

I hope you can see what I have done above. I created a new Plane, then converted the OD of the cylinder to a sketch line. I then Trimmed the sketch to get 190deg arc. I then drew another circle sketch to use for my Sweep-Cut. I finished off the groove by Filleting the ends to simulate a ball end mill cut.

[green]"I think there is a world market for maybe five computers."[/green]
Thomas Watson, chairman of IBM, 1943.
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[ctopher]

You can aalso do what Heckler suggested about subtracting the groove from the part.
Also, see Help for revolve-cut.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[bme0319]

I would also create a sketch on a plane square to the axis of the cylinder and then create an extrusion, removing material to obtain the required groove width.

PP

 

[cadcamguy]

I'd go for creating a datum first so I can tie the up and down with that, then create a revolved cut of the arc... then create 2 more revolved cuts on the square ends, with the first arc driving that

then it will be just like a cut with a ballend mill

 

[EEnd]

I do not think that a full radius fillet of the ends of the slot will give the desired geometry. I believe that sbmathias wants 190 degrees between the centers of the end arcs. A full radius fillet essentially shortens the slot. Trying to cheat and lengthen the slot to compensate does not create the desired geometry either. If a square end mill is being used, the bottom of the end cuts should be planar, not curved.

http://home.comcast.net/~ewetemp/SolidWorks/Round_Slot.JPG

- This is a screen shot of a part with two slots. The ends of the slot on the top were created with an extruded circle. The ends of the slot on the bottom were created with a full radius fillet.

http://home.comcast.net/~ewetemp/SolidWorks/Round_Slot.pdf

- This is a PDF of an end view of the shaft for each slot, showing the shortening of the length of the slot, and the curved vs. straight bottom in the rounded section.

I think you will just have to bite the bullet and make this feature the hard way. I would start with a revolved cut for the slot, and then make two extruded cuts for the rounded ends. Then create a datum plane 90 degrees from each end face, through the bottom of the face. A circle there can be related to the end of the slot and then extruded “up to next”.

As you can see by the number of posts, this is but one of many ways to create the feature. Unfortunately this results in 5 features for what seems like a single feature. I would put them all into a folder in the feature tree and continue to think of it as a single feature.

Eric

 

[meintsi]

a) "I can do in eight features.

b) "I can do in five features.

a) "I can do in three features.

b) "I can do in ONE feature.

a) Name that feature. <-applause goes here.



Anyway, the three feature method is the simple full radius groove with square ends thru a 190° arc, a full revolve on top, and a circular pattern of the revolve with one instance at 190°.


As far as the one feature method, what about a quarter circle ..

(with a small rectangle sticking out of the top to manage the start and end of the sweep, because of the cylinder)( try it without the rectangle and you'll see what I mean)

..used as the profile of a cut-sweep where the path is defined by the perimeter of the entire completed path.

The path would requrie 4 planes to be constructed and a composite curve to be made from the 4 sketches.


But would 4 planes and 1 cut-sweep put me back at 5???







Remember...
[navy]"If you don't use your head,[/navy]
[navy]your going to have to use your feet."[/navy]

 

[crjones]

Try this site there is a tutorial addressing what you are talking about.

http://home.pct.edu/~jmather/content/DSG322/solidworks_surface_tutorials.htm