Tool manufacturer start parameters

IanSathornCorp · Nov 8, 2017

Hello there, just posting a question regarding start parameters from different tool manufacturers. I almost never use the start parameters because most of the time the feed is simply too high for any application I'm using. Does anyone have any possible wisdom about how to use the start parameters in conjunction with common sense? For example, roughing a pocket in 6061-T6 with a 3/8 3 flute, 5/8 stub length, 50 percent stepover, 1/4" depth of cut. Off the top of my head I would generally start around 65 inches per minute at 12,000 rpm in a new Haas vf-2. Rego-fix hydo holder. Using water based coolant.

Now, the parameters from the book say

.0075-.0112 chip per tooth for side milling. Axial = equal to or less than 1xD
Radial = equal to or less than .5xD
CPT 2-3% of diameter

So if I go middle of the road CPT its .0093

So if you do 12000x3x.0093 = 334 IPM

Hmmmm common sense wise you think that is going to work out well as a START parameter?

Please let me know what you think.

Thank you

Ian

LockNut · Nov 10, 2017

Personally, I would start with the lower number, .007 per tooth. Totally feasable given a rigid setup. But I never go near .5D for high feed milling. At those numbers, radial depth of cut should be 15-20%of diameter and axial depth of cut could go up to 3XD. We do this all the time.

Paul

huskermcdoogle · Nov 10, 2017

It's all about ideal setup / machine / workpeice situations. In those cases, the starting parameters are just that, a good starting point. I have had many cases especially in drilling where I did have a good setup and machine and could almost double book starting values and get better life that at the starting point. But most of the time you have have back off on them. Now cutting wood most the time, it's all about how fast can you feed, then set the spindle based on desired chip load / quality of cut. So backward from how we have all been trained. But in most cases you can set the spindle speed based on how the tool sounds and then set your feeds accordingly.

Jashley73 · Nov 10, 2017

I'd be careful with at 3-flute, 3/8" diameter endmill with 50% stepover in aluminum. There's not much chip-space in the gullets on such a tool, and that's a large width-of-cut, combined with a large depth-of-cut for such a cutter. Your biggest enemy there is going to be clearing the chips from the flutes...

Cutting aluminum is usually pretty forgiving in regards to speed & feed. You can't really run too fast on the speed, and you can't really feed too hard for the cutting edges. The two biggest killers are clogging the flutes & breaking the tool, or simply breaking the tool from too much feed, and not enough core-strength for the feed-thrust - but even still, the cutting edges are usually still fine.

I'm not an aluminum expert, but I'd be careful going over 30% width on such a small cutter. If I had to go larger on width-of-cut, I'd go to a 2-flute and watch my depth-of-cut.

Contrary, if I had to go larger depth-of-cut, I'd go with a 3-flute and watch my width of cut.

Maybe this is ignorance, but I'd probably program my RPM to 90% of the machine's max - usually this keeps you in the power-band for the spindle, before power tapers off, and it still gives you some room to override to max-rpm if you want. And then I'd program the feed to like 14,237,793,544.999 inches/minute, and just use the override knob to approach 100% feed and see how things went.

DMF_TomB · Nov 11, 2017

IanSathornCorp said:
Hello there, just posting a question regarding start parameters from different tool manufacturers. I almost never use the start parameters because most of the time the feed is simply too high for any application I'm using. Does anyone have any possible wisdom about how to use the start parameters in conjunction with common sense? For example, roughing a pocket in 6061-T6 with a 3/8 3 flute, 5/8 stub length, 50 percent stepover, 1/4" depth of cut. Off the top of my head I would generally start around 65 inches per minute at 12,000 rpm in a new Haas vf-2. Rego-fix hydo holder. Using water based coolant.

Now, the parameters from the book say

.0075-.0112 chip per tooth for side milling. Axial = equal to or less than 1xD
Radial = equal to or less than .5xD
CPT 2-3% of diameter

So if I go middle of the road CPT its .0093

So if you do 12000x3x.0093 = 334 IPM

Hmmmm common sense wise you think that is going to work out well as a START parameter?

Please let me know what you think.

Thank you

Ian

.
usually tool manufacturer is listing maximum possible assuming a stub length cutter and high pressure coolant and short tool holder, rigid part and setup and machine with plenty of hp
.
i would using a excel make your own chart of feeds and speeds and other settings and note any sudden tool failures. so specific tool in specific tool holder setup to tight stickout distances and other dimensions you can see your own range of last 10 to 100 settings tried and see any sudden tool failures
.
one tool setup and rigid part maybe do 50 ipm feed and another long tool setup and flimsy part have trouble with 10 ipm. scrapping parts and breaking tools you have to learn based on you own experiences with your equipment. usually best to start slow and slowly increase things. sometimes tool failures are sudden with little warning often only a few seconds
.
many many times i have had settings work ok on 6 parts then i get a part out of a harder metal thats different and i get sudden tool failures, you need safety factor. when you run at max the slightest difference in metal being cut can cause sudden tool failure. dont assume all metal is exactly the same

litlerob1 · Nov 11, 2017

IanSathornCorp said:
For example, roughing a pocket in 6061-T6 with a 3/8 3 flute, 5/8 stub length, 50 percent stepover, 1/4" depth of cut. Off the top of my head I would generally start around 65 inches per minute at 12,000 rpm in a new Haas vf-2. Rego-fix hydo holder. Using water based coolant.

Ian

So .0018" chip load seems okay to you, in T6? :eek:

Some people have stopped thinking in IPM and are thinking in chip load. BUT that is not the only factor in a set-up, as we know. My first concern would be running 334 IPM on a......nevermind.

R

Bobw · Nov 11, 2017

I have a hard time everytime I go to machine aluminum... And plastics..

I always start WAY TOO LOW on the feed...

Years ago, just for fun, had a machine in the shop that was 12krpms and would feed up to 708ipm (IIRC).
Standard carbide 1/2" 4 flute finisher, and we wanted to see how hard we could feed it in aluminum..
around a .150 or .200 woc, 5/8 or so deep.. 708ipm and 12krpms, .015 a tooth, no problem.. Started
backing down the revs, got down to around 6k and called it quits.. almost .030 a tooth.. Kind of
crazy..

On those Korloy ripper mills, I start at about .016 - .018 per tooth.. And run it dry.

Years ago in MMS, they had an article on single flute endmills, little solid carbide jobbies
that looked like a router bit.. They were running .060 a rev/tooth with a 3/8"

If you can get the chips to clear, you can do pretty much do anything you want..

zero_divide · Nov 11, 2017

With the given DOC and WOC I would start here:

Material: 6061-T6 Series Aluminum 95 HB
Tool: 0.375in 3FL Carbide None HP/Roughing End Mill
Speed: 1177.5 SFM/ 12000.0RPM
Feed: 0.0066 in/tooth 0.0197 in/rev 235.98 in/min
Chip Thickness: 0.0066 in
Engagement: DOC=0.25 in WOC=0.19 in
MRR: 11.06 in³

You got to realize that is is a really stubby cutter and the engagement is not even that much.

Jashley73 · Nov 11, 2017

Bobw said:
Years ago in MMS, they had an article on single flute endmills, little solid carbide jobbies
that looked like a router bit.. They were running .060 a rev/tooth with a 3/8"

If you can get the chips to clear, you can do pretty much do anything you want..

Some people get really nit-picky about those though, because they're unbalanced. One of those little guys spinning 30K will create some vibrations, and some machine tool people aren't cool with that.

IanSathornCorp · Nov 13, 2017

Thank you for the respones

IanSathornCorp · Nov 13, 2017

litlerob1 said:
So .0018" chip load seems okay to you, in T6?

Some people have stopped thinking in IPM and are thinking in chip load. BUT that is not the only factor in a set-up, as we know. My first concern would be running 334 IPM on a......nevermind.

R

I am here to learn and broach a question. Not deal with douchebags such as yourself. If you have something informative to add do so, otherwise don't comment.

DMF_TomB · Nov 13, 2017

Bobw said:
I have a hard time everytime I go to machine aluminum... And plastics..

I always start WAY TOO LOW on the feed...

Years ago, just for fun, had a machine in the shop that was 12krpms and would feed up to 708ipm (IIRC).
Standard carbide 1/2" 4 flute finisher, and we wanted to see how hard we could feed it in aluminum..
around a .150 or .200 woc, 5/8 or so deep.. 708ipm and 12krpms, .015 a tooth, no problem.. Started
backing down the revs, got down to around 6k and called it quits.. almost .030 a tooth.. Kind of
crazy..

On those Korloy ripper mills, I start at about .016 - .018 per tooth.. And run it dry.

Years ago in MMS, they had an article on single flute endmills, little solid carbide jobbies
that looked like a router bit.. They were running .060 a rev/tooth with a 3/8"

If you can get the chips to clear, you can do pretty much do anything you want..

.
not proud of it but programming error where you dont pull up or retract enough and it moves in rapid ploughing through part at 1" depth with 1" dia end mill. been there done that.
.
still not sure i would want to run all the time at 800 ipm rapids in aluminum

IanSathornCorp · Nov 13, 2017

zero_divide said:
With the given DOC and WOC I would start here:

You got to realize that is is a really stubby cutter and the engagement is not even that much.

So run it with smaller depth smaller stepover and I could run the feed a lot higher?

Almost like highfeed mill strategies.

Thanks

DMF_TomB · Nov 13, 2017

IanSathornCorp said:
So run it with smaller depth smaller stepover and I could run the feed a lot higher?

Almost like highfeed mill strategies.

Thanks

only problem with high feeds is you are often moving machines sections weighing tons fast and inertia can effect accuracy. you can plow 2" depth and full width cutting with 2" dia end mill but at 5 ipm hp needed is high and with carbide at 20 ipm obviously you need 4x more hp and can be putting tons of cutting force on a part and thats a cast iron part other materials faster is possible.
.
but i have faulted out cnc before cause it exceeded its max amount of position error. that is if setup for .002" error when exceeded machine will stop with error message. obviously if parameter set so it accepts big errors it will never stop with fault or error message. might want to check what cnc setup to allow

zero_divide · Nov 13, 2017

IanSathornCorp said:
So run it with smaller depth smaller stepover and I could run the feed a lot higher?

Almost like highfeed mill strategies.

Thanks

With aluminum you can do that.
Sometimes the only way to prevent chatter is to run very hard at low depth of cut.

mhajicek · Nov 13, 2017

At the risk of sounding like a broken record, use HSMAdvisor and the Helical Milling Advisor.

DMF_TomB · Nov 13, 2017

zero_divide said:
With aluminum you can do that.
Sometimes the only way to prevent chatter is to run very hard at low depth of cut.

medium size cnc you got part over 1 ton and move too fast it will easily just stop with fault message. in some cases better you use bigger cutter at higher depth and width and travel slower

zero_divide · Nov 13, 2017

DMF_TomB said:
medium size cnc you got part over 1 ton and move too fast it will easily just stop with fault message. in some cases better you use bigger cutter at higher depth and width and travel slower

Omfg. Do you realize that about 0.1% or people routinely machine 1 ton parts around here?
Gosh! The question was about a 3/8" endmill christsake!

Mtndew · Nov 13, 2017

zero_divide said:
Omfg. Do you realize that about 0.1% or people routinely machine 1 ton parts around here?
Gosh! The question was about a 3/8" endmill christsake!

You're fighting a losing battle.
He never contributes to the conversation, instead all he does is spew shit about big cast iron parts on a large machine. Never addressing the actual question the OP asks.

litlerob1 · Nov 13, 2017

IanSathornCorp said:
I am here to learn and broach a question. Not deal with douchebags such as yourself. If you have something informative to add do so, otherwise don't comment.

Grow some skin man. If you read what I wrote without getting your feelings hurt, there are points there. .0018" CL is very small in 6061 T6, there is more to Machining than chip load, IPM is irrelevant, in context of MRR.

But just to validate you, I am a douchebag.

R

Tool manufacturer start parameters

Plastic

Stainless

Stainless

Titanium

Diamond

Diamond

Diamond

Stainless

Titanium

Plastic

Plastic

Diamond

Plastic

Diamond

Stainless

Diamond

Diamond

Stainless

Diamond

Diamond

Similar threads