Speeds and Feeds - 25mm 3 Flute Indexable End Mill - In Steel

**herrmc** · 11-27-2018, 02:03 AM

Greetings,
I have a Tormach PCNC-1100 Series 3

I am very inexperienced with calculating speeds and feeds on my tooling ... and determining what proper depth of cut I should be using.

I have a 25mm 3 Flute (non center cutting) end mill. I have a block of 4" thick Mild steel (Hot Roll) that I need to carve a notch out in ... Can someone please help me with determining a good set of Speeds and Feeds and Depth of cut?

Thanks in advance,
Curtis

Similar Threads:

Need Help!- Steel Feeds and Speeds
Newbie- Proper Feeds and Speeds - Steel Turning with Carbide on Taig CNC Mill
Need Help!- Recommended speeds and feeds for TTS indexable mill inserts?
Need Help!- OSG 3 flute carbide end mill in mild steel - Stupid slow recommended feeds
Need Help!- Countersink Speeds and Feeds, 6061, 6-flute carbide

**jttoner** · 11-27-2018, 09:16 AM

I'm not in my shop right now, but I'd give HSM Adviser a shot.

**jwatte** · 11-27-2018, 07:11 PM

G-wizard says run at 1270 rpm, feed at 24.8 ipm, cut 0.04 deep.
(I had to guess on your mill geometry a little bit == how much stick-out, how deep are you cutting total?)
This is going to be mostly horsepower limited, so the low RPM may actually be a problem unless you move the belt to low gear.
ALso, lighter cuts at the same feed/speed will use less HP and thus be safer.

Speeds and Feeds - 25mm 3 Flute Indexable End Mill - In Steel-g-wizard-cut-example-jpg

I haven't done this exact cut, but what G-wizard recommends sounds pretty good to me. (This is the most aggressive setting, btw; finer finish by feeding significantly less and slightly lowering RPMs)

**zero_divide** · 11-27-2018, 09:25 PM

According to HSMAdvisor
If it is a non-coated carbide cutter, and assuming slotting operation:

Material: A36, 44W Hot Roll Steel 160-220 HB
Tool: 25.000 mm 3FL Carbide None Solid End Mill
Speed: 94.6 m/min / 1205.2RPM
Feed: 0.0726 mm 0.2179mm/rev 262.66 mm/min
Engagement: DOC=2.57 mm WOC=25.00 mm

Or in imperial:

Material: A36, 44W Hot Roll Steel 160-220 HB
Tool: 0.984 in 3FL Carbide None Solid End Mill
Speed: 310.4 f/min / 1205.2RPM
Feed: 0.0029 in 0.0086in/rev 10.34 in/min
Engagement: DOC=0.10 in WOC=0.98 in

Speeds and Feeds - 25mm 3 Flute Indexable End Mill - In Steel-capture25mmtormach-jpg

But i agree. You need to provide more info.

**herrmc** · 11-28-2018, 02:12 AM

-- I typed a long reply, then while attempting to add pictures, it got lost -- so here I go again.
.................................................. .................................................. .............................................

-- I included to pictures ... I cut the slots in these a different way (not milled)... just showing you to illustrate what I am doing, and how I am orienting it in the vise.

-- The Stock (4" x 4" x 15" HR A-36) ... The "Top" of this part (as it will be installed) is with the 15" standing up tall.... in the "top" of the part ... I need to cut a "U" shape (the radius in the bottom of the "U" is not important, can be about anything)

-- I am working on the stock "laying on it's side" ... X = 15", Y = 4", Z = 4"

-- I am not sure if the correct terminology is "mill a slot"... or ... "Mill a pocket" (probably neither)... it is like milling a pocket .. except one end is open so I can approach the material from the side.

-- The geometry of my Cut: X = 2", Y = 1.5", Z = 4"

-- I believe the Tormach 25mm end mill will take a .25" DOC ... I entend to approach the stock from the side... at 0.25" DOC and 0.6" WOC ... work my way through that (8 times) to reach a depth of 2" ... then turn the material over and come 2" deep from the other side (my thought is that 4" deep is just too deep to go, and better to come from each side 2")

****

This is the first time I have ever heard of "HSMAdvisor" ..... I have looked it up (google) and read a little about it after seeing it in the posts (your answers to me)... I will continue to research it. I did Just last night get GWizard... and Have been working with it.

This is one scenario I have come up with (below):

RPM = 1200
Feedrate = 11 IPM
DOC = 0.25" (Axial Engage = 25.5%_
WOC = 0.6" (Radial Engage = 61.2%)
SFM = 308
Chipload = 0.0031 IPT
Deflection = 0.000101 (10%)
HP = 1.0938

************************************************** ********

I have watched Youtube videos .... read tutorials and articles, and generally tried to learn what I can about this .... I am admittedly very inexperienced with this (and unsure of myself). I think I grasp the concept, but I would rather any mistakes in my thinking be flushed out here ... if you guys are willing to help and educate me... than crashing my machine.

-- I have learned that I can work with the numbers (RPM, Feedrate, DOC, WOC) and come up with several recipes that seem that they "Should" work .... but I obviously lack the experience to know how to choose the best recipe ....

-- Thank you all for your attempts to help me.

Regards,
Curtis

**herrmc** · 11-28-2018, 02:24 AM

The 25mm end mill = 1.53" long ... then when it is attached to the arbor ... it's possible cut dept is a little more

-- I have all 3 arbors for this mill (short, medium, long)

Short allows me a max cut depth of about 1.73"

Medium allows me a max cut depth of about 3" deep

Long would allow me more than 4" possible cut depth (I didn't figure on using this one)

***************************************

-

**jwatte** · 11-28-2018, 02:34 PM

There's a continuum between "many fast shallow passes" and "few deep passes."
If you approach work from the side, and take deep (in Z) but shallow (in X) cuts, you can use more of the sides of the flutes, which may improve tool live, but you spend more time not engaged (shuttling back to the next cut engagement,) which may increase cut time.
The "2D adaptive" tool paths in Fusion 360 generate pretty good "deep Z, shallow X" tool paths, using the "slowly varying engagement" style -- but, as you can see, spends a lot of the time not engaged.
The proposal I made was to step down 0.4 for each cut, so "shallow Z, deep X" (or "axial" vs "radial" to use industry terminology)
You could mill this slot/pocket with almost constant engagement by simply profiling it, using ramping, with a stepdown of 0.04 per ramp step.

The product of radial times axial engagement ends up being the material load on the cutter -- another way of thinking about that is "chip load times depth" -- which ends up determining your material removal rate, which ends up determining how heavily loaded the spindle is.
In this case, for steel with a wide cutter, the end limitation is going to be horsepower of the Tormach spindle, and the choice between "fast shallow constant engagement" and "slow deep shaving" is up to your preference.

Also, if the end result is 4" deep, and the flutes on your end mill are 1.5" of cutting, is the end mill of the "relieved shank" variety? Else you can't stick the 4 inches down you need. (Or even 2 inches, if you flip the part in the middle.)
You're also going to have trouble doing a smooth finish cut at the end (if you have some "stock to leave" to shave off last.) because you'll see the stair stepping. Maybe that's OK.

**herrmc** · 11-28-2018, 08:04 PM

jwatte --- Thank you very much for the reply. That is my conundrum ... is understanding "when" to choose the "few deep" or the "many shallow" ...... plunge, adaptive, or normal pocket ...... and it seems like if I ask 5 people, I get 5 different answers :-)

--- I love learning, and the things you say make sense.... thank you for taking the time to help me.

> Overall time to process the part is not too important to me (within reason)...

> I was up until 4am this morning going through Fusion tutorials ... I am getting there... (to be functional)... but I am not there yet.

> The shank is relieved (made that way)... it is 0.87" diameter .... I can pretty easily get 1.73" with the short arbor (tool is 1.53 .. and the arbor allows another .2) ... I can switch to the medium length arbor... and reach well below halfway.... the long shank would allow me to stick all 4" (and more) into the slot.... a little stair stepping I can handle...

--- Thank you again for your help!

**jttoner** · 11-29-2018, 03:50 PM

The best 360 tutorials are Lars Christensen and Paul McWhortor, and no annoying goofy background music.

**AUSTINMACHINING** · 11-30-2018, 10:32 AM

Originally Posted by herrmc

jwatte --- Thank you very much for the reply. That is my conundrum ... is understanding "when" to choose the "few deep" or the "many shallow" ...... plunge, adaptive, or normal pocket ...... and it seems like if I ask 5 people, I get 5 different answers :-)

--- I love learning, and the things you say make sense.... thank you for taking the time to help me.

> Overall time to process the part is not too important to me (within reason)...

> I was up until 4am this morning going through Fusion tutorials ... I am getting there... (to be functional)... but I am not there yet.

> The shank is relieved (made that way)... it is 0.87" diameter .... I can pretty easily get 1.73" with the short arbor (tool is 1.53 .. and the arbor allows another .2) ... I can switch to the medium length arbor... and reach well below halfway.... the long shank would allow me to stick all 4" (and more) into the slot.... a little stair stepping I can handle...

--- Thank you again for your help!

So many variables, its just best to try different methods and see what works best for your set up. Obey SFM, and start light and shallow. Bump your way up from there. I like to do a reality check first with the longest tool stick out (worst case scenario) to guage what im in for.