Thread: Poly V cutting, who makes a good tool?

We are turning some aluminum pulleys for 6 groove serpentine. We are using an iscar insert ($38ea) and we have to take off the Ti coating on them so they wont gum up on the grooves in aluminum. We had to have a special holder made for the Iscar inserts to amke sure they have a better angle but yet we are getting chatter. We have tried 50SF and .002 and we have tried up to 800SF and .010 and we still get noticable chatter. Who makes a GOOD poly V cutter for aluminum?

Any help ?

http://www.toolflo.com/cats/Automotive.pdf

Originally Posted by Limy Sami

Any help ?

http://www.toolflo.com/cats/Automotive.pdf

That's what I use. Buy them thru Bass Tool in Houston.

Thought;- If you're plunging straight in at 90deg to axis the likelehood of chatter is increased , try feeding at 1/2 deg under 1/2 of the included angle, - just like screwcutting.

I'd give PH Horn a shout:

http://www.hornusa.com/company/

Best,
Steve

When i was using Iscar they had an ic20 grade that was ground on the
top. It worked well with aluminum.

Iscar reppage has sucked sucked sucked in out area (MN). Our tool rep couldnt even get a return phone call those guys have proven themselves incompetant to our business. They used to be good but the other rep now works for Allied which now has a great influence on our surface footage I dont know if you could give me any Iscar lathe tooling right now I am so upset about their service. Their mill tooling rocks but the service blows goats. As you guys can probly tell this is a very personal issue with me right now. I will call the Houston outfit in the morning.

Originally Posted by alphonso

That's what I use. Buy them thru Bass Tool in Houston.

How do you use the insers what surface footage and what chip load do you use on aluminum? We are talking 3" to 6.75"

I second the toolflo tools. I have used them in the past. I used the 3 tooth ones and the 4 tooth ones both. Larger sizes if I recall. You may need to plunge on an angle to reduce cutting force. That is what I did anyway. Though I was cutting gray iron, and not aluminum. But the AL should be much much easier.


Husker

Originally Posted by IAMATT

How do you use the insers what surface footage and what chip load do you use on aluminum? We are talking 3" to 6.75"

Plunge straight in. 1500 sfm. .004 ipr. 2 to 14 inch diameters.

FLV 3RJ AT50 (steel) GP25, DX200 (non ferrous)

I use a 35 deg diamond insert in a neutral holder to cut poly v grooves. The grooves are a 40 deg angle so you can just profile the pulley. I have al specific inserts from seco and they do a great job. I rough and finish with one tool, and the insert lasts a long time in 6061. I don't think the cycle time would be as fast as with a form type tool but I bet the finish and chip control is better with the single insert. You probably need cam to program the profile. Speed is what you would normaly use to turn al with carbide. Feed is .004 ipr. The best part is I can turn any profile poly v with the same insert.

The insert I'm using is a SECO VCGT331F-AL KX in a SVVBN123 holder if your interested.

Here is a pic of a custom 12 rib multi vee pulley I made for a procharger. It's 2.8" dia. The stocker is the black pulley.

http://s445.photobucket.com/albums/q...werpulley1.jpg

Good luck.