So I know this topic comes up a lot but I'm still confused. My question regards cutting feeds and speeds in 6061 and 7075 aluminum. the majority of our machining is done on a Haas Mini Mill. During roughing i have an rpm of 2400 and a feerate of 11 (guessing its inches per minute). Now that gives me a chip load of 0.0011. It is about a 75% stepover cut at 0.125 depth. Im trying to get the fastest safe possible cut. now as i speed up rpm and feedrate to maintain chip load my spindle load meter skyrockets and im not real sure what a "safe" Load would be. Any help in these areas would be greatly appreciated. oh the tool is a 1" carbide 4 fluted endmill.
Wrkn, you need to develop some understanding on how to set your speeds and feeds for various materials and cutter types. One way is to use one of the PC or online based speed/feed calculators. I use the rules of thumb below to get me close, and dial in from there on how the machine is responding.
Figuring your SFM (Surface Feet/Minute, which will determine your RPM)
SFM with HSS endmills
Stainless Steel 40
Mild Steel 100
With carbide endmills, multiply those settings by 3 as a starting point, so:
SFM with Carbide Endmills
Stainless Steel 120
Mild Steel 300
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 your 1" four flute carbide endmill in 6061, your RPM should be:
RPM = 4 x 1200/1 = 4800
Your feedrate should be:
Feed Rate = 4800 x 4 x 1/200 = 96 ipm
This is 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, and with a 1" endmill the MiniMill will probably not be able to make a cut as big as the guidelines show. However if the machine is up to it, I use the following guidelines for max radial and axial cut (borrowed from Stan Dorfeld):
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
You can also use the HP calculations below to estimate how much HP a particular cut will require:
MRR (Cubic Inches per Minute) IPM x WOC x DOC
Horsepower Consumption = MRR x mf
mf - steel = 1
mf - gray iron = .65
mf - aluminum = .3
So with your 1" endmill in aluminum at 96ipm, a slotting cut at 1/2" depth would require:
HP = IPM x WOC x DOC x mf = 96ipm x 1" x 0.5" x 0.3 = 14.4 HP
Keep in mind that his is HP at the spindle, which means the motor has to be capable of supplying even more than that.
With roughing aluminum with carbide, I throw SFM out the window.
Take a look at your machine's spindle power curve and find the rpm range where the machine makes it's highest POWER, then look at the maximum rpm that the machine can hold it's maximum power. Use this spindle speed for roughing aluminum.
Use your spindle's maximum rpm for finishing aluminum.
Depending on your part geometry, it is typically efficient (in several regards) to take a deeper axial cut with a much smaller stepover. I generally plan for 30-40% stepover for roughing.
My WAG/ROT is to plan for .3 hp per cubic inch of aluminum removed per minute. Having said that, if you have 10 hp on your nameplate, you should be able to take 33 cubic inches/minute at roughly 100% spindle load.
I typically plan for 70-90% spindle load when roughing. You have lots of room to grow.
2 great replies.
FP really nailed it when trying to make time on a low power machine.
Not much to offer other than experiment and do some searches here.
The tools can make a big difference too. You need the right geometry and either no coating or the right coating (ZRN).
If you run into chatter problems then you need to change your approach or your tool or both. A tool like the Variable helix rough/finish mill from LakeShoreCarbide can make a wimpy machine like a Haas look like a hero.
I have been using Destiny Tool. They have are some serious material removers. They very free cutting allowing for high feed rates and a very good selection for long and relieved are very good as well.
I would recommend giving them a try. I use them in 2024, 6061, 7050, 7075. You can even cut dry with there Stealth and Zirconium coatings.
DESTINY TOOL - online cataloge and shop
I use a brand of end mill that is local made here in Mississippi by a place called GLC manufacturing. But even with accupro brand mills, I usually run between 6000-7000 RPM and between 30-50 IPM with about a .150-.250 depth of cut. I always get the carbide ZrN coated endmills. I love machining aluminum cause you can hog the crap out of it.
Originally Posted by PaulT
Wow awesome post. Just saved that for later.
I've been pretty good at "guessing" speeds and feeds for endmills which come out very close to the formulas you suggested but what about calculating cutting info for drills? General rules?
Peck = (1/2 drill diameter?)
Feed = ?
Speed = ?
Try Bob Warfield's Gwizard.
GWizard: A Machinist's Calculator
Bob's a member here.
Not necessarily. Most machines if not all will have a set time allowance that it can run at 100%. My Mazak 50 taper 30 HP VMC will hold 100% but only for 30 mins.(as per Mazak Rep) It also has a time range to run in the yellow.(not sure what it is)
Originally Posted by sniper1rfa
i just tried posting almost identical questions but i had to leave the computer for a while and it must have timed out or something, i'm just glad i don't have to rewrite everything.
x2 on the drilling feeds. and how about feeding in z with an endmill?
my machine is a boss 5 with mach 3. i'm working on my first project and wore out a hss endmill pretty fast. i wasn't too sure on feeds so i took it easy because i don't want to loose steps and trash this part. but i think i was moving too slow and just making alot of heat
Drilling feeds/speeds: get from the tool manufacturer.
For instance, don't try 70ipm at 12k rpm with a 3mm drill from just any manufacturer. (and BTW, that is slower than what is recommended...I'm just a chicken)
Originally Posted by dstryr
The guidelines I showed work well for drilling also, although typically you can be more aggressive on the chip load/feed than the guidelines show.
For example, lets calculate the feed and speed for a 1/2" HSS drill bit in mild steel.
RPM = 4 x SFM/Diameter = 4 x 100/0.5 = 800 RPM
Chip Load = Diameter/200 = 0.5/200 = 0.0025"
Feed Rate= RPM x Num of Teeth x Chip Load = 800 x 2 flutes x 0.0025" = 4ipm
But with drilling, this feedrate will be on the conservative side, look to bump it up if the machine can handle it.
Regarding pecking, I follow the rule to go 2 x Diameter on the first peck, and the 1 x Diameter for each peck after that. Note that like a lot of the info in these guidelines, I believe I "borrowed" this suggestion from one of Stan Dornfeld's posts.
Keep in mind that these guidelines "get you in the ballpark". If you are making a lot of parts, I'd go to the manufacturers websites for the cutting tools you are using and look at their recommendations. Keep in mind that these recommendations typically assume a perfectly rigid machine and workpiece, but they can still be useful to look at.
Fpworks also had a good point regarding maximizing your metal removal rate (MRR). If the speed suggested by the guidelines puts you too far out of the range where your machine supplies maximum HP to the spindle, you could end up with a lower MRR than if you back the RPM down to the HP max for your machine.
This is something you have to play with on your machine. On my machine I run out of rigidity on roughing cuts before I get HP limited, so I typically run at the guidline RPM settings and then adjust the feed until the machine complains too much.
amishmafia00, straight drilling with an endmill is something you want to avoid if you can, they just don't cut that efficiently as a drill and you have to be very careful with chip evacuation to keep the flutes from getting packed. If you can, use a normal drill to make that first deep hole.
Originally Posted by amishmafia00
In general if I have to go straight down witn an endmill, I'll go at about 1/2 the feed that the guidelines suggest. I strongly prefer helically interpolating the hole if that's possible, this is a nice way to go if the workpiece has both pockets and holes, it minimizes tool changes. When ramping during interpolation, I usually ramp at 5 degrees and slow the feed down during the ramping by around 20%.
Paul, a good guideline is to take whatever the feed should be and when plunging, divide it by the number of flutes on the cutter. So 1/2 works for a 2 flute in aluminum, and so forth. This was recommended to me by one of the manufacturers and is the algorithm G-Wizard uses to determine the plunge rate.
Originally Posted by PaulT
CNC Cookbook: Blog
PS Scud, thanks for the call out!
Thanks Bob, that's a good tip.
Originally Posted by BobWarfield
@ Paul T.
Originally Posted by PaulT
First off, let me heartily thank you for this post. I had been beating my head against a wall for quite some time before I found this forum. All the equations I had found looped back and forth between each other. For example, from the Haas Machinist's CNC Reference Guide, "SFM = 0.262 X DIA X RPM" and "RPM = 3.82 X SFM / DIA". How can you find one without the other?! Your post finally gave me an easy starting point.
Secondly, I'd like to ask your permission to directly qoute this post for training purposes. I work in a student run machine shop at Purdue University and I do a lot of the training for our new employees. This post has given me much needed information in an easy format for training people who don't know anything about machining.
Lastly, I was wondering what is the acronym "mf" which I have highlighted in green above from your post?
Thank you so so much,
Drills.. Screw machine length and split point, two flute.
Originally Posted by dstryr
Basic chip load per flute. 1.6% of the diameter, near 3% including both flutes.
*At 300 rpm move the drill's diameter, decimal point one place to the right. .250 drill 1/4" 300 rpm, inches per min. feed rate = 2.5 IPM.*
*3000 rpm move 2 places to the right. One half inch drill 1/2" drill = 50 inches per minute.*
If the material will allow you to go 9000 rpm (3 times 3000) , then 150 IPM. This keeps the chip load the same.
So now you have a .040" drill, and you have 5000 rpm available use the 3000 rpm standard (move decimal 2 places to) 4 ipm and then 5000 rpm/ 3000 rpm = 1.6 * 4 ipm = 6.4 IPM.
In other words you can pick any drill off the chart and use its decimal diameter and you can calculate the feed rate @ the RPM you want to use. 300 rpm is 10 times slower than 3000 rpm. These rpm's just come out even with the decimal numbers and the feed rate. You can if you want, use the chip load per flute percentage of the drill diameter times 2 (both flutes) times your RPM. It's the same thing,
Calculate the RPM as you would for an end mill. I've also used this method for most all materials. One of my successes was a .0130" diameter drill, drilling 12 diameters deep in 316 SST. 1/2 diameter pecks 2000 rpm. ,, I only had the nerve to do it once. Materials which are not strong enough to support the drilling will be difficult. OFHC soft Copper is one of these. I cut the feed back to 1/3 of normal. Sometimes the material will become warm with the cutting and soften. Keep the RPM down and you may get away with it.
I have used this formula from 1" drills down to .010" drills.
Where did you durive 200 from in this formula? I'm new to the machining world and like it a lot.
(Chip Load = Diameter/200) This is a great post and learned a lot from it.
Also check out my calc
FSWizard - Free Advanced CNC Speed and Feed Calculator
I am not only a member here, but also a machinist