Helical cut on a shaft

Here are some pictures of the endmill exit point I was refering to:

I think you are correct. Planar sections won't work and the reason is seen if you consider the "pitch angle" (cutter tangent) for a given pitch helix at different radii. At the work piece axis (zero rad) the angle is zero, relative the axis, and moves toward 90 with increasing radius.

The best deal I've found is to model a "ribbon" surface (by what ever means is available to you) that would represent the trace of the cutter axis. If, for instance, you use the work piece axis as a sweep trajectory, the helix as the section X vector control, and section (profile) plane defined as normal to work piece axis; you can than sweep a line connecting the axis and helix to produce the desired surface. (You'd actually want to sweep a portion of the line or trim the surface at groove diameter.) Some "loft" or "blend" functions appear to work as well, I believe. Depends on how they map the input curves (axis and helix). Wrapping a curve on cylinder and then surface normal "pulling" it to groove dia can also give you a good set of curves for a loft type function or maybe sweep. Doing a symmetric, surface normal thicken of that surface should produce an accurate groove. Groove walls should be, I can't remember if it looked like a good rep of groove bottom as cut by an end mill or not. Ball end would make things just a little more complicated, but I think combining a swept circle cut and the thicken might work.

(Ya know, I've never actually heard this from a machinist but think what they will really be interested in is a curve that describes the intersection of the cutter axis with a cylindrical surface of some (any arbitrary) diameter. I'm guessing they'd be happier having that curve than trying to reverse engineer it from model surfaces. More important if the curve isn't something as simple as a helix (?).)

Dr J.D Mather Has some very good tutorials that may be of use checkout 5b.

James,

Try performing two extruded cuts simulating the plunging of a slot drill (you can't plunge end mills in the real world) into the start and end of the helix. This may be difficult to set up, but you should be able to work it out. Then perfom a sweep along the helix with a rectangle normal to the helix like you were before. These "plunge cuts" are good machining practice, and should provide the runout you need at the end of the helix to overcome this problem. It is something that you don't notice in the real world and most machinist would not know about it, as it cannot be distinguished from normal tool chatter in smaller sizes.

Dominic V.

James,

What you are trying to do is actually more complex than one would think.

There are multiple ways to create the slot with actual machine tools. The most common misconception is that you can just plunge the tool in and then rotate the part about Y for instance while traversing in X. This will create a slot with the requested width, pitch and max depth, however the slot will be shallower at the side walls due to the undercut created by the diameter of the tool. The correct way to create such a slot is to use a small tool (roughly 25% of the slot diameter) and perform a pocketing routine using the slot outline as your boundary. The easiest way I have found to create this is to model the slot in 2D then wrap the profile using Y axis substitution to control the Y rotation. (in mastercam not SolidWorks)

That said, the second method of creating the slot on an actual machine takes longer than the first to program (not too much though) so we calculate the undercut for a given tool diameter and pitch then select the appropriate depth to compensate for that undercut. Then we create the helical blind slot the easy way as is modeled in the SolidWorks Part below.

You can also make sure your CAM that follows the slot has a generous enough radius that the undercut doesn't matter.

I have inserted a link below to the part for you to look at in SW2006 SP0

Cadguru

Thanks for the tips guys.

Cadguru, thanks for posting the part. However, my SW2006 is still sitting in its pretty little box on the shelf. None of my clients have upgraded yet. I'd love to, but until at least one of my clients do, I probably won't.

I agree with Jeff Howard - what the machinist probably really wants is the centerline of the endmill cutting the helix. The rest is sort of for looks.

For the function of the part, I need to have a pin follow the helical path. I know if a 1/16" end mill could do it, that a slightly undersized pin will follow the groove. So really, the rest is just for looks in my case.

You don't have to upgrade to 2006 - just load it as a new installation. That way you can have both. I install each version in its own folder such as C:\Program Files\SolidWorks2006 and the same thing with the common files. However, I don't have toolbox, so there may be an issue there. Someone that does, please chime in here.

WT

Yeah, I'm sure I'll end up using both simultaneously, but I'm not looking forward to it.

"Ooops, I opened the SW2005 client's files in SW2006...". I'm dreading the day I do that. The longer I postopone installing 2006 as a second installation, the longer I'm safe from that happening.

It's frustrating though, because I'd really like to start playing with it!

Here is a link to the part you can open in 2005. It is featureless, but shows the actual geometry created by the tool in this type of cut path.

Cadguru