Need help on this tool

[jean]

Need some help on using this 6 FLT carbide EM to machine some 1018 for tooling purpose. Getting A lot of chatter. I’ve used the parameters given but the tool is not even close in performance. It asks for 450-500 SFM and chip load at .069 which is absurd I think.

Brand: Monster

Part Number: 292-401243

Radial step over: 5%

Full depth cut

Tool path used: 3D High Speed (Dynamic Opti Rough)

Tool projection: 2.8”

Holder projection: 2.4”

Coolant: yes

 

[crazy^millman]

22 minutes ago, jean said:

Need some help on using this 6 FLT carbide EM to machine some 1018 for tooling purpose. Getting A lot of chatter. I’ve used the parameters given but the tool is not even close in performance. It asks for 450-500 SFM and chip load at .069 which is absurd I think.

Brand: Monster

Part Number: 292-401243

Radial step over: 5%

Full depth cut

Tool path used: 3D High Speed (Dynamic Opti Rough)

Tool projection: 2.8”

Holder projection: 2.4”

Coolant: yes

 

I looked up the tool. I see .0042 per rev in 10XX material, but with a 2" LOC you are 4 X D not something I normally try in Steel. I will go with a Stub flute relieved shank if I need to cut that deep and would cut that in 4 depths. Cutting that that much in one depth is asking a lot. According to HSM advisor at those speeds and feed with that cut you are at .0043 deflection. Might try adjust the SFM down to find the sweet spot to get rid of the harmonics that are happening doing what you are doing.

[GoetzInd]

I find milling with that much length engaged is also pretty risky as far as tool pullout goes. Even with shrink fit and powergrip. 

 

MIke 

[motor-vater]

I make cuts like that often, but the sfm seems highand there are multiple things to consider, first your holder, I would use a hydraulic then a shrink fit, never a Weldon. They recommend the high chip load because the radial depth of cut is so light. So it takes into account Radial chip thinning..  That being said. I would still start some where around 360 sfm, chip load I would just set it at .002 or .003 and turn on the chip thinning option in your tool tab (RCTF).

Next in your cut parameters you want to make sure you are not forcing this the tool into tight spots, you do that by setting your minimum toolpath radius to like 15%. 

And finally most of these tools do not do well with 3d step ups, like Opti rough, they are designed to be full depth cutters as soon as they are not using the full length of the flute, harmonics will start to happen. I use these tools for material removal then go to a shorter or reduced neck tool for step ups... This is just my opinion as I am not a tool rep, just someone that removes metal everyday... Good Luck

 

[huskermcdoogle]

You are way too slow for that radial engagement.

Not that I want to help a competitor sell tools...  I would do as follows.  If this is in a 50 Taper with a good setup, run full depth by all means.  If this is a 40 taper, you have too many points of contact for full depth.  But if you back it down to 1.625" depth or less, but not less than 1", you will find success.

Keep the 5% stepover for now.

I'd run 1000SFM, .0112fpt.  This takes into account chip thinning and speed factor based on the light radial.

5093 RPM, 341 IPM.  Feel free to back off the feed a little bit if the machine can't keep up, but I would go no slower on the feed than about 200.  If it burns up try to maintain the chipload, but reduce the surface footage.  Air blast would be better than coolant, but coolant would be ok if you can't get the chips away from the cutter.  I'd prefer dry if you don't have a chip evacuation issue.  A little heat will help you as long as you aren't re-cutting chips.

I would consider the above parameters middle of the road for our tools.  The fact that you have chatter is likely a function of machine stiffness.  Your original parameters show 6 points of contact, which IMHO for almost any 40 taper is way way too much.  3-4 points is better and should work on even on a medium quality machine

17 hours ago, crazy^millman said:

but with a 2" LOC you are 4 X D not something I normally try in Steel.

Nothing wrong with 4 or 5xd in steel.  Many people do it everyday.  But quality holders, setups and machines become very important very fast.  As I mentioned earlier, I likely wouldn't be doing that in a 40 taper with a 3/4" tool.  If you needed to, I would use a tool with a tapered core and maybe drop a flute or two to keep the contact points / force down.

My favorite 5xd tool is the Kennametal Harvi II long.  Never had trouble getting it to work.  I've run it in anything from alloy steel to Inconel with very good results.  One notable success was in Inconel 718, similar depths to what you are doing now, in a 40 taper, taking about .010 stepover.  We had a little springing, but that was from the setup as we were cutting on a weak trunnion table.

Husker

 

[So not a Guru]

1 hour ago, motor-vater said:

and turn on the chip thinning option in your tool tab (RCTF).

I never noticed this before. What exactly does it do?

[motor-vater]

1 hour ago, huskermcdoogle said:

You are way too slow for that radial engagement.

Not that I want to help a competitor sell tools...  I would do as follows.  If this is in a 50 Taper with a good setup, run full depth by all means.  If this is a 40 taper, you have too many points of contact for full depth.  But if you back it down to 1.625" depth or less, but not less than 1", you will find success.

Keep the 5% stepover for now.

I'd run 1000SFM, .0112fpt.  This takes into account chip thinning and speed factor based on the light radial.

5093 RPM, 341 IPM.  Feel free to back off the feed a little bit if the machine can't keep up, but I would go no slower on the feed than about 200.  If it burns up try to maintain the chipload, but reduce the surface footage.  Air blast would be better than coolant, but coolant would be ok if you can't get the chips away from the cutter.  I'd prefer dry if you don't have a chip evacuation issue.  A little heat will help you as long as you aren't re-cutting chips.

I would consider the above parameters middle of the road for our tools.  The fact that you have chatter is likely a function of machine stiffness.  Your original parameters show 6 points of contact, which IMHO for almost any 40 taper is way way too much.  3-4 points is better and should work on even on a medium quality machine

Nothing wrong with 4 or 5xd in steel.  Many people do it everyday.  But quality holders, setups and machines become very important very fast.  As I mentioned earlier, I likely wouldn't be doing that in a 40 taper with a 3/4" tool.  If you needed to, I would use a tool with a tapered core and maybe drop a flute or two to keep the contact points / force down.

My favorite 5xd tool is the Kennametal Harvi II long.  Never had trouble getting it to work.  I've run it in anything from alloy steel to Inconel with very good results.  One notable success was in Inconel 718, similar depths to what you are doing now, in a 40 taper, taking about .010 stepover.  We had a little springing, but that was from the setup as we were cutting on a weak trunnion table.

Husker

 

OP please report back after trying this, I would love be get some feed back, I feel like I need some Midal and a maxi pad after hearing Huskers input..... Let that baby eat!!!!

[motor-vater]

1 hour ago, So not a Guru said:

I never noticed this before. What exactly does it do?

IT CALCULATES THE RADIAL CHIP THINNING FOR YOU. A lot of the high end tool manufactures give u recommendations with RCTF already built into the recipe, but I like the little button. If you change step over, it changes feed rate as you do it. Play with it and see what I'm talking about.

 But I'm apparently a Sissy so there is that... LOL in my defense most of the machines I run and the window size I work in, the machine would never reach those feeds. I have programmed many aluminum parts and ran it at 100 200 and 500 ipm, and seen no reduction in cycle time "at the machine" from 200 to 500. It just can never get there on small moves. Ive always felt most of us are just lying to ourselves when we try to program those feeds. But without a doubt their are plenty of machines out there capable Ive just never had one... 

[So not a Guru]

2 minutes ago, motor-vater said:

IT CALCULATES THE RADIAL CHIP THINNING FOR YOU. A lot of the high end tool manufactures give u recommendations with RCTF already built into the recipe, but I like the little button. If you change step over it changes feed rate as you do it. Play with it and see what I'm talking about, But I'm apparently a Sissy so there is that... LOL in my defense most of the machines I run with the window size I work in the machine would never reach those feeds. I have programmed many aluminum parts and ran it at 100 200 and 500 ipm, seen know reduction in cycle time at the machine from 200 to 500. It just can never get there on small moves. Ive always felt most of us are just lying to ourselves when we try to program those feeds. But without a doubt their are plenty of machines out there capable Ive just never had one... 

Hmm. Well, I usually use the tool mfg recommendations, at least to start at. But we have a titanium job we're running right now, that is 48 hours (according to MC, it will undoubtedly take longer) and I just tried checking the RCTF box on 5 operations, and it dropped around 7.5 hours off of the time!

I'm a bigger sissy than you though, because I'm not going to try it until I know a whole lot more about it.

[huskermcdoogle]

6 hours ago, motor-vater said:

Let that baby eat!!!!

Most people don't maximize the productivity they can get out of the tools they buy.  Granted it's about finding a good balance of productivity and economy from tool life.  At least 4 out of 5 applications I run into out there, I can get more productivity without sacrificing any tooling cost per part, often with a more expensive tool.

I know what I threw out there would fly without trouble using our tools.  Hope I haven't steered anyone down the wrong path due to not knowing the complete setup.

[Colin Gilchrist]

12 hours ago, So not a Guru said:

Hmm. Well, I usually use the tool mfg recommendations, at least to start at. But we have a titanium job we're running right now, that is 48 hours (according to MC, it will undoubtedly take longer) and I just tried checking the RCTF box on 5 operations, and it dropped around 7.5 hours off of the time!

I'm a bigger sissy than you though, because I'm not going to try it until I know a whole lot more about it.

Feed is your friend with Titanium. Hopefully your spindle has some decent torque. Don't be afraid to push the feed, and remember to keep that RPM low. I really wish more MTB's would make their spindle overrides with finer graduations. I love the ability on the Haas to use the Hand Wheel, to adjust the RPM in 1% increments. Sometimes a 10-15 RPM change (up or down) from nominal makes all the difference. But many builders only give you 25% increments...

[zero_divide]

You would need a very rigid machine to use anything over 1/2" with high-speed machining.

That said if that tool is all you have I would start to run it like this:

If it handles it nice, turn off coolant and double the RPM and feed (to keep the chip load the same). You will get better tool life without coolant.

[huskermcdoogle]

On 11/6/2021 at 12:59 PM, So not a Guru said:

I'm a bigger sissy than you though, because I'm not going to try it until I know a whole lot more about it.

Zeke,  Feel free to reach out for some optimized parameters.  I know you guys run Widia and Kennametal endmills.  I'm happy to compare notes on some parameters and see how conservative you actually are right now.

[So not a Guru]

11 hours ago, huskermcdoogle said:

Zeke,  Feel free to reach out for some optimized parameters.  I know you guys run Widia and Kennametal endmills.  I'm happy to compare notes on some parameters and see how conservative you actually are right now.

Nick, we are running the job on our Mazak Variaxis i800: CAT50, max torque 432, max RPM 10,000.

For the main 3D roughing passes we're using Widia's Varimill III 3/4" 7 flute with 2.25" length of cut (order #5971446). Unfortunately I have been unable to persuade management to invest in a shrink fit system, and I have had too many pull out problems with hydraulic holders on roughing paths, so we are using standard endmill holders (we grind a flat on the tool).

The cutting parameters we're using right now are: 180 SFM, 200% (1.50") Ae, 8% Re (0.06"), 0.003" IPT.

[cruzila]

Its kinda internet normal to get 50 replies and 50 different answers. My initial takeaway is acknowledgement that hands on experience is a thing of the past. My experience is the so called "book" gives a range and is only a guide to get you in the ballpark. I've run a 3/4 em to 50% cutwidth at 1-5/8 depth and it works. Granted it was one small corner plunge and the rest was light side cuts. My first go to with chatter is to increase feed by increasing feed or reducing speed. There is always always always going to be fine tuning to be done. Too many variables in setup, tool, tool brand tec.

[jean]

On 11/6/2021 at 9:57 AM, huskermcdoogle said:

You are way too slow for that radial engagement.

Not that I want to help a competitor sell tools...  I would do as follows.  If this is in a 50 Taper with a good setup, run full depth by all means.  If this is a 40 taper, you have too many points of contact for full depth.  But if you back it down to 1.625" depth or less, but not less than 1", you will find success.

Keep the 5% stepover for now.

I'd run 1000SFM, .0112fpt.  This takes into account chip thinning and speed factor based on the light radial.

5093 RPM, 341 IPM.  Feel free to back off the feed a little bit if the machine can't keep up, but I would go no slower on the feed than about 200.  If it burns up try to maintain the chipload, but reduce the surface footage.  Air blast would be better than coolant, but coolant would be ok if you can't get the chips away from the cutter.  I'd prefer dry if you don't have a chip evacuation issue.  A little heat will help you as long as you aren't re-cutting chips.

I would consider the above parameters middle of the road for our tools.  The fact that you have chatter is likely a function of machine stiffness.  Your original parameters show 6 points of contact, which IMHO for almost any 40 taper is way way too much.  3-4 points is better and should work on even on a medium quality machine

Nothing wrong with 4 or 5xd in steel.  Many people do it everyday.  But quality holders, setups and machines become very important very fast.  As I mentioned earlier, I likely wouldn't be doing that in a 40 taper with a 3/4" tool.  If you needed to, I would use a tool with a tapered core and maybe drop a flute or two to keep the contact points / force down.

My favorite 5xd tool is the Kennametal Harvi II long.  Never had trouble getting it to work.  I've run it in anything from alloy steel to Inconel with very good results.  One notable success was in Inconel 718, similar depths to what you are doing now, in a 40 taper, taking about .010 stepover.  We had a little springing, but that was from the setup as we were cutting on a weak trunnion table.

Husker

 

this is the set up pictures

set-up.docx

[JB7280]

On 11/6/2021 at 10:57 AM, huskermcdoogle said:

  Your original parameters show 6 points of contact,

What do you mean by this?  Are you saying the tool is touching the part in 6 places?  How do you even determine this?

[jean]

2 minutes ago, JB7280 said:

What do you mean by this?  Are you saying the tool is touching the part in 6 places?  How do you even determine this?

He is referencing the flutes of the cutter..

[jean]

ok, based on the set up the optimal running parameters are S1834 F33. for this tool.

I tried S3370 F175.28 and it was cutting good but since the vise was on a Midaco pallet it lifted the pallet slightly.

thanks to all that provided some insight. 

[huskermcdoogle]

On 11/8/2021 at 4:37 PM, JB7280 said:

What do you mean by this?  Are you saying the tool is touching the part in 6 places?  How do you even determine this?

What I mean is how many cutting points/flutes are in contact with the material at one time.  It is not reference to how many flutes there are in the cutter, yet that is part of the calculation, but so is width of cut, depth of cut and helix angle of the cutter.  It's a decent indicator of how much cutting force you are going to have.

[jean]

18 minutes ago, huskermcdoogle said:

What I mean is how many cutting points/flutes are in contact with the material at one time.  It is not reference to how many flutes there are in the cutter, yet that is part of the calculation, but so is width of cut, depth of cut and helix angle of the cutter.  It's a decent indicator of how much cutting force you are going to have.

Thanks for the clarification, I though you where talking about the flutes as point of contact.  

[Matthew Hajicek - Singularity]

On 11/7/2021 at 12:34 AM, Colin Gilchrist said:

Don't be afraid to push the feed, and remember to keep that RPM low.

I'm cutting Ti at 50K RPM right now, but then I'm using a .020" ball.

[JB7280]

On 11/11/2021 at 12:34 PM, huskermcdoogle said:

What I mean is how many cutting points/flutes are in contact with the material at one time.  It is not reference to how many flutes there are in the cutter, yet that is part of the calculation, but so is width of cut, depth of cut and helix angle of the cutter.  It's a decent indicator of how much cutting force you are going to have.

How do you calculate this?

[huskermcdoogle]

27 minutes ago, JB7280 said:

How do you calculate this?

LOL, I knew you were going to ask this.  I have a calculator that gives me this information.  I do not have the formulas right handy at the moment.  When I get a minute I will see if I can create something that can be shared to calculate this.  Or I will at least dig up the book I have should have this in it.  May be online, worst case I could derive it.

[JB7280]

3 minutes ago, huskermcdoogle said:

LOL, I knew you were going to ask this.  I have a calculator that gives me this information.  I do not have the formulas right handy at the moment.  When I get a minute I will see if I can create something that can be shared to calculate this.  Or I will at least dig up the book I have should have this in it.  May be online, worst case I could derive it.

I'd even accept steering me in the right direction to finding the info on my own.  My google-fu is failing me on this one.