Machining Hard Jaws

[StoneyNH]

The standard height of hard jaws for my Kurt vise is 1.750.They workout better for me if I can remove some material off of them to about 1.730.We don't have a surface grinder here to do it properly.

 

Anyone got any tricks up their sleeve for how to machine them down using something else? I have a couple of face mills with inserts I could use if I knew what inserts would cut those hardened jaws.

 

Im thinkin maybe ceramic or diamond?

[Thad]

Carbide should work just fine.

[StoneyNH]

I have carbide inserts & I cant even take a .005 cut with them,all they do is shoot sparks even with coolant on & they dull quickly.

[chris m]

Interesting. I wouldn't run coolant in that application because of thermal cracking, but i am surprised you can't get the job accomplished

 

I would think high surface speed, high feed, light DOC, and air blast if you have it; call your insert guy and say "WTF?"

[Mr. M]

Guys I used to work with cut the Kurt hard jaws with solid carbide endmills all the time  

I would just take a few passes with something like an SGS Z-Carb with a .03-.06 corner rad.

[Thad]

I was thinking solid carbide end mill, not carbide inserts, though you should be able to cut it with the inserts too.

[Matthew Hajicek - Singularity]

Calculate your feed and speed using something like HFMAdvisor.  If it's sparking it's going too fast, and I agree cut it dry.

[StoneyNH]

OK sounds like Ive been trying to go too fast & use coolant.I haven't done it in awhile but far as I can remember I was using 1-1/4 dia facemill with 2 inserts running about 3800RPM & a FR of 10.

 

So when I get the chance to try it again I'll slow the RPM to 2000 & try a FR of 5. (5 inches per minute). And if it still shoots sparks Ill figure Im still going too fast,so I'll try slowing it down.

 

Thanx

[robgbritt@westpharma]

I was thinking solid carbide end mill, not carbide inserts, though you should be able to cut it with the inserts too.

This would be my approach.  I feel like a sharp carbide EM will give you better results than a facemill.

[Mic6]

I like to keep my tools .01 above my hard jaws when doing vise work, although every once in awhile I'll keep it -.01 and it cuts fine  

[Guyinthedesert]

Are you trying to end mill them? You'll have a whole lot better luck laying them down and side milling them

[StoneyNH]

Well,thats another thing I haven't tried,Ive been milling across the top of them as they would sit secured to the vise.Sounds like another thing to try is hold them vertically on parallels & mill them from the side not the top.That way I could find an endmill with good cutting flutes & maybe chewed up on the corners & use it.Thanx for all the suggestions.

[djstedman]

1500RPM is almost 500SFM for that cutter.. I wouldn't spin it a whole lot faster than that if you ask me.. also.. that feed sounds pretty darned slow I would probably be going at least 10 IPM and probably 15 IPM

 

so 1500 RPM 15 IPM .02 depth air blast.. that's where I would start..  also depends on insert geometry though.. what facemill? what insert?

[jeff]

 

Im thinkin maybe ceramic or diamond?

Definitely NOT diamond.

As others stated above, go with solid carbide, preferably with a decent corner radius.

[BenK]

Use something like a Z-carb with a .030 radius on it would be correct. Speed and feed would be something like 3000 @ 85ipm. .008 step down and 20% step over using a dynamic style facing path will work great. Definitely do not use coolant, only air blast. 

[jlw™]

a 1in 6fl em always works on accident for me...

run it like 13-8 stainless.

 

But seriously, a 1in 5 or 6 flute email with 0.030cr running 0.005ipt and 140sf should handle it.

 

Like I said, it always accidently works for me.

[Guyinthedesert]

a 1in 6fl em always works on accident for me...

run it like 13-8 stainless.

 

But seriously, a 1in 5 or 6 flute email with 0.030cr running 0.005ipt and 140sf should handle it.

 

Like I said, it always accidently works for me.

Seriously?  He could go out and buy a used surface grinder for less than a 1" carbide end mill would cost.

[88Matt]

Geometry is key when hard milling. There are plenty of off the shelf inserts and solid carbide end mills on the market to do this all day long.

What insert holder are you using?

[BenK]

Seriously?  He could go out and buy a used surface grinder for less than a 1" carbide end mill would cost.

 

Who in their right mind would wan't a $200 used up surface grinder? You are far better off learning a new process and bettering your skills than buying some pile of crap surface grinder. An endmill to hard mill can cost you as little as $50 and the experience can be invaluable in the future.

[Guyinthedesert]

I must be buying my tools at the wrong place. Where can you get a 1" 6 fl carbide em for $50?

 

At several recent auctions I've seen decent 6x12 manual surface grinders go for , give or take, $600

[BenK]

I must be buying my tools at the wrong place. Where can you get a 1" 6 fl carbide em for $50?

 

At several recent auctions I've seen decent 6x12 manual surface grinders go for , give or take, $600

 

I wasn't referring to a 1" at that price. Use a .5" endmill with a corner radius. You don't need a 6fl endmill to hardmill. Use any high performance tool for steel and you can get the job done. I'm sure every shop has some slightly used endmills they could use for this. Again it will be cheaper and add valuable experience if you take the time to learn to hardmill.

[Thad]

I'm still trying to figure out why a 1" carbide end mill with 5-6 flutes is required for this job.

[Dave Allen]

I'm just wondering if we had cut the thing yet. .02 off the top of some jaws happens everyday without even trying.  

[88Matt]

I'm still trying to figure out why a 1" carbide end mill with 5-6 flutes is required for this job.

I run this end mill all time; can't wear it out!

[jlw™]

I must be buying my tools at the wrong place. Where can you get a 1" 6 fl carbide em for $50?

 

At several recent auctions I've seen decent 6x12 manual surface grinders go for , give or take, $600

He didn't specifically say a 1 in em, I did. So, buying a used surface grinder, setting it up, Learning to dress the wheel, and then grind a set of jaws is better than buying a $290 em? Let's buy something with its own unique safety concerns and maintenance requirements because an em is pricey. as I recall, he had a milling question and your advice was to buy a wore out grinder. No wonder you can't find $50 endmills. Your not looking.