# Problem machining drill rod



## black85vette (Jan 30, 2010)

I asked this question in another thread but did not get an answer. Thought I might try again.

Was making a cut with a .5 inch mill when things went :toilet:  I had made some cuts on the lathe without a problem.

This is my first experience with drill rod so I thought my end mill was bad. Put on another and it promptly quit cutting also. Just to verify they were bad, I put in some aluminum and both end mills cut really poorly.  More like scraping than cutting.

So I am stuck not wanting to break out another end mill until I have some idea of what happened. I suspect localized work hardening ( even though I have never actually experienced it ) but it could be I just don't know what I am doing. ( much more likely )

Wondering if I need a better end mill? I am open for suggestions before I doom one of my new end mills to a very short life.


----------



## deere_x475guy (Jan 30, 2010)

It's definately work hardening. I have experienced the same with with some pins I am making out of Oil Hardening drill rod. I ended up using carbide fine roughing end mill and mist coolant to solve the problem.


----------



## Bernd (Jan 30, 2010)

You definitely work hardened the steel if you were using HSS end mills and running them at a high RPM.

Best to use carbide. Run at a slower RPM. Coolant not necessary but helps keep things cool. Also a heavier cut will help.

I know your going to ask how much is a heavier cut and what RPM. I usually do it by what the machine is telling me.

Bernd


----------



## gbritnell (Jan 30, 2010)

What rpm were you running the cutter at? I use high speed tooling almost exclusively on drill rod and stainless steel with no trouble. High speed is the worst thing. It doesn't really work harden the material but the heat at the point of contact burns the flutes on the end mill. The heat can be absorbed into the material but not the small surface area of the flutes. 
gbritnell


----------



## black85vette (Jan 30, 2010)

:idea:

OK. The little light bulb is starting to come on now. Sounds like I am running my RPM way to high. I usually run about 1800 to 2000 and make light cuts at moderately low feed rates. What should I be running on an X2?

I may go ahead and order a carbide end mill since I have to replace two end mills anyway.

Do you guys use any cutting oils on drill rod?


----------



## Philjoe5 (Jan 30, 2010)

With a 1/2" end mill on drill rod I doubt if I ever run faster than 400 - 500 rpm. I have a set of end mills that has gone about a year and the 1/2" recently was declared dead - but it's the size I use most often. Hope this helps,

Cheers,
Phil


----------



## Maryak (Jan 30, 2010)

B85V,

I would run a 0.5" HSS end mill in drill rod at around 400 max rpm.

Best Regards
Bob


----------



## Rustkolector (Jan 30, 2010)

I was end milling some 1/2" O1 yesterday cutting some individual cam lobes on the rotary table. I used a 3/8" carbide end mill at 700 RPM. Depth of cut was .200" with a width of cut of .090". My feed rate on the RT was slow to get a good finish. It cut like cast iron. I usually have trouble with the finish on O1, but the carbide made me smile yesterday. I have a light mill/drill and have been trying to find cutters that work better with steel in my light equipment. The improvement I find with carbide on steel has been a pleasant surprise. 
Jeff


----------



## polepenhollow (Jan 31, 2010)

1/2 endmill in O-1, I would use 500 to 600 RPM. Conventional cut @ .050 DOC.
Minimal spindle extension.
 Finish pass at same last number only climb mill.
Use Oil,
Slight drag on cross feed lock.
KL


----------



## Debian (Jan 31, 2010)

Could someone please explain what "drill rod" is? I didn't found it in any dictionary english-italian, for sure a kind of steel but... which? Thanks


----------



## Richard1 (Jan 31, 2010)

Hardenable tool steel. Might be known as Silver Steel (British / Australian) Drill Rod (American) O1 (England and probably rest of world). If in flat sheets then maybe gauge plate or ground flat stock. From the name I guess originally to make carbon steel drills. I'm sure other people on here can tell you more than I can.


----------



## Maryak (Jan 31, 2010)

Debian,

It's a carbon tool steel containing 1.1-1.2% carbon.

In the US it's known as Drill Rod, in the UK it's known as Silver Steel.

Hope this helps.

Best Regards
Bob


----------



## black85vette (Jan 31, 2010)

Debian  said:
			
		

> Could someone please explain what "drill rod" is? I didn't found it in any dictionary english-italian, for sure a kind of steel but... which? Thanks



In addition to the make up of the material it has a couple of characteristics that are useful. It is precision ground to size and it is designed to be hardened. Useful for making cutting tools. You can make reamers and other tools out of it.


----------



## BobWarfield (Jan 31, 2010)

black85vette  said:
			
		

> :idea:
> 
> OK. The little light bulb is starting to come on now. Sounds like I am running my RPM way to high. I usually run about 1800 to 2000 and make light cuts at moderately low feed rates. What should I be running on an X2?
> 
> ...



Yep, way too much rpm. G-Wizard would have you run 400 rpm like the gent said. But just as bad as the rpm is the "moderately low feed rates". Feeding too slowly on any work hardening material is bad news. Depending on depth of cut, G-Wizard would have you feed between 1 and 5 IPM. The latter is a really light cut of 0.015 or less. Before I had CNC I used to convert these numbers to "seconds per handwheel turn" and literally count it off. 

Work hardening is so annoying. I remember being at the drill press one day merrily making holes in some stainless. Got distracted momentarily and stopped feeding, but the bit was still in the hole. That piece had to be scrapped as did the bit!

Cheers,

BW


----------



## black85vette (Jan 31, 2010)

Appreciate all the great tips and info. Everytime I get into unknown territory you guys bail me out! Thanks.  :bow:


----------

