Sign in to follow this  
parallax7761@comcast.net

Does High Feed Tooling generate more heat?

Recommended Posts

Hi guys, I am about to cut a 17-4 ph part, condition hr1150. It has a few tab/tang arms that are about .25 thick about 3/4 long. I want to make sure not to put any unnecessary heat in the part while cutting. I was going to us a 2" Mitsubish AJX high feed but I am not sure if it will heat the material any more traditional cutters like the apx3000. I have used the AJX before but it was on a part that had no potential for tweaking and stressing. Please let me know what you all think.

Share this post


Link to post
Share on other sites
26 minutes ago, [email protected] said:

Hi guys, I am about to cut a 17-4 ph part, condition hr1150. It has a few tab/tang arms that are about .25 thick about 3/4 long. I want to make sure not to put any unnecessary heat in the part while cutting. I was going to us a 2" Mitsubish AJX high feed but I am not sure if it will heat the material any more traditional cutters like the apx3000. I have used the AJX before but it was on a part that had no potential for tweaking and stressing. Please let me know what you all think.

Do you have external/internal Air Blast?

I love high-feed cutters specifically because they put the heat into the chip, not the tool or work-piece, when run correctly.

  • Thanks 1

Share this post


Link to post
Share on other sites

I think one of our machines has air blast or we can rig one up if we don't. I have done that in that past with these cutters when you need to evacuate chips from pockets. Thanks, I knew the most of the heat went in chip due to it's color...but I couldn't remember if the workpiece was any hotter with the negative rake of a high feed vs positive rake of a tradition insert cutter

Share this post


Link to post
Share on other sites

Heat not normally, but depending how thin you are making the floors could be. My main worry with highfeed is stress unless they are a high shear type of tool which is rare in 17-4 grades of inserts.

Let me explain my thoughts behind that statement. Metal is really like dirty just highly compacted and more dense. I teach people the differences between Positive, Neutral and Negative tooling it the following example. For a neutral tool take a Shovel and put in 90 degrees into the ground and pull it forward. Watch how the dirty in front of the shovel is broken up. In softer dirty verses clay you see a big differences. For a Negative tool do the same thing but at 45 degree angle backwards to the 90 degree then try to drag or push it around to remove the dirt. Watch how the soil is broken up from that point. Then for a Positive tool put the shovel at 10-15 degree angle to the soil and take smaller depth and see how the soil breaks up. Metal is not different in my opinion. Yes it is a shallow cut with a highfeed, but the earth around it still responds different to each of the 3 approaches to remove material depending on the rake of the tool. The thinner the area coming up to a bottom the more of a risk that the transfer of the process effects the backside. These different ways the earth handles this again to me is similar to the way metal reacts to being cut. Just cut a 2" thick piece of 17-4 removing 60% of the material from one side leaving .5 thick floors. The part was flipped over and it only moved .005 across 25" length of Material, if we roughed it with a Highfeed verses the 5 Flute I think it we would have seen as much as .06 movement. 

In 17-4 I am finding 5 flute endmills are doing a better job roughing to not put more stress into the Material. With 17-4 the high feed inserts are not normally high shear they are honed edges with some negative to neutral edge contact with the material. Now if roughing sending out of heat treat to then come back and finish no worries, but in 1150 condition it is already harder than annealed. Being that thin I would stay away from a high feed inserted tool just because how thin will the floor be when done. Might look to the solid carbide style tools that are high feed if dead set on using one they seems to be a little more positive on the cutting edge. Without knowing what the final part looks like and many other possible trappings hard to say what is the best method here. Where I will test the process and see if it yields the results I want. If it works and is reasonable for a runtime making a good quality part that is repeatable then I roll with it. If not then I backup and rethink the process to not only have a good run time, but also make the best part possible. Sometimes you cannot get in a hurry and have to accept the right balance of speed to feed to make the process repeatable and best quality part. If running one off then I would use a 5 flute endmill to rough it using a start hole or a ramp that is going to not hurt the tool feeding down to depth and call it a day.

  • Thanks 1
  • Like 4

Share this post


Link to post
Share on other sites

i just finished machining some parts with that same material. (.312" thick)  Tried using a 6 flute and warped my part about .010".  Then tried using a high feed cutter and it warped about .007. 

Played around with speeds and feeds on the High Feed Cutter and got it to warp only .003. The only issue was tool life.

I ended up running it dry with no air and was able to finish the job and inserts still look good. :) it was only 35 pcs. :)

 

  • Like 3

Share this post


Link to post
Share on other sites
1 hour ago, cncchristalsco said:

i just finished machining some parts with that same material. (.312" thick)  Tried using a 6 flute and warped my part about .010".  Then tried using a high feed cutter and it warped about .007. 

Played around with speeds and feeds on the High Feed Cutter and got it to warp only .003. The only issue was tool life.

I ended up running it dry with no air and was able to finish the job and inserts still look good. :) it was only 35 pcs. :)

 

Great feedback gives me something to think about. I really appreciate you putting that up. Are you willing to share your speeds and feeds with tool that worked for you?

Share this post


Link to post
Share on other sites

Sure Ron, the following cutting parameters worked for me at least.....

i was using the Kyocera MFH Raptor High Feed Cutter. 

1.250" in diameter / 5 cutting inserts / Grade PR1535. 

SFM 390 = 1191 Spindle Speed

IPT .0169 = 100.00 Feed rate

DOC = .020"

WOC = 80% = 1.000"

No coolant

 

  • Like 2

Share this post


Link to post
Share on other sites
20 hours ago, crazy^millman said:

Heat not normally, but depending how thin you are making the floors could be. My main worry with highfeed is stress unless they are a high shear type of tool which is rare in 17-4 grades of inserts.

Let me explain my thoughts behind that statement. Metal is really like dirty just highly compacted and more dense. I teach people the differences between Positive, Neutral and Negative tooling it the following example. For a neutral tool take a Shovel and put in 90 degrees into the ground and pull it forward. Watch how the dirty in front of the shovel is broken up. In softer dirty verses clay you see a big differences. For a Negative tool do the same thing but at 45 degree angle backwards to the 90 degree then try to drag or push it around to remove the dirt. Watch how the soil is broken up from that point. Then for a Positive tool put the shovel at 10-15 degree angle to the soil and take smaller depth and see how the soil breaks up. Metal is not different in my opinion. Yes it is a shallow cut with a highfeed, but the earth around it still responds different to each of the 3 approaches to remove material depending on the rake of the tool. The thinner the area coming up to a bottom the more of a risk that the transfer of the process effects the backside. These different ways the earth handles this again to me is similar to the way metal reacts to being cut. Just cut a 2" thick piece of 17-4 removing 60% of the material from one side leaving .5 thick floors. The part was flipped over and it only moved .005 across 25" length of Material, if we roughed it with a Highfeed verses the 5 Flute I think it we would have seen as much as .06 movement. 

In 17-4 I am finding 5 flute endmills are doing a better job roughing to not put more stress into the Material. With 17-4 the high feed inserts are not normally high shear they are honed edges with some negative to neutral edge contact with the material. Now if roughing sending out of heat treat to then come back and finish no worries, but in 1150 condition it is already harder than annealed. Being that thin I would stay away from a high feed inserted tool just because how thin will the floor be when done. Might look to the solid carbide style tools that are high feed if dead set on using one they seems to be a little more positive on the cutting edge. Without knowing what the final part looks like and many other possible trappings hard to say what is the best method here. Where I will test the process and see if it yields the results I want. If it works and is reasonable for a runtime making a good quality part that is repeatable then I roll with it. If not then I backup and rethink the process to not only have a good run time, but also make the best part possible. Sometimes you cannot get in a hurry and have to accept the right balance of speed to feed to make the process repeatable and best quality part. If running one off then I would use a 5 flute endmill to rough it using a start hole or a ramp that is going to not hurt the tool feeding down to depth and call it a day.

I was told once "metal is plastic" also true in it's way but I like the dirt analogy!!

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now
Sign in to follow this  

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us