Machining a groove in a cylindrical part

[pshepherdson]

Hi All,

Today's question is this:

I need to cut (machine) a goorve about the circumfernce of a round part, a cylinder. It's a zig-zag cut, that repeats twice around the part. The width of the cut needs to be constant, as well as the depth. The inner points of the zig zag need to be sharp. Ideally, I envision the part being chucked in a lathe, then the end mill would drop down & cut the groove.

The attemp shown is done with the graph sweep path, but the feature that sweeps remains constant to the part axis, it's not 'normal' to the intended cutting path, which is what I'm after. I'm assuming there is a simple way to 1) make the path I want to cut along (Assumign the graph path I created above), and 2) then sweep a solid feature (the end mill / a cylindrical shape) along the path to remove the material. this feature wodu be tangent to the surface of the cylinder..

Any ideas?

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[TomD.inPDX]

There are two issues here but one is easy, the second is problematic in Creo.

Your fabrication method is accurate. The sweep profile is pretty easy to accomplish, I suggest using a Wrap feature and have the sketch understand the pi*d characteristic to control the angle on the face. This is pretty easy. The wrapped curve should understand the normal, but it not, you may need to have a "shadow" curve that is offset from the 1st to manage the normal. Sharp points on the inside is easy with a minor caveat depending on the tool shape.

Know that as the tools changes from vertical to horizontal, the aspect of the edges changes due to the cylindrical nature of the surface. Rectangular tools are immune to this, but angles or radius tools are not. Similar to milling a chamfer into the curved surface of a rod.

The problem comes in where Creo will cut a planar sweep but not a 3D tool sweep. This is hugely problematic in Creo as there is only one way to confirm that the tool is different from the planar sweep. The difference is minute in some cases and doesn't matter, but in many, the variation is huge. For instance, the involute on a gear tooth is created with a hob tool (cylindrical) and all the faces are straight. The involute is created due to the leading edge of the tool, not the section.

The only way to account for this is to pattern a material-remove 3D shape of the tool along the origin of the sweep. You can place a point on the sweep origin and pattern that point along the curve. Then use a reference pattern to emulate the tool along the origin. This often fails several instances due to accuracy settings, but it will give you an idea as to much the tool affects your intent.

Let us know if you would like more information on a specific part of this reply.

[TomD.inPDX]

Of course, I say all this and try it afterward and things are different. The sharp corners are undercut as you go deeper into the part. You have to decide where you want the sharp to be.

You can drive a machinist absolutely batty with something like this:

[pshepherdson]

Hi Antonius,

Yes, not the machinist, but the jeweler! this is only about 1/4" - 3/8" in diameter! The part will probabaly be cast once teh design is finalized. yes, good point on teh undercut. Hadn't really thought of that. So, a 'cone' for a cutting tool is acceptable, to manage the undercut. (And due to teh size, the 'flat' at teh top of eth undercut will be ... small.

Either image you've shown is good.. Your first paragraph is interesting. Can you elaborate a bit more..

>>Your fabrication method is accurate. The sweep profile is pretty easy to accomplish, I suggest using a Wrap feature and have the sketch understand the pi*d characteristic to control the angle on the face. This is pretty easy. The wrapped curve should understand the normal, but it not, you may need to have a "shadow" curve that is offset from the 1st to manage the normal. Sharp points on the inside is easy with a minor caveat depending on the tool shape.<<

I assume I've done the wrap feature, and the pi*d characteristic needs a bit of an explanaiton. And a bit of guidance as to how to 'punch' a solid to follow [cut] the path.

I think I get it, but understanding it & doing it in Creo are sometimes two different worlds!

[TomD.inPDX]

A v-cut would make things easier but it still has artifacts of it's own.

This document will probably make it easier to use the wrap tool... apply the information to your wrap feature...

Closed and Ground Spring - Alternative to Helical Sweep

Remember to use the construction coordinate system in your wrap sketch!

I am using a relation in the flat sketch to provide the circumference of the part. This way you can manage exactly where features land radially on the cylinder. You can use "pi" in relations as a function.

I will also suggest considering an alternative fabrication method. You can do a lot more with rapid prototyping. You don't have the machining limitations. You just have to get around the 3D modeling challenges. Have a look at what Shapeways can do for one-of-a-kind metal castings. http://www.shapeways.com/