Need Help!- cutting micro V profile for belts

[boilerbots]

I need to make some micro-V pulleys, "K" type. The "K" size is most commonly used on automobiles since the 90's.

The V groove is a 40 degree angle with the grooves repeating with a 0.140 pitch. I am making a pulley to match belts with 4 ribs.

I have a 3 axis CNC mill, manual mill and a really good Monarch lathe.

The first several pulleys I made with on the lathe using a bit I ground to a simple V shape getting it as close to 40 degrees as possible. This worked sort of but it was hard to control the chatter since the tool was cutting into a V and cutting on both sides. The cut needs to be at least 0.134 deep according to Gates drawings.

What is the best way to go about doing this?

If I only use the lathe, what type of tool should I use?

If I use the mill, how should I do it? Custom end mill?

[Charles Lessig]

For cutting 60 degree screw threads the tool is usually fed
in at 29 and 1/2 degrees so it cuts on the left side and just
shaves a little on the right side. Sometimes the last pass on
threading is a tiny movement straight in just to shave both sides.

This might help for your 40 degree grooves.

[John Welden]

You should be able to do it without chatter on the lathe.

If your setup and bit are good than most of the time you can increase the feed or decrease the rpm to get rid of chatter. Don't be afraid to use very low rpm, like as slow as the lathe will go if need be.

Cutting in .140" isn't asking for much.

Make sure your setup is as rigid as possible.

Maybe your grind on the bit is bad? Take a picture and post it.

You could do it on the mill but you'd need to get a custom cutter or have the tools to grind your own. I suppose you could make a tool holder to hold your 40deg lathe bit.

[boilerbots]

Originally Posted by John Welden You should be able to do it without chatter on the lathe. If your setup and bit are good than most of the time you can increase the feed or decrease the rpm to get rid of chatter. Don't be afraid to use very low rpm, like as slow as the lathe will go if need be. Cutting in .140" isn't asking for much. Make sure your setup is as rigid as possible. Maybe your grind on the bit is bad? Take a picture and post it. You could do it on the mill but you'd need to get a custom cutter or have the tools to grind your own. I suppose you could make a tool holder to hold your 40deg lathe bit.

I will post a picture, my grind isn fairly flat on top, no chip breaker because I was concerned with patching the angle of the V and couldn't worry about much else.

Also 0.14 isn't that deep but with a 40 degree angle it is cutting on both sides of the tool quite a bit.

My tool post and lathe is very rigid.

It might be interesting to to make a holder for the mill like a fly cutter without any angle to the cutter bit and see what would happen. I already have to do some secondary operations on the mill so if I can just do the whole thing on my CNC mill that would save me some time.

I need to make 3 more pulleys this weekend, so I might be back posting some updates soon.

[John Welden]

Since you've got other milling to do, the fly cutter type setup might be fastest and most consistent. All you would have to do is turn down a shank, mill a slot and put in some set screws.

To figure out the diameter of your custom cutter, you can use the mill to quickly figure it out. Center the spindle over the edge of a block of aluminum and set a zero. Load your custom cutter and back away from the block. Feed back into the block until the bit just scratches. (its up to you how accurate you want to be when you pick up the edge.) Now you'll know the radius of your cutter and you can program your part.

[HuFlungDung]

What is a Monarch? Is that as good as a Summit?

I've made quite a few poly-v sheaves on my Summits: its a 19" swing, uses a 12" chuck and while not considered to be heavy duty, its no p***y either. Chatter has not been a problem.

You need to support the pulley with a chuck, and not between centers. You can use a mandrel if you want, but it should be a chucking mandrel that you make up with a threaded stub to hold the pulley blank.

For tools, I take a Kennametal top notch thread tool holder and rough the grooves with an ordinary thread tool. This will help the more acute custom tool to last longer. Then, I take and grind the 40 degree point on another top notch thread or grooving insert and finish the machining with that. It is to your advantage to use carbide because if you can run the part fast (400SFM in steel), you can get a much smoother, shiny groove that doesn't require some sort of hand filing and polishing.

Take care that your custom tool is not given too much clearance. The flanks should almost be vertical, and not way undercut, because your feedrate is very slow anyways. Minimizing the tool clearance causes the cutting edge to approach the condition where the tool almost wants to rub on the work. While this increases the required infeed pressure, it also stabilizes the workpiece and kills chatter. So experiment a little bit with that, less clearance is better than more, and you only need a wee bit.

I wouldn't feed in with the compound along the angle of the vee because most likely, you'd be using the compound to space the grooves.

Advance the tool fairly aggressively, don't baby it. Firmer pressure, combined with minimal tool clearance keeps chatter at bay. Feed in to depth quickly, then back out immediately, as soon as the workpiece has come around once at depth. Don't give chatter a chance to build. Do all the grooves this way, then come back and take a more careful tack when finishing: feed in to a distance say .010 or .020 from bottom depth, and feed the tool right, then feed left, trimming one sidewall at a time. Advance the tool and feed right and left again. At final depth, you won't have much room to jog right and left, but by then, you'll not be trying to remove much material anyways. If necessary, grind the tool to a sharper point so that you can move it .001" left or right when at full depth.

You'll need to be concientious about observing the compound dial readings to do all this, and competent at keeping track of backlash in the compound as well, But that will take the hair off your head and put it on your chest, where it counts

[boilerbots]

Originally Posted by HuFlungDung You need to support the pulley with a chuck, and not between centers. You can use a mandrel if you want, but it should be a chucking mandrel that you make up with a threaded stub to hold the pulley blank.

I have soft jaws that I cut to match the stock material. I am only making pulleys from aluminum.

Originally Posted by HuFlungDung For tools, I take a Kennametal top notch thread tool holder and rough the grooves with an ordinary thread tool. This will help the more acute custom tool to last longer. Then, I take and grind the 40 degree point on another top notch thread or grooving insert and finish the machining with that. It is to your advantage to use carbide because if you can run the part fast (400SFM in steel), you can get a much smoother, shiny groove that doesn't require some sort of hand filing and polishing. Take care that your custom tool is not given too much clearance. The flanks should almost be vertical, and not way undercut, because your feedrate is very slow anyways. Minimizing the tool clearance causes the cutting edge to approach the condition where the tool almost wants to rub on the work. While this increases the required infeed pressure, it also stabilizes the workpiece and kills chatter. So experiment a little bit with that, less clearance is better than more, and you only need a wee bit. I wouldn't feed in with the compound along the angle of the vee because most likely, you'd be using the compound to space the grooves. Advance the tool fairly aggressively, don't baby it. Firmer pressure, combined with minimal tool clearance keeps chatter at bay. Feed in to depth quickly, then back out immediately, as soon as the workpiece has come around once at depth. Don't give chatter a chance to build. Do all the grooves this way, then come back and take a more careful tack when finishing: feed in to a distance say .010 or .020 from bottom depth, and feed the tool right, then feed left, trimming one sidewall at a time. Advance the tool and feed right and left again. At final depth, you won't have much room to jog right and left, but by then, you'll not be trying to remove much material anyways. If necessary, grind the tool to a sharper point so that you can move it .001" left or right when at full depth. You'll need to be concientious about observing the compound dial readings to do all this, and competent at keeping track of backlash in the compound as well, But that will take the hair off your head and put it on your chest, where it counts

Thanks for the suggestions and tips. I am going to give my mill a chance but might be back to the lathe quickly. I haven't been using my compound, just set my pitch using a dial indicator. If I continue with that method I could center my compound and then use that to cut a little off the left and then the right sides. The grooves don't have to be well formed in their bottoms because the belt never gets very deep into the V.

This is all for a Battlebot robot so it's life expectancy is measured in minutes!

[boilerbots]

Pictures of the tool I ground and used on my lathe. It doesn't look so good in the top down picture. It appears that the bottom is wider than the top but I think that is a shadow. I better inspect it closely.

John's post got me thinking so I went out to the garage and dug through my junk and found some cheap fly cutter sets. One set holds the tools at a 20 degree angle, that seems perfect for my 40 degree V, so I ground only one side of the tool at 20 degrees and mounted it in the fly cutter.

I am going to try it out in the mill after I post these pictures.

[John Welden]

Boilerbot,

I'm in no way trying to be mean, but your bit grinding is very crude. Looks like you could use a finer wheel on your grinder. Tool grinding isn't that easy and takes some practice so please don't feel bad if it's not perfect. Take your time, keep the bit cool and get those cutting edges cleaned up nicely.

Make sure your wheel is dressed properly and running true.

Good luck on your battlebot. I'd love to see some pictures when you're done.

[boilerbots]

Yeah, I know my grinding is crap but I think the camera makes it look worse. If I knew what I was doing that would certainly help. But when I was grinding I use my bare hands so I can feel the steel getting hot then I put it in water to cool it back down.

I had dressed the wheel just before I started but I don't have guides for grinding. I set the stand at a slight angle for the relief.

I will certainly post some pictures when finished. Actually the robot is finished and fought a couple of times. We are now working on the Beta version for the upcoming robot games next weekend.

[maz43]

FWIW,
I had a similar problem but on a much larger scale.
I had to cut 1.18 deep v grooves on a 48" diameter part on an old T lathe. The material was pretty hard cast iron.
I ground a profile tool for the job .
I plunged to half the depth, moved the tool in z in both directions leaving .01 per side. I then plunged to full depth and moved side to side in z to finish the width being careful not to dwell more than 1 rev while on the sides.
This approach worked quite well on the old manual lathe T lathe to defeat chatter.

[boilerbots]

Originally Posted by John Welden Good luck on your battlebot. I'd love to see some pictures when you're done.

The website is not finished but if you poke around in the gallery of photos and blog you can see pictures, "Counter Revolution" is my newest bot. That was basically the Alpha version, 100% designed and some testing done in SolidWorks, parts machined in my garage except for the waterjet cutting.

http://robots.boilerbots.com/counter_revolution/index