What's new
What's new

First try on D2 62Rc(video)

jamesu229

Hot Rolled
Joined
Feb 20, 2011
Location
Grant Alabama USA
In an effort to perfect our speeds and feeds while hardmilling, this is the first try. Its not right yet, but far from a failure. I apologize for the language at the end, but I do not edit my videos. The endmill was a reground garr VRX at .353 diameter. Parameters were 750 sfm, .018 radial, .300 axial and .004 ipt.
The next run will be at 650 sfm, .006 ipt using a mist sprayer. Also, any small areas will be blocked off to be ran at lower speeds to allow cooling time for the cutter. Just a note for anyone using a Mag Fadal, The E-stop button is not quick enough, use feed hold. The endmill was badly worn on the corners, but not broken, and will be resharpened and used again.


Hsm on heat treated D2 - YouTube
 

bryan_machine

Diamond
Joined
Jun 16, 2006
Location
Near Seattle
A general question (maybe there's a good thread on this somewhere) - how to decide where flood coolant is and is not a good idea? Is air blast always suitable when flood coolant is not?

It would be nice to see a closeup of the resulting part, if allowed.
 

Orange Vise

Stainless
Joined
Feb 10, 2012
Location
California
A general question (maybe there's a good thread on this somewhere) - how to decide where flood coolant is and is not a good idea? Is air blast always suitable when flood coolant is not?

When milling low carbon or annealed alloy steel, the flood coolant threshold is typically around 300 SFM on an inserted cutter. That's when the cutting edge gets too hot and thermal shock from flood coolant can damage the cutting edge. This threshold lowers as the cutting edge dulls. The threshold can also change significantly depending on material hardness and cutter geometry, so it's best to gage cutting zone temperature by chip color. When chips start changing color from silver to bronze, it's time to turn off the coolant. When chips are blue/purple, it's just about guaranteed that flood coolant will damage the carbide.

Fresh, solid carbide endmills with HSM toolpaths can cut much faster than 300SFM without generating much heat, but most folks will crank up the speed and turn off the coolant anyway. High feed mills also generate less heat.

Air blast is optional. Its primary purpose is clear chips to prevent recutting. During long, dry cycles, air blast can also significantly cool the toolholder body. We machine hardened materials on a regular basis and air blast will keep the toolholders around 100 degrees F, compared to 150+ without the air blast. Good for the spindle and good for holding tolerance. Makes no difference to cutter life, however.

-Sol
 

jamesu229

Hot Rolled
Joined
Feb 20, 2011
Location
Grant Alabama USA
I agree with Orange vise up until the part about air blast not helping cutter life. Maybe tis is due to how fast we generally run. The coating on the endmills used in my videos is heat tolerant, not heat activated, so any temp drop is welcomed. Even the fan effect of the cutter spinning at high rpm helps. A mist sprayer used with the cutter in this video may only lower the running temp by a hundred or so degrees, but that will allow extended engagement time without overheating. This also helps with TiAln coatings.
 

Dave K

Diamond
Joined
Mar 21, 2004
Location
Waukesha, WI
I gotta ask, even though this is a rookie question when it comes to high speed machining like this. If the material is heat treated D2, are these standard off the shelf endmills you use for something like this? Is it a special type of carbide that allows this much sparking off the cutter? Is it the coating, tool grind geometry?

And if heat treated tool steels can be cut at this type of feed and speed, then can't soft cold roll steel be cut even faster? Frankly, I've seen this before but never attempt to try this type of cutting myself unless I'm on aluminum.

I too, would have liked to have seen the finished product of that run.
 

jamesu229

Hot Rolled
Joined
Feb 20, 2011
Location
Grant Alabama USA
I gotta ask, even though this is a rookie question when it comes to high speed machining like this. If the material is heat treated D2, are these standard off the shelf endmills you use for something like this? Is it a special type of carbide that allows this much sparking off the cutter? Is it the coating, tool grind geometry?

And if heat treated tool steels can be cut at this type of feed and speed, then can't soft cold roll steel be cut even faster? Frankly, I've seen this before but never attempt to try this type of cutting myself unless I'm on aluminum.

I too, would have liked to have seen the finished product of that run.


The basic endmill is common, just C4 carbide. The grind and coating is what makes the difference. Othe materials are machined like this on a regular basis, only larger cuts and faster. It will be two weeks befofe I get back to where I left the block, but it was ( D 2) machined in block letters. It did not finish the inside of the D because of my programming error. I'm not sure the endmill could have entered the cut, the corners were in bad shape. I am working on this because ceramic cutters arent always the best way to machine intricate details.
 

zero_divide

Stainless
Joined
Feb 2, 2012
Location
Toronto
Sure beats grinding.
How many parts (estimate) with one end mill?

Buck

Lol, one!
Seriously though I bet if you reduce the speed a bit it could help with tool life a lot.
For hard stuff like that AlTin nano-coating works pretty good.

Imo when I see sparks it generally means "slow down"
I have machined 60rc D2 before at half the speed and no sparks.
Not sure how it would affect the cutter life though -only ran for 2minutes or so.
 

jamesu229

Hot Rolled
Joined
Feb 20, 2011
Location
Grant Alabama USA
Sure beats grinding.
How many parts (estimate) with one end mill?

Buck

I am trying to get 15 minutes actual "in cut time" at this speed, or as Zero said, twice as long at 50% of what I was doing here. Also in his post he said 2 minutes, this had around 6 without breaking. A 1/2" would have done better in this situation because of its thicker core absorbing the heat slower. As mentioned, it beats grinding. This regrind cost $17.22 delivered. I will have this worked out before the end of the year. The next run will have a koolmist sprayer and just a bit less sfm, higher feed. I will probably use a 1/2" also.
 

Smrtman5

Cast Iron
Joined
Apr 15, 2011
Location
NJ, USA
What kind of thought process goes into grinding a cutting tool like this? Do you start with a standard set of angles and reliefs and then make adjustments from there?

If so, what factors would allow you better tool life, or faster cutting speeds?

Im sure its heavily dependent on what material is being cut, but maybe there are some generalizations?
 

zero_divide

Stainless
Joined
Feb 2, 2012
Location
Toronto
I am trying to get 15 minutes actual "in cut time" at this speed, or as Zero said, twice as long at 50% of what I was doing here. Also in his post he said 2 minutes, this had around 6 without breaking. A 1/2" would have done better in this situation because of its thicker core absorbing the heat slower. As mentioned, it beats grinding. This regrind cost $17.22 delivered. I will have this worked out before the end of the year. The next run will have a koolmist sprayer and just a bit less sfm, higher feed. I will probably use a 1/2" also.

We often machine 50-55RC tool steel dry.
At 150 SFM we get 1 hour of tool life slotting.

In your HSM application i bet 10$ your tool will survive for at least an hour at 350 SFM

We don't bother with regrinds so our target is usually at least an hour.
 

jdj

Diamond
Joined
Oct 22, 2007
Location
detroit,mich.
Imo when I see sparks it generally means "slow down"
I have machined 60rc D2 before at half the speed and no sparks.


When you get to machining 58Rc and over, hard steel, at higher speeds, the small chips incinerate in the air. It isn't QUITE the same type of spark as if a dull tool was cutting/rubbing. When turning hardened steel, it sometimes appears that a fountain of fire is coming off the tool/part interface. D.O.C. plays a big part (among other things!) in these unusual situations.
 

jamesu229

Hot Rolled
Joined
Feb 20, 2011
Location
Grant Alabama USA
A general question (maybe there's a good thread on this somewhere) - how to decide where flood coolant is and is not a good idea? Is air blast always suitable when flood coolant is not?

It would be nice to see a closeup of the resulting part, if allowed.


Heres a picture of the part. I have made the needed modifications to the endmill and tool path that should give the results I'm looking for. The new parameters are 650 sfm , .015 radial and .010 ipt. All small areas are blocked off, and will be machined at the end of the program using 350 sfm at .015 z steps at .004 ipt. The customer that asked me do develop this cutter/path was very pleased with the initial results and will be using them quite often after a successful run.





D2.jpg
 

zero_divide

Stainless
Joined
Feb 2, 2012
Location
Toronto
Heres a picture of the part. I have made the needed modifications to the endmill and tool path that should give the results I'm looking for. The new parameters are 650 sfm , .015 radial and .010 ipt. All small areas are blocked off, and will be machined at the end of the program using 350 sfm at .015 z steps at .004 ipt. The customer that asked me do develop this cutter/path was very pleased with the initial results and will be using them quite often after a successful run.





View attachment 87723
0.01 ipt!
Wow 0.004 ipt for slotting seems like alot.
Do you have some sort of radius on the corners?

Becase i dont see how it will not chip.
 

jamesu229

Hot Rolled
Joined
Feb 20, 2011
Location
Grant Alabama USA
.004 ipt should be no problem. The end grind I chose is basically a modified feed mill. I understand 30Rc is very different, but using a 3/4 endmill with my normal grind, I can face at .015 deep, 7500 rpm and 175 ipm, reliably. The new end grind is much tougher. I have 3 prototype cutters and plenty of material to play with. DLC coating with a protective outer coating is also an option, as $75 is the customers upper limit for a 1/2 that will run at the rates we are looking at. The endmill in the video was under $20, and I want to keep the cost low like this, better for business.
 

Dave K

Diamond
Joined
Mar 21, 2004
Location
Waukesha, WI
I understand 30Rc is very different, but using a 3/4 endmill with my normal grind, I can face at .015 deep, 7500 rpm and 175 ipm, reliably.

Am I reading this correctly? That's about a 1470 SFM. With a normal ground endmill, this is the speed you run on D2?
 

jdj

Diamond
Joined
Oct 22, 2007
Location
detroit,mich.
Am I reading this correctly? That's about a 1470 SFM. With a normal ground endmill, this is the speed you run on D2?


Soft D2 isn't as bad as some people make it out to be. You have a point however! That is pretty damn fast. I am guessing that the grind is Jamesu229's, NOT regular. The low D.O.C. also helps.
 








 
Top