SUCCESS!! A toolpath cut normal to a cylinder (cylindrical cam)

Not to worry. "Distracted" defines my normal state of existance. 8~)

yes post it if you like

I'd VERY MUCH like to look at that model, John. I'll send you an email, but a valid email address for me can be found on the main page of my Web site.

Thanks very much, Mark Staplet>

Unfortunately I don't believe it is accurate, Matt. The surface offset to the inside is what I tried with my cylindrical cam. It doesn't seem to want to offset accurately radial to the axis (or normal to the surface). See the pic I've got up on my Web site:

It doesn't really work. Although I think it SHOULD work.

'Sporky'

Muggs wrote:

Jeff,

My message apparently doesn't go through. My e-mail program fails to send each time I attempt to send a message. How can I send you the STEP files? Do you have a FTP site to which I can upload them?

My approach is to use the Deboss Wrap feature to directly make the cut into the cylinder. In other words, I use no offset surfaces as in Dr. Mather's tutorial.

This approach is fairly close, but deviates from the desired result quite a bit. As the toolpath works around the cylinder, the profile's shape is changing on this part. I can send a jpeg illustrating the problem to anyone interested.

Thanks a million, John. The message is on the Earthlink server (~1 MB). You probably got a spam trap message back (how I long for the "good ole days" when such things weren't necessary). I'll retrieve it and get back to you if it didn't make it thru intact.

Thanks again and sorry to put you thru the trouble.

========================

Anyone else besides me think that the Offset Surface oughta work (although it doesn't)? A radial surface offset radially really SHOULD produce the exact geometry we're talking about with an end mill tool path. The fact that it doesn't says something about what's going on under the hood with SolidWorks. In other words, something smells really fishy here.

'Sporky'

John Eric Volt>

I had to modify the e-mail address before my e-mail program would send it.

I agree completely. I'm quite surprised by some of the deviations I'm seeing as a result of these different approaches.

I would have thought that sweeping along a path created by the Wrap feature would work quite nicely as well, but it has some very strange behavior.

Mark, when you say "radial surface" do you mean something like what's in the screenshot_cam.jpg? If it is, the easiest way to see why that won't work well is to simply create a planar sketch of an arc of, say, 320 degrees rotation and offset that. Offset it to the inside and outside by some distance. If you draw rays thru the arc end points they should intersect at the arcs' center. The same thing happens when offsetting surfaces. (Also applies to emboss type features which work by creating surface offsets.)

If, on the other hand you when you say "radial surface" you mean something like J.D.'s example; it should work for groove sides when "mid" offset or thickened (I have a theory that using a "thicken" function will also give you a good groove bottom surface). If you think it's not working can you explain?

Hello All, I sent this to spork, but you all might have a look:

It avoids the offset surface problem, but still doesn't seem to be right.

Muggs Change "home" to"comcast" to reply

Hi, John. Sorry 'bout my email goof up. Guess "---" isn't going to get it anywhere.

I have to occasionally "re-learn" why sweeping a 2D section doesn't work well. Visualizing the reason is pretty simple though (unless I'm confusing myself again). Simply wrap an inclined line around a cylinder (a helix). Offset the wrapped curve to a smaller diameter cylinder. These two curves could represent sweep paths for the groove ID and OD but they have different normal angles. The difference changes with offset distance; if you offset to 0 diameter the curve is equivalent to the cylinder axis. A planar section is only good for pure annular (revolving about cylinder axis) or axial (parallel to cylinder axis) cuts (or so I believe).

What a wonderful discussion, thanks folks this is very entertaining and educational.

A DUMB QUESTION, though...

I can't claim to be a SW guru, so perhaps I'm just missing something and somebody here can *_edumacate_* a goofy Southern boy with wa-a-ayy too much

*_edumacation_*. I read, and re-read, the posts, and didn't see anything addressing my question.

Consider this:

Since the cam follower path is explicitly defined by a function of (x, theta) where 'x' is the distance of the path in the direction of longitudinal axis of the cylinder and 'theta' is the rotational component of the path on the cylinder

Then why is it not possible to: (a) program a Visual Basic macro of API calls that creates 3D points around the cylinder (on surface or at a depth...no matter) (b) create a 3D spline through the 3D points (c) put a plane normal to the endpoint of the spline (d) put a cutting profile sketch on the normal plane (e) sweep-cut a path along the spline?

I played around with this concept briefly, manually creating abitrary 3D points through a solid object, 3D spline, planes, sketches, 3D sweep. I couldn't figure out how to sweep-cut, though, even though the Help says I can do this (getting too old & lazy, need more coffee). Once upon a time I had done something very similar with Alibre Design and THAT's where I got the idea.

It seems like this would be straightforward to do this. I can't say if the geometry would be accurate, tho.

The original idea that I had was to program a VB macro to create a kazillion

3D points around the surface of the cylinder, create a sketch plane at each point, then extrude-cut the cutter shape all the way around the cylinder as if it was an actual machining process. But I figure that method would have created a monster part file, so I dropped that idea.

Comments?

Kev

"I think what we really need is a way to sweep one solid (endmill) along a path on another solid resulting in the intersecting body being removed - just like the actual machining operation."

This is the method I like to use.

Best Regards, Devon T. Sowell

Show me an example. I was not aware that it was possible to sweep one solid along a path on another solid with the resulting intersection removed. Please try this problem before replying and provide example files. You can post files at the SolidWorks forum at mcadforums.

: "Dale Dunn" wrote : Stepping through the tutorial, it doesn't appear to model what and endmill : would cut. The cam path generated is the shape left by a flat rectangle : swept around the path. Since the endmill has width, there will be parts of : the profile that do not appear to form a smooth surface.If you made an SLI : cam from this model, a cylindrical cam follower would bind in it.

You're right. The tool profile or cross section needs to be always normal to the cut C/L for the model geometry of the cut to be realistic.

David Janes

David, I believe the problem (with a swept planar section) is that there is not a constant normal direction. To cut an accurate groove the plane of the section must warp to match differences in what can essentially be thought of as "pitch angle" at different radii. Or, I might just be confusing myself. Anyhow, I've posted a STEP from a WF2 model at

If you've got the time and inclination examine it and let me know if you spot any inaccuracies. I can also email you a swept groove (WF2 also) and proof that it's not accurate (simple check-fit pin surfaces and intersection curves) to the tune of about .025" on a radius (if I remember correctly).

Here is the method I'm referring to:

1. Create a "solid" of the path the cutter creates. This solid can follow a linear or curved path, as needed.

1. In an assembly, mate the two parts correctly.

2. Using the cavity feature, subtract the "solid" cut from the part.

Best Regards, Devon T. Sowell