# facing hard metals like lathe toolholders, how to do it?



## unterhausen (Dec 1, 2009)

This is a basic question, but I figure I'm not the only person who would like to know. I'd like someone to walk me through machining 1/8" off the top of a 3/4x3/4" lathe toolholder. The machinist at work suggested I get a 5 flute (or more) end mill and he was muttering something about coatings. I don't like to press him for too much info since I'm not paying him. What size end mill should I get? Do I just run it in a lawnmower pattern? If I'm running a cnc, should I climb mill? 

Are there any good books that answer questions like this?


----------



## 65535 (Dec 1, 2009)

A lot of it depends on the machine you have. Lots of guys here use index able endmills with good carbide inserts.


----------



## precisionworks (Dec 1, 2009)

> I'd like someone to walk me through machining 1/8" off the top of a 3/4x3/4" lathe toolholder.


Surface grinder would be my first choice 

Lathe insert holders are generally really hard, especially Iscar, Valenite, Kenna, Sandvik, etc. If using solid carbide tooling, run the largest 4-flute end mill that your machine will take - usually 3/4", but a 1" end mill is stronger if you have an ER-40 collet chuck. 200 sfpm is plenty fast. Set DOC and feed where they feel right & sound right for your machine ... this is not a really fast process. Although you can take all .125" off at one, a pair of passes at .0625" are easier on the machine & on the nerves.

An indexable face mill (or indexable end mill) is perfect for this use, as replacing a few chipped inserts is a lot cheaper than replacing a 3/4" or 1" solid carbide end mill. This is not the time to use a high shear or free cutting tool, but better to use an insert that is close to unbreakable. If you have a tool that runs CNMG's, they work well. As do most negative rake milling inserts.

My "go to" choice of inserts is a CNMG-432 or CNMG-433 in cermet. EBay was good to me a few years ago & provided 100 CNMG-432 made in USA cermets ... at the grand price of $50 

If you don't have or cannot find cermets in the shape you need, an insert made to run tough materials can also work. Most of the lathe insert holders are at least 50 HrC, and tough as nails.

Some people have great success with solid carbide end mills, but it makes me cry when I break a $100 end mill of a $20 eBay holder :nana:


----------



## unterhausen (Dec 2, 2009)

precisionworks said:


> Surface grinder would be my first choice


So can I put it in a 4-jaw and use my toolpost grinder? I spent most of the day trying to get my mill to run with only frustration, so maybe this isn't going to work out. I guess I should look at the 3/4" BXA tool holders


----------



## 65535 (Dec 2, 2009)

unterhausen said:


> So can I put it in a 4-jaw and use my toolpost grinder?



I'm sure there's a way that could work, but it would be far from recommended.

A surface grinder is a completely separate machine, basically a precision grinding wheel on a mill style table that moves.


----------



## precisionworks (Dec 2, 2009)

> can I put it in a 4-jaw and use my toolpost grinder?


A TP grinder is mostly used for ID or OD finishing on round stock - I don't see how the bottom surface of the insert holder could be presented to the TP grinder stone.

This might be a good time to look at an indexable face mill with R-8 shank. Mine see frequent use on a variety of work, so much so that the solid carbide end mills don't get used nearly as much as before. Dorian makes a 2" face mill that takes the CNMG-4xx insert, and Euro and Asian copies are available - the Euro copies being pretty nice.







What makes this face mill neat is that it recycles CNMG inserts. When a CNMG insert is used on a lathe toolholder (like a MCLN), it uses the 80-degree tip. When placed in the face mill the 100-degree tip is used, allowing you to cut with the remaining four edges. Nothing much better than free inserts :nana:

Shars sells an imported 2" face mill that uses the APKT-1604 insert. These are thick & tough and will do a nice job on your lathe holder. Don't have any idea about the quality, etc., but the price is low:

http://www.shars.com/products/view/7859/2quot_90_degree_Face_Mill_APKT_Insert


----------



## StrikerDown (Dec 2, 2009)

precisionworks said:


> This might be a good time to look at an indexable face mill with R-8 shank. Mine see frequent use on a variety of work, so much so that the solid carbide end mills don't get used nearly as much as before. Dorian makes a 2" face mill that takes the CNMG-4xx insert, and Euro and Asian copies are available - the Euro copies being pretty nice.
> 
> What makes this face mill neat is that it recycles CNMG inserts. When a CNMG insert is used on a lathe toolholder (like a MCLN), it uses the 80-degree tip. When placed in the face mill the 100-degree tip is used, allowing you to cut with the remaining four edges. Nothing much better than free inserts :nana:



I really like the idea of re-using the CNMG inserts. Do you have a recommendation for a good place to get the Euro copies? I have another 1" tool holder to mill down and the last one was a little hard on the end mill... one chip on one flute


----------



## wquiles (Dec 2, 2009)

precisionworks said:


> ... 200 sfpm is plenty fast. Set DOC and feed where they feel right & sound right for your machine ... this is not a really fast process. Although you can take all .125" off at one, a pair of passes at .0625" are easier on the machine & on the nerves...


This is exactly where the VFD in my mill really shined, the first time I used the mill after the conversion - the ability to instantly vary/adjust the speed to match the job should not be overlooked as a primary reason to get a VFD. When I was creating the 1" BXA tool holder I adjusted the speed of the 1" two-insert end mill (on ER40 collet) just like you said above (I was taking 0.050" passes myself) to find a "sweet spot" or range where it was cutting well with the least vibration/noise. Then when I moved to the cobalt 3/4" end mill for cleaning up the cuts, it was just as easy to pick up a faster speed appropriate for the light cutting that was needed, and then just as easily to pick up a good lower speed for drilling/tapping the set-screw holes. I can't wait to add the VFD to the lathe now!


----------



## precisionworks (Dec 2, 2009)

> a good place to get the Euro copies?


I wish there was a good source, Ray. Dorian still sells the original version, at a price premium. There was an eBay seller who had a few with Weldon shanks, problem being that a Weldon shank reduces collet to shank contact by about 30% (the same area lost to the flats & edges). 

The APKT-1604 face mills & end mills are a good alternative. Vic @ Rani Tool has inexpensive inserts ... $4 each.


----------



## unterhausen (Dec 2, 2009)

precisionworks said:


> A TP grinder is mostly used for ID or OD finishing on round stock - I don't see how the bottom surface of the insert holder could be presented to the TP grinder stone.


you have no imagination  I was thinking I could take the material off the top, the bottom gets referenced to the toolholder. Not sure if that would get me low enough to get to the center of the spindle though.

I have a cnc Bridgeport Series II. Thought I was going to get the new control working, but setup problems ended up today with smoke coming out of the serial port on one of my drives. What a nightmare. Switching drives tonight I guess.

I like the idea of recycling old inserts too. I'd need a straight shank, I have 30 taper tooling.


----------



## precisionworks (Dec 2, 2009)

Another way to go at it is to mount the holder in the lathe 4-jaw with the bottom of the holder facing the tailstock. The surface to be machined will have to be at least .125" proud of the jaws, probably another .062" or so, around .200" sticking out in the wind. Center the part of the shank to be faced so that the insert support is off center. You may need to add a balance weight opposite the insert support. Face as you would any unbalanced part 

If you have any negative rake lathe tooling, this is a great time to use it.


----------



## StrikerDown (Dec 2, 2009)

precisionworks said:


> I wish there was a good source, Ray. Dorian still sells the original version, at a price premium. There was an eBay seller who had a few with Weldon shanks, problem being that a Weldon shank reduces collet to shank contact by about 30% (the same area lost to the flats & edges).
> 
> The APKT-1604 face mills & end mills are a good alternative. Vic @ Rani Tool has inexpensive inserts ... $4 each.



Thanks Barry,

I remember that tool with the Weldon shank, maybe I should have bought it.

What do you think of these from Shars?
Too cheap? 
Is this 15 deg positive Rake going to be a problemfor hard milling?

http://cgi.ebay.com/2-R8-CARBIDE-IN...emQQptZLH_DefaultDomain_0?hash=item45eed75f23


----------



## precisionworks (Dec 2, 2009)

> What do you think of these from Shars?


Using part of a screw head for insert retention is not the best method in the world. If you keep looking, you'll probably find something that uses inserts secured by a Torx screw that goes through the center of the insert & pulls the insert tightly into the pocket. That is a much better mechanical solution.



> Is this 15 deg positive Rake going to be a problem for hard milling?


It depends on the insert. I believe the CNMG face mill also presents the insert at 15 deg positive, even though the insert itself is sloped "downward" when used on a lathe (negative rake). Some inserts are really tough to break, like the CNMG and the APKT-1604. Look for something along those lines & it should work fine on the hardest machinable materials, especially if you switch to cermets whenever the material is over 40 HrC. Cermets will allow hard milling to around 62 HrC.


----------



## wquiles (Dec 2, 2009)

Would this be too big (diameter-wise) for your setup?

Ebay link ...


How about this one:
another link from Ebay ...


Or this one without flats?
yet another link from E???? ...


----------



## precisionworks (Dec 2, 2009)

> Or this one without flats?


Okay, Mexico has a lock of great tequila, superb beers, awesome foods, but machine tooling??? :nana:

If that end mill works half a good as it looks, it is a screaming bargain at $50. It would be my first choice, because of the three APKT-1604 inserts. That shape & style is built like a brick house. Any insert can be destroyed, but you have to work twice as hard to kill the APKT-1604 

Quite a few makers are starting to offer that insert for aluminum as well.


----------



## StrikerDown (Dec 3, 2009)

I don't have larger than 3/4" shank capability. How big does your ER 40 collets go up to? 1" or so?


----------



## PEU (Dec 3, 2009)

ER40 collets go from 1/8" to 1"


Pablo


----------



## StrikerDown (Dec 3, 2009)

The 3/4" end mill Will showed uses an APXT insert. Do you know if this is similar and/or interchangeable with APKT? 

Maybe it is a typo!

http://cgi.ebay.com/NEW-BISON-3-4-I...QQptZBI_Tool_Work_Holding?hash=item5884a21143


----------



## unterhausen (Dec 7, 2009)

just to put some closure on this, I milled the slot in the toolholder out with a 5 flute endmill. No drama. Phase II doesn't seem to be too concerned with how square those surfaces are.


----------

