Constant surface feed for milling

cncwhiz · Aug 26, 2016

I have a tool that is running at multiple diameters and depths. The machine it is running on is a POS. I pretty much found a sweet spot where the tool needs to run at. I use constant surface for tapping but have not used it for milling. I use to use it on lathes but that was many moons ago. Anybody use it and what is your format?

toolmaker96 · Aug 26, 2016

You serious?

chucker · Aug 26, 2016

Popcorn in hand feet on stool gona be interesting.

cncwhiz · Aug 26, 2016

toolmaker96 said:
You serious?

For "most" milling formulas, the actual cut diameter is not used. From a geometry stand point the smaller diameter the heavier cut. If this is done using a constant geometry ie; spindle speed varaition and or feed variation the cut will be uniformed. This is done on lathes all the time but why not mills? So "am I serious", yes.

LockNut · Aug 26, 2016

Because in milling the driving factor is not the part geometry, it is the cutter geometry. 50 IPM is still 50IPM regardless of the diameter of the part. Milling does not use constant surface footage except as being applied to the end mill diameter. No spindle speed variation, no feed variation.

(SF per M X 3.82) divided by cutter diam. = RPM

RPM X Feed per tooth X number of teeth = Feed

So, yes, are you serious?

JNieman · Aug 26, 2016

cncwhiz said:
For "most" milling formulas, the actual cut diameter is not used. From a geometry stand point the smaller diameter the heavier cut. If this is done using a constant geometry ie; spindle speed varaition and or feed variation the cut will be uniformed. This is done on lathes all the time but why not mills? So "am I serious", yes.

I have no clue what you are talking about. Or maybe you have no clue what you're talking about. I'm not sure.

Constant radial tool engagement, chip load, surface speed... in CNC machining that's typically controlled with the toolpath. Your RPM 'typically' runs the same for each toolpath. Your feedrate will 'typically' be the same while the tool is cutting.

I have no idea what it is you think you're trying to accomplish, though, 'cncwhiz'

cncwhiz · Aug 26, 2016

JNieman said:
I have no clue what you are talking about. Or maybe you have no clue what you're talking about. I'm not sure.

Constant radial tool engagement, chip load, surface speed... in CNC machining that's typically controlled with the toolpath. Your RPM 'typically' runs the same for each toolpath. Your feedrate will 'typically' be the same while the tool is cutting.

I have no idea what it is you think you're trying to accomplish, though, 'cncwhiz'

I know exactly what I am talking about. Example, I have a bore that I am roughing out and it has multiple diameters at different depths. Forulas say if sfm is known, rpm = 3.82 * sfm/dia. Feed is ipm = ipr x rpm. Now, what I am talking about is from the zero point of the bore the feed and or speed change"like facing in a lathe", either the spindle, feed or both, change so the material removal and chip load stay constant. Its not hard to see that you program the spindle speed at the start of the tool, once the tool is into the cut, depending on the diameter of the cut the geometry changes. You can add a feed rate at every diameter but it will not be constant. The given speed and feed work well for a 2" cut but not for a .5 cut as well as the arc in move.

CarbideBob · Aug 26, 2016

Constant surface footage or constant feed rate at the periphery of the cutter? I think you are looking for #2.
Some controls will modify the feed rate if you input the correct tool radius and are using comp.
Contouring the inside of a 4 inch hole with a 3.75 inch cutter is an example of where this is handy.
Tiny actual machine circle, needs to slow down a bunch. Opposite needed when you are outside a boss. Think 14" cutter making a 1/4 inch pin. Big circle. You need to be flying crazy fast on cutter center-line.
Not the same as CSS on a lathe. Different animals.
Bob

cncwhiz · Aug 26, 2016

CarbideBob said:
Constant surface footage or constant feed rate at the periphery of the cutter? I think you are looking for #2.
Some controls will modify the feed rate if you input the correct tool radius and are using comp.
Contouring the inside of a 4 inch hole with a 3.75 inch cutter is an example of where this is handy.
Tiny actual machine circle, needs to slow down a bunch.
Bob

You are correct in that I am thinking about item # 2.I am thinking about building a macro with math functions but not sure how it will work. It can't work for every tenth but if it have given points then it might work. The machine I was working on this for just finished dying but I still think I will do this. I believe it will result in a better finish, better tool life and less wear and tear on the machine. I just hate that I start thinking about this shit on Friday afternoon.

Red James · Aug 26, 2016

Your formula is correct. BUT the diameter in your formula is the diameter of the rotating part, i.e. the end mill diameter.

Matt@RFR · Aug 26, 2016

Maybe instead of making up names that nobody has heard of, you could just describe what it is you're trying to do right off the bat. You don't need macros, you need formulas to figure the correct feedrate for each diameter. This has nothing to do with depth or SFM, and it shouldn't. Here are the formulas you need:

ID Nominal IPM * (minor dia - cutter dia) / minor dia = adjusted feedrate
OD Nominal IPM * (major dia + cutter dia) / major dia = adjusted feedrate

Bobw · Aug 26, 2016

cncwhiz said:
I know exactly what I am talking about.

At least there is one person that knows what you are talking about.

angelw · Aug 26, 2016

Bobw said:
At least there is one person that knows what you are talking about.

JNieman said:
Quote Originally Posted by cncwhiz View Post
For "most" milling formulas, the actual cut diameter is not used. From a geometry stand point the smaller diameter the heavier cut. If this is done using a constant geometry ie; spindle speed varaition and or feed variation the cut will be uniformed. This is done on lathes all the time but why not mills? So "am I serious", yes.

Reply by JNieman
I have no clue what you are talking about. Or maybe you have no clue what you're talking about. I'm not sure.

Constant radial tool engagement, chip load, surface speed... in CNC machining that's typically controlled with the toolpath. Your RPM 'typically' runs the same for each toolpath. Your feedrate will 'typically' be the same while the tool is cutting.

I have no idea what it is you think you're trying to accomplish, though, 'cncwhiz'

Hello Bob and JNieman,
I'm thinking the OP is a Disciple of Johnny Larue; accordingly, Johnny may be on the same page. However, Johnny advocates that CSS should NOT be used - ever. But he was referring to a Lathe at the time, so it may be the inverse when using a Mill control.

Regards,

Bill

MaxPrairie · Aug 26, 2016

Change your feed rates higher as you get larger on the diameter. If your bore is a one line bore cycle then thats a different story.

JNieman · Aug 29, 2016

cncwhiz said:
I know exactly what I am talking about. Example, I have a bore that I am roughing out and it has multiple diameters at different depths. Forulas say if sfm is known, rpm = 3.82 * sfm/dia. Feed is ipm = ipr x rpm. Now, what I am talking about is from the zero point of the bore the feed and or speed change"like facing in a lathe", either the spindle, feed or both, change so the material removal and chip load stay constant. Its not hard to see that you program the spindle speed at the start of the tool, once the tool is into the cut, depending on the diameter of the cut the geometry changes. You can add a feed rate at every diameter but it will not be constant. The given speed and feed work well for a 2" cut but not for a .5 cut as well as the arc in move.

You... realize the diameter of your bore is not the diameter to be used in that formula... don't you?

Context is important, here. You're applying lathe habits to a mill. You really do have to basically unlearn a lot of what you take for granted when you switch from lathe to mill. It seems basic and normal when you're in front of a lathe, but you have to understand that the mill works almost opposite to a lathe.

I mean, think about it... why would there be milling formulas for diameter of cut-feature when mills cut an infinite amount of shapes? The dia refers to your tool. The one in the spindle, before you assume too much..

I think you just got started on a big misunderstanding. Sometimes, if the world looks upside down maybe you should first determine whether or not you're standing on your head, first!

JNieman · Aug 29, 2016

MaxPrairie said:
Change your feed rates higher as you get larger on the diameter. If your bore is a one line bore cycle then thats a different story.

Why would your feed rate, in in(dist)/min, change on a mill?

Brad_Applied · Aug 29, 2016

There are lots of optimization programs out there that adjust federate based on chip load, tool engagement angles, etc.. We use both Optipath and ThirdWave. The programs actually insert changing federate lines into the original program (doesn't change path, just feed rate and your program can get really big quickly). If your machine has a sweet spot these types of programs might keep you in the sweet zone (assuming nothing else changes while in the cut).

Another possible is programming in inch/rev. This would take into account any spindle bog while cutting and then slow the feedrate.

Matt@RFR · Aug 29, 2016

JNieman said:
Why would your feed rate, in in(dist)/min, change on a mill?

Because you program at the spindle centerline, but you cut at the periphery of the tool, so on arcs the actual chip load varies. The closer to the tool size that the arc is, the greater the discrepancy.

JNieman · Aug 29, 2016

Matt@RFR said:
Because you program at the spindle centerline, but you cut at the periphery of the tool, so on arcs the actual chip load varies. The closer to the tool size that the arc is, the greater the discrepancy.

Judging from the nature of the OP, we're talking about the very basics, here, and not getting into trochoidal, radial chip thinning, adaptive or constant tool engagement strategies... unless I'm mistaken. It seemed to me, that the OP had a misunderstanding of how the programming was done. I might be wrong - it's sometimes hard to read peoples off-hand forum posts about technical things unless they are very clearly and thoroughly written in detail.

cncwhiz · Aug 29, 2016

Brad_Applied said:
There are lots of optimization programs out there that adjust federate based on chip load, tool engagement angles, etc.. We use both Optipath and ThirdWave. The programs actually insert changing federate lines into the original program (doesn't change path, just feed rate and your program can get really big quickly). If your machine has a sweet spot these types of programs might keep you in the sweet zone (assuming nothing else changes while in the cut).

Another possible is programming in inch/rev. This would take into account any spindle bog while cutting and then slow the feedrate.

This is what I am referring to. For the record, I have been a machinist for over 30 years. I am fully aware of the forumlas and what they do. Using the basic forumlas does not take into account that one of the biggest factors is the relationship of the tool geometry "size" to the diameter of the hole diamater is not taken into account. If I use a 1" cutter and I cut a 2" bore with it as well as a bore that is 1 1/4" the removal rate and the geometry are not even close to the same. If you could use a constant surface feed based on the tool diameter as well as the hole diameter either the spindle speed or the actual feed rate would change. I have not programmed a lathe for over 20 years but I think that the way they use constant surface feed should be applied to the mill as well.

Constant surface feed for milling

Aluminum

Hot Rolled

Aluminum

Aluminum

Stainless

Titanium

Aluminum

Diamond

Aluminum

Stainless

Titanium

Diamond

Diamond

Hot Rolled

Titanium

Titanium

Aluminum

Titanium

Titanium

Aluminum

Similar threads