Need help with adaptive toolpath options

Joe Miranda · Jul 21, 2020

We have been trying to use adaptive machining more and more and have not really found a scientific approach to selecting the depth of cut and step over amounts. We are currently cutting some gray iron with 1/2 carbide endmills at 1" doc and 1/8" step over @ 200sf and 16 ipm feed rate.

I love the material removal rate but we occasionally snap endmills. I would really rather not do that but I want to maximize material removal on this job. To give you an idea - the blocks start at 150lbs and finish at 15lbs - that's a lot of material. In the future they will be cast near to finish - these are prototypes.

What have you guys found as a sweet spot? Thanks.

dodgin · Jul 21, 2020

Joe Miranda said:
We have been trying to use adaptive machining more and more and have not really found a scientific approach to selecting the depth of cut and step over amounts. We are currently cutting some gray iron with 1/2 carbide endmills at 1" doc and 1/8" step over. I love the material removal rate but we occasionally snap endmills. I would really rather not do that. What have you guys found as a sweet spot? Thanks.

I'll usually program 8 to 12 percent of the cutter diameter as a stepover for adaptive cutter paths.

Mike1974 · Jul 21, 2020

Typically (Ya I know, setup, rigidity, etc, but you have to determine that) adaptive paths use full LOC, if possible, and 5-15% stepover, depending on cutter diameter and flute length.... Also, chip load per tooth will seem abnormally high, like .005-.01 because of chip thinning.

Didn't mention if you are using coated carbide, hss, or...? I would use a variable helix coated 4 flute carbide for what you describe. YMMV.

Milland · Jul 21, 2020

What are you doing for chip clearing? If you're running into pockets filled with CI chips, I'd expect tool breakage.

Your stepover sounds high (as those above say), I'd try less (.06") and up the IPM to start.

Hardplates · Jul 21, 2020

I usually work in steel but a safe starting point for me is a 3/8" 6 flute .900" deep, .03 stepover 6000 RPM 200 IPM. These numbers can be pushed much harder but I have found I can usually reduce cycle times by taking a lighter cut faster rather than a heavier cut slower.

Small cuts mean small chips which don't require as much flute volume on the endmill, which lets you run more flutes and end up with a larger core that is more rigid.

ChipSplitter · Jul 21, 2020

Joe Miranda said:
We have been trying to use adaptive machining more and more and have not really found a scientific approach to selecting the depth of cut and step over amounts. We are currently cutting some gray iron with 1/2 carbide endmills at 1" doc and 1/8" step over @ 200sf and 16 ipm feed rate.

I love the material removal rate but we occasionally snap endmills. I would really rather not do that but I want to maximize material removal on this job. To give you an idea - the blocks start at 150lbs and finish at 15lbs - that's a lot of material. In the future they will be cast near to finish - these are prototypes.

What have you guys found as a sweet spot? Thanks.

That sounds like heavy roughing would work just fine. Just make sure you use a variable pitch, variable helix, coated EM with an edge prep to prevent fracturing.

I would use a 4-fluter and start at 400 SFM, 0.350" WOC, 1" DOC, and .003 IPT.

Alternatively, you could use a 6-fluter and run 800 SFM, 0.050" WOC, 1" DOC, and .005-.007 IPT.

The 2nd approach would be HEM but I'll bet the first would run circles around it in this application.

primeholy · Jul 21, 2020

It's gonna depend on a few things like material, machine, setup rigidity. Im assuming that adaptive machining is High Speed Machining? I use volumill with Gibbscam on a Makino F5. I use 5 flute .5 diam end mills with 1.25 loc. On 1018 I run at 1050 surface feet at .0048 chip per tooth with up to 1.25 doc. Stepover at 1.25 i use .02, but I will increase that if my doc is lower.

Joe Miranda · Jul 21, 2020

primeholy said:
It's gonna depend on a few things like material, machine, setup rigidity. Im assuming that adaptive machining is High Speed Machining? I use volumill with Gibbscam on a Makino F5. I use 5 flute .5 diam end mills with 1.25 loc. On 1018 I run at 1050 surface feet at .0048 chip per tooth with up to 1.25 doc. Stepover at 1.25 i use .02, but I will increase that if my doc is lower.

You're running 1050sf in gray iron?

We are using coated variable pitch endmills with flood coolant.

Mtndew · Jul 21, 2020

Joe Miranda said:
You're running 1050sf in gray iron?

Read again.

primeholy · Jul 21, 2020

Joe Miranda said:
You're running 1050sf in gray iron?

We are using coated variable pitch endmills with flood coolant.

I haven't machined cast iron in many years. Nowadays its a heavy rotation of 1018, finkl, 4140 pre, m2, s7, with a dab of aluminum.

These are how I base my surface feet with different materials. I use coolant on 1018, 4140 pre, and aluminum. If I run out of spindle RPM, I bring my surface feet down till it falls in range. Stepover I do about 40 % tool diameter

Volumill surface feet

Take recommended surface feet and chip load x3
Surface feet Chip Load (tool diameter x .0032)

D2/M2 260 x 3 x 3
H13 230 x 3
4140 300 x 3
1018 350 x 3
A2 250 X 3
FORGE DIES 200 X 3
S7 215 X 3
6061 AL 800x3

Joe Miranda · Jul 22, 2020

primeholy said:
I haven't machined cast iron in many years. Nowadays its a heavy rotation of 1018, finkl, 4140 pre, m2, s7, with a dab of aluminum.

These are how I base my surface feet with different materials. I use coolant on 1018, 4140 pre, and aluminum. If I run out of spindle RPM, I bring my surface feet down till it falls in range. Stepover I do about 40 % tool diameter

Volumill surface feet

Take recommended surface feet and chip load x3
Surface feet Chip Load (tool diameter x .0032)

D2/M2 260 x 3 x 3
H13 230 x 3
4140 300 x 3
1018 350 x 3
A2 250 X 3
FORGE DIES 200 X 3
S7 215 X 3
6061 AL 800x3

What kind of endmills are you using? Your surface feet sounds really high. What kind of tool life are you getting?

Mike1974 · Jul 22, 2020

primeholy said:
I haven't machined cast iron in many years. Nowadays its a heavy rotation of 1018, finkl, 4140 pre, m2, s7, with a dab of aluminum.

These are how I base my surface feet with different materials. I use coolant on 1018, 4140 pre, and aluminum. If I run out of spindle RPM, I bring my surface feet down till it falls in range. Stepover I do about 40 % tool diameter

Volumill surface feet

Take recommended surface feet and chip load x3
Surface feet Chip Load (tool diameter x .0032)

D2/M2 260 x 3 x 3
H13 230 x 3
4140 300 x 3
1018 350 x 3
A2 250 X 3
FORGE DIES 200 X 3
S7 215 X 3
6061 AL 800x3

Gawd I hated finkl. That shit was nasty! :ack2:

primeholy · Jul 22, 2020

Joe Miranda said:
What kind of endmills are you using? Your surface feet sounds really high. What kind of tool life are you getting?

This is the 1/2"
STR540.500D3R015.0Z5 ALCRN | Secotools.com

1/2 is our main tool used for this type of application, but we do use up to 3/4, and down to 1/8. Mostly Niagara, but we use some YG sometimes.
We aren't production, so I cant give you a good tool life answer, but the amount of material we machine, I think we do pretty well. I definitely wouldn't have been able to pull off these numbers with the fadals/haas I used to run, but the Makinos have more finesse/accuracy to make precision high feed movements. Although they definitely don't have the balls to hog out material the old traditional way I used more on the fadals.

primeholy · Jul 22, 2020

Mike1974 said:
Gawd I hated finkl. That shit was nasty!

I hated it when I first started. I still don't love it. Mainly doing 3d toolpaths with bn ranging from 8mm down to 1mm. Cutting stellite though, is a real pia. I have my surface feet dialed in much better for the stellite than when I first started.

What did the end mill say to the stellite?

OH SNAP!

Mtndew · Jul 22, 2020

Are you on a machine capable of higher feedrates?
I'd suggest 1" depth, .05" stepover, 950sfpm, and .0065" ipt.
This would effectively double your MRR.
Oh and check out HSM Advisor, it's well worth the small price tag.

Hardplates · Jul 22, 2020

Joe Miranda said:
What kind of endmills are you using? Your surface feet sounds really high. What kind of tool life are you getting?

It's not uncommon to run over 1000 SFM since most of the heat is getting put into the chip. I personally can run faster dry than with coolant (in steel), not sure if that would hold true if I had TSC but I don't.

Lately I have been running AlCr coated six fluters with a corner radius and they just won't die.

Search

Largest Manufacturing Technology Community on the Web

Search

Need help with adaptive toolpath options

Joe Miranda

Titanium

dodgin

Hot Rolled

Mike1974

Diamond

Milland

Diamond

Hardplates

Stainless

ChipSplitter

Titanium

primeholy

Aluminum

Joe Miranda

Titanium

Mtndew

Diamond

primeholy

Aluminum

Joe Miranda

Titanium

Mike1974

Diamond

primeholy

Aluminum

primeholy

Aluminum

Mtndew

Diamond

Hardplates

Stainless

Attachments

Similar threads