What's new
What's new
By:
Advanced search…

Finish pass speed and RPM?

B

bellinoracing

Hot Rolled
Joined
Aug 27, 2009
Location
Arizona USA
In general when cutting your finish pass do you want to go faster, or slower, or the same speed as your roughing speed? Part of me thinks faster, but part of me thinks slower. I am guessing probably slower so that it cuts the hole on size and tool flex is not an issue(I am only cutting .015 on my finish pass so I would be very surprised if any tool flex would occur but I am not positive). I am using a 1/2 three flute finish endmill to cut aluminum. I am turning it about 3,000 rpm and moving about 25 ipm for roughing and finish passes. Its cutting very well but I thought maybe we can cut our time down a little, improve cutter life, and finish quality. I think I may step rpm up to 4,000 but what should I do with my roughing and finish feeds. Its niagara coated endmill for aluminum and I am using a Haas TM1 with a 6,000 max rpm. I could turn it 6,000 but would prefer not to run it at max speed constantly.

Thanks
 
It that's a carbide endmill you're spinning way slower than you should.

Below are some basic guidelines for setting your speeds, feeds and depth of cuts.

Most of this was stolen liberally from Stanley Dornfeld who gave me these basic recommendations when I was starting out.

These ares starting points, adjust your feed rates up or down depending on how your machine is taking it.

Paul T.

Figuring your SFM (Surface Feet/Minute, which will determine your RPM)

SFM with HSS endmills
Stainless Steel 40
Mild Steel 100
Brass 300
Aluminum 400

With carbide endmills, multiply those settings by 3 as a starting point, so:
SFM with Carbide Endmills
Stainless Steel 120
Mild Steel 300
Brass 900
Aluminum 1200

Then:

RPM = 4 x SFM/Diameter

Now to find your feed, first calculate your chip load. A reasonable starting point for the chip load is to divide your endmill diameter by 200.

Chip Load = Diameter/200

Then to calculate your Feed Rate:

Feed Rate= RPM x Num of Teeth x Chip Load

So for example with a 1/4" HSS endmill in steel, your RPM should be:

RPM = 4 x 100/.25 = 1600

Your feedrate should be:

Feed Rate = 1600 x 2 x .25/200 = 4 ipm

This a starting point, I usually crank down a little from these recommended settings to see how the machine responds.

As far as your maximum depth of cut, on smaller machines this is often determined by the available spindle HP you have. However if the machine is up to it, I use the following guidelines for max radial and axial cut (borrowed from Stan Dornfeld):

Slotting: Cut Depths
6061 Aluminum, Brass - 1/2 endmill diameter
7075 Aluminum - 40% endmill diameter
Mild Steel - 30-35% endmill diameter
Stainless Steel - 25% endmill diameter

Rough Profiling Tool Overlap: 70% endmill diameter or less
Finish Profiling Tool Overlap: 3% endmill diameter

Plunging Rates:
Take the normal slotting feedrate and divide by the number of flutes.
 
1. Quit babying that thing. I run my VF-2ss at 12k (top speed) for hours and hours with zero issues. I run EVERYTHING 1" and under (except drills/reamers/taps) at 12k in aluminum. There are a few threads on this subject on cnc zone. If you want to speed up, RPM is the quickest way to do it.

2. Start thinking in chip load or inches per tooth (different way of saying the same thing). Now try stuff! At some point, you need to just try different feeds and find out for yourself what works for your parts on your machine with your tooling, your coolant, your programming style, etc. Myself and many others are happy to help, but what are you REALLY learning? How other people would machine your parts? You need to start seeing what changes do for yourself.

3. Don't call me an asshole. I'm well aware of this. :)

PaulT said:
Chip Load = Diameter/200
Click to expand...
Is that a typo? With that formula, that's .0025 ipt for a 1/2" endmill. I run nearly double that in a slot. In stainless. On a Haas. And .0025 ipt is a FINISH pass in aluminum! bellino is looking to speed up, not slow down.

Please see #3 above.
 
Cutter flex is a function of chipload so twice the RPM at twice the feedrate results in the same tool deflection, possibly less since the tool cuts more efficiently at higher SFM.

The question then becomes what is the limiting factor on your machine?

On my mid 90s Cincinatti Arow it runs out of contouring accuracy at elevated feedrates before it runs out of RPM (with a 1/2" coated carbide end mill, anyway).

I let GWizard calculate the speed and feed ratio required to maintain chip thickness for cutter longevity (too thin of a chip promotes rubbing and tool edge wear) then scale back the feed to 40 IPM and scale the speed proportionally.

With smaller tools the spindle may run at max (6000 RPM) for hours, that's just the way it is.

Joe
 
Sorry I should have said its just a HSS endmill. You know I learned those rules in school about 4 years ago but from what little I have seen it seems like they more or less throw those rules out the window when you start running cnc machines with some of the new coated cutters. I know most materials are a little more picky than aluminum but I have had lots of people tell me to run the RPM as fast as possible.

And yeah I was wondering if Diameter/200 was a typo as well. By my calculations with my .5 endmill thats only .0025 chip per tooth? I thought a good starting point was usually around .003 per tooth but some of the new cutters I have looked at go to .006 per tooth or better.

Thanks for the depth cuts formula, I actually didn't know those.

I would run it at 6,000 rpm but I cant afford a spindle rebuild anytime soon. It probably will take it but I would rather not take the chance right now. And I know I will just have to play around with things and find out what works best for me. The real reason I started this thread was to figure out what to do with the finish pass feed speed and rpm. I am thinking you want to up your RPM a little and slow down your feed but I am not sure.

thanks
 
Chip Load = Diameter/200

Is that a typo? With that formula, that's .0025 ipt for a 1/2" endmill. I run nearly double that in a slot. In stainless. On a Haas. And .0025 ipt is a FINISH pass in aluminum!

No, its not a typo, remember these are rules of thumb for a starting point. If things are going well, crank it up until the machine starts complaining. As you found with a good quality endmill, rigid mill and good workholding, twice this starting point is achievable.

Paul T.
 
At that spindle speed and that radial engagement, 70ipm or there about.

The smaller your radial engagement is, the faster you feed it due to chip thinning.
 
You should run your finishing pass at the same RPM as your roughing pass. You should reduce the chipload for your finishing pass. However, you want to run an end mill with more flutes for finishing than for roughing. Therefore, your feedrate will be close to the same as roughing. For example, roughing in Aluminum you would want to use a 2 or 3 flute end mill. For finishing you would use a 3 or 4 flute end mill. Speeds and Feeds would look something like this with 6,000 RPM spindle.

2 Flute Rougher
6,000 RPM
0.012" clpt
6,000 X 0.024" ipr = 144 IPM

3 Flute Finisher
6,000 RPM
0.008" clpt
6,000 X 0.024" ipr = 144 RPM
 
Think about there being different "sweet spots" for what you're trying to accomplish:

SweetSpots.jpg


As you can see, if your goal is Material Removal Rate--fastest feeds and speeds.

If it's Surface Finish, keep the speeds (rpms) up, and reduce the feedrate.

If you want max tool life, ease off a little on both.

As you can also see, there are penalties for going too fast, but also (surprising to most) for going too slow. If you allow the chipload to fall below the radius of the cutting edge (not always obvious when that is, BTW!), your tool will start to rub and burnish the work instead of cleanly slicing into it. That heats the tool and radically reduces tool life. Too many rpms (too much surface speed) and you'll kill tool life as well.

The chart is from my course on feeds and speeds:

CNC Milling Feeds and Speeds Cookbook and Tutorial

Lots more there to help figure out these simple cases as well as much more complex cases.

Best,

BW
CNC Cookbook: Software and Information for Machinists
 
bellinoracing said:
I would run it at 6,000 rpm but I cant afford a spindle rebuild anytime soon. It probably will take it but I would rather not take the chance right now. And I know I will just have to play around with things and find out what works best for me. The real reason I started this thread was to figure out what to do with the finish pass feed speed and rpm. I am thinking you want to up your RPM a little and slow down your feed but I am not sure.

thanks
Click to expand...

Part of the deal is that stuff breaks. If you have no plan for dealing with it, you'll lose your shirt when it does happen, and it will. Something will break, and it may well break running at 4k.
If it makes more money to make parts faster, then it makes money to cover repairs, otherwise you are just wasting time. If you need to run fast you need to take this stuff into account.
If you don't need to make the parts faster, then don't. Get good first, then get fast.
 
PaulT said:
It that's a carbide endmill you're spinning way slower than you should.

Below are some basic guidelines for setting your speeds, feeds and depth of cuts.

Most of this was stolen liberally from Stanley Dornfeld who gave me these basic recommendations when I was starting out.

These ares starting points, adjust your feed rates up or down depending on how your machine is taking it.

Paul T.

Figuring your SFM (Surface Feet/Minute, which will determine your RPM)

SFM with HSS endmills
Stainless Steel 40
Mild Steel 100
Brass 300
Aluminum 400

With carbide endmills, multiply those settings by 3 as a starting point, so:
SFM with Carbide Endmills
Stainless Steel 120
Mild Steel 300
Brass 900
Aluminum 1200

Then:

RPM = 4 x SFM/Diameter

Now to find your feed, first calculate your chip load. A reasonable starting point for the chip load is to divide your endmill diameter by 200.

Chip Load = Diameter/200

Then to calculate your Feed Rate:

Feed Rate= RPM x Num of Teeth x Chip Load

So for example with a 1/4" HSS endmill in steel, your RPM should be:

RPM = 4 x 100/.25 = 1600

Your feedrate should be:

Feed Rate = 1600 x 2 x .25/200 = 4 ipm

This a starting point, I usually crank down a little from these recommended settings to see how the machine responds.

As far as your maximum depth of cut, on smaller machines this is often determined by the available spindle HP you have. However if the machine is up to it, I use the following guidelines for max radial and axial cut (borrowed from Stan Dornfeld):

Slotting: Cut Depths
6061 Aluminum, Brass - 1/2 endmill diameter
7075 Aluminum - 40% endmill diameter
Mild Steel - 30-35% endmill diameter
Stainless Steel - 25% endmill diameter

Rough Profiling Tool Overlap: 70% endmill diameter or less
Finish Profiling Tool Overlap: 3% endmill diameter

Plunging Rates:
Take the normal slotting feedrate and divide by the number of flutes.
Click to expand...

Not trying to revive an old thread here but I just wanted to say that your explanation was sooooooo much easier to understand and got me on the right path. Easier to understand than what I found on cnc cookbook or other sites that spent way to much time explaining something that is very simple. Not knocking cookbook or others but I have a short attention span so long explanations buried within an even larger sales pitch typically lose me before I get to the middle leaving me confused. That said there is some good info on cookbook that has been very very useful too. :)

Thanks for posting this and thanks to all the other sources out there for posting this and other information. You have helped me go from never touching a CNC mill to making Money in 10 months! Now to pay off my s500x1!!!
 
bellinoracing said:
In general when cutting your finish pass do you want to go faster, or slower, or the same speed as your roughing speed? Part of me thinks faster, but part of me thinks slower. I am guessing probably slower so that it cuts the hole on size and tool flex is not an issue(I am only cutting .015 on my finish pass so I would be very surprised if any tool flex would occur but I am not positive). I am using a 1/2 three flute finish endmill to cut aluminum. I am turning it about 3,000 rpm and moving about 25 ipm for roughing and finish passes. Its cutting very well but I thought maybe we can cut our time down a little, improve cutter life, and finish quality. I think I may step rpm up to 4,000 but what should I do with my roughing and finish feeds. Its niagara coated endmill for aluminum and I am using a Haas TM1 with a 6,000 max rpm. I could turn it 6,000 but would prefer not to run it at max speed constantly.

Thanks
Click to expand...
.
.
finish cuts can often be run at a higher rpm providing vibration from cutter, the machine vibration, and part vibration is not causing a vibration finish pattern that will be unacceptable.
.
also higher sfpm and ipt causes more wavy finish that can often be measured with a .0001" indicator and if end mill deflecting you can easily get tapered edges that is toward cutter tip dimensions are less from cutter bending under load which with bores can often be measured .001 smaller size farther into bore
.
short tool length, rigid machine and part and you often can run 200 to 1000% faster as long as chips not getting recut piling up
 
If you are selling the parts speed up the spindle or you will never be able to afford a replacement spindle. If that makes sense.


Sent from my iPhone using Tapatalk
 
D Nelson said:
If you are selling the parts speed up the spindle or you will never be able to afford a replacement spindle. If that makes sense.


Sent from my iPhone using Tapatalk
Click to expand...

Just for info, your TM1 has the same spindle as the Minimill. It is limited to 6000rpm from the factory for longevity. I have ran mine for hours and hours=days and weeks on end at that speed with zero issues. Good luck
 
You must log in or register to reply here.

Similar threads

S
HDPE tooling for best surface finish
2
Replies
20
Views
682
George-H
G
A
Wall finish with dormer S903
2
Replies
20
Views
806
Antoine21130
A
U
Aluminium 6061/6082 on profiling surface finish
2
Replies
36
Views
2K
usolutions
U
M
Aluminum endmill, floor finish
2 3
Replies
48
Views
3K
rjwalker1973
rjwalker1973
B
EN40
Replies
5
Views
264
guythatbrews
G








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top