Block with helical slot 2

[vtmike]

Hi,
I am trying to get a helical cut in my model and the problem is that I want the profile of the cut to remain vertical while it follows the helical path (just like it would be manufactured i.e. the tool is stationary while the part rotates and translates).

Tried to adjust the settings of the swept cut, but wasn’t able to get a cut that would represent the actual part. I have the part file attached and would highly appreciate any suggestions.

Thanks,
Mike

 

[handleman]

This is basically the only application of the swept solid functionality added in SW 2008.

-handleman, CSWP (The new, easy test)

 

[vtmike]

I tried using the swept solid functinality by creating a multibody part, but solidworks '08 just would not accept the part to create the sweep cut. The part I made was a long cylindrical part with a round base.

 

[handleman]

Since the sweep cut is very new there are pretty strict conditions on how you have to set up the sweep. Did you follow the Help instructions carefully?

-handleman, CSWP (The new, easy test)

 

[CorBlimeyLimey]

The 'cutting tool' has to be in contact (interfering) with the part being cut.

 

[handleman]

My guess is you missed this:

For cut sweeps only, when you select Solid sweep, the path must be tangent within itself (no sharp corners) and begin at a point on or within the tool body profile.

-handleman, CSWP (The new, easy test)

 

[vtmike]

Hi,
Thanks for the replies. Tried it again and this time it worked (attached file & was missing the interfering condition). But the problem still persists i.e. the profile of the hole is still the same as it is with a 2D profile cut. Can't seem to figure out how i can get a cut resulting from the tool being stationary and the part translating and rotating.

 

[rfus]

I took a quick look at your file and found the solution. I first looked at your solid swept cut, and though that you could just change the path alignment type in the options to minimum twist, but that didn't work. I then supressed the swept cut, started a new 3d sketch, selected the helix in the feature tree, and hit convert entities. I went and created a new swept solid cut using the ball nose cutter solid, and the 3d sketch path, and selected minimum twist. This gives you the results you are looking for. I believe since the helix has a inherent normal that does twist, keeping minimum twist will still have it follow this normal, but if it is a simple 3d sketch curve, the cutter will stay normal to its profile with minimum twist selected.

rfus

 

[rfus]

file:

 

[handleman]

Mike,
Is that really what you want? Vertical sides? That's not what will happen when you machine the part in the way you describe. As I understand it, you want the final shape to be the result of holding the cutter in the position you've modeled it in and then rotating the part about the Z axis while simultaneously rotating the part about the Z axis. I hope you don't expect that result to be different from the second model you posted. If you follow rfus's post you will get what you say you want, but that is not the result of the operation you describe. It would be the result of holding the cutter still and moving the part along the X and Z axes while simultaneously moving away from the cutter in the Y axis then moving back to the original Y position.

-handleman, CSWP (The new, easy test)

 

[vtmike]

Thanks rfus!....your idea of creating a 3d sketch from the helix worked fine.
The cutter will remain stationary in verical position, while the part will translate about Z, rotate about Z, and also translate about Y.
Now what in the actual operation will decide the twist of the cut. The angle of the cutter is the only factor that will change the twist, so keeping minimum twist will imply keeping the cutter fixed in vertical direction. I think the part should come out close to the model.

 

[vtmike]

Im sorry the part will not translate about Y...It will only rotate and translate about the Z axis

 

[handleman]

OK, put the part into an assembly. Mate it so that it can only rotate about Z and translate along Z. Model the cutter and mate it in position. You'll be able to manually drag the the part in the way it will be manufactured and see that the second model you posted is right.

Rotating the part and holding the cutter still is no different from rotating the cutter and holding the part still. It's just a matter of your reference frame. This is sophomore kinematics.

-handleman, CSWP (The new, easy test)

 

[vtmike]

handleman you are right, there is going to be a twist due to the rotation of the part. But what I was trying to do was to minimize the twist of the cutter and not make the walls of the cut exactly vertical. The 2D sketch I used earlier was just giving me too much twist for some reason, but the 3D tool made it much better even without the minimum twist selected. This is how I think the part will look like after being machined (attached file)

 

[mjcole]

Use a planar circle as the main path and then guide the sweep along a helix as a guide curve this way the profile is always aligned properly and the guide will position it.

Michael

 

[apmendes]

Hello Mike,
Try a cut loft with a helix as a guide curve.
See attached model.
Paul

 

[handleman]

Guys,

No method other than the solid sweep cut is capable of generating the geometry to accurately represent the result of the physical cut described. This type of helical cut is precisely the reason SW added solid sweep cut functionality.

That being said, there is no reason (in my opinion) to accurately create this geometry in SW unless you plan to create a final "barrel cam" profile via rapid prototyping or similar process. I don't know for a fact, but I seriously doubt any CAM package is going to be able to take the very complex surface from the model and realize that it's created by a simple cutting process. Instead it will try to create the surface with a lot of ball-nose cutter passes.

-handleman, CSWP (The new, easy test)

 

[apmendes]

Hello All,
Attached is another try at this using a cut sweep
with the twisted along path with normal constant option at 0 degrees. I have included an assembly with the a shape
and block with a path mate.
Maybe I am misunderstanding the "remaining vertical" part
of Mike's problem.
Paul

 

[handleman]

The "remaining vertical" part was a misunderstanding of what geometry would be created by the cutting process he described.

-handleman, CSWP (The new, easy test)