Results 1 to 20 of 29
Thread: Determining Depth of Cut
08-12-2011, 11:17 AM #1
Determining Depth of Cut
i am curious what other experienced machinist use to determine an end mill depth of cut.
for example i use the 2x longer then 2 square (2x2) rule. that is a end mill sticking out 2 times longer then 1/4 depth of cut.
i ordered 1/2" end mill with 1.25" LOC but received 1.625 length of cut. Formula says with aluminum and HSS end mill
0.80" stick out from collet then 0.684" max depth of cut
1.40" stick out from collet then 0.223" max depth of cut
1.88" stick out from collet then 0.125" max depth of cut
even at 0.100" DOC and climb milling i was getting vibration marks with 0.005" to 0.008" thick chips. Of coarse i could slow feed and lower depth of cut but even doing this vibration marks were still seen.
my point is i never realized before how much a slightly longer end mill could seriously effect machining rates. at first it would appear better to have a longer end mill just in case you might need it but if you do not need the length it can really increase the time to machine a part.
just wondering if anybody has studied this before?? you would think during a war time when producing arms like during WW2 somebody would have studied this. Or the Automakers would have studied this, although they might not publish the info and treat it as a trade secret.
...... Just wondering what formulas others use other than trying things and increasing til vibration is too severe. But doing this you might not realize the vibration is more from the end mill length than anything else.
08-12-2011, 11:32 AM #2
Two words, book title:Machinery's Handbook
08-12-2011, 01:07 PM #3
I use the shortest emdmill I can.
Rigidity goes down eponetentialy the further you stick out.
Always try to maximize rigidity in your set ups. A little bit here and a little bit there adds up. It's common for inexperienced guys to not appreciate how much of a difference rigidity makes. For example, they might stick their work piece extra far out of the lathe chuck because they don't want to risk hitting it. Or they'll use an extra long endmill to lessen the risk of hitting the tool holder or whatever.
Rigidity makes everything easier.
08-12-2011, 01:10 PM #4
It's always best to use the shortest possible end mill. The current trend is towards full depth cuts and very low radial engagement, though.
My formula is typically "set radial engagement to desired specs for tool, then increase DOC until power runs out". It works great.
Texas Tim liked this post
08-12-2011, 01:55 PM #5
Rigidity of a beam (end mill) decreases by the power of 3 as length increases.
Rigidity of a beam (end mill) increases by the power of 4 as diameter increases.
I'd be interested to see any formulas for calculating end mill defection. It should be straight forward based on material machinability ratings.
cncbrit liked this post
08-12-2011, 02:33 PM #6
That's why my Power Center has the power of 65,000 Dremels
Another note, you need to have the full dia of the cutter at the collet cutter interface , if you don't, you will set up a load point that will help snap the cutter.
08-12-2011, 03:54 PM #7
GWizard Machinist's Calculator will let you play with these numbers.
You can see how much deflection various combinations of stick-out, tool diameter, axial and radial depth of cut, tool material, work piece material, etc... will create.
In terms of machining dynamics, this presentation that Boeing did at IMTS in 2008 is pretty interesting:
BLUESWARF | Boeing High Speed Machining Seminar
08-12-2011, 05:20 PM #8
I use three flute end mills only. (job shop)
When cutting a full width slot you use the full diameter of the tool, maximum pressure when milling. Standard length end mills. When I'm really serious, I use stub length for extra rigidity.
The slotting cut
I divide the diameter by 120 to establish the chip load for the tool. I figure the gullets (flutes) are wide enough for the particular chip load. This is good for 80% of the materials I cut including, sst, the aluminums, and regular steel. The only time it was over kill is OFHC copper. Reason: The copper itself wasn't strong enough to support the cutting pressure and it was flowing. In general the chip load is the same for all materials. I had to lighten up about 2/3rds on the chip load for the OFHC Copper.
However! The depth of cut may vary from 25%- 50% of the end mill diameter. The tougher the material the shallower the cut. I had 6061-T6 aluminum near the 50%, but 7075-T6 had to be near 40% or it squealed because it's a much harder material.
The roughing cut
I divided the tool by 80 for the chip load. Why? Because the cutting pressure was only 2/3's
the width of the slot cut. Therefore the tool can stand a 50% heavier feed rate. Which means when cutting a pocket, if you start in the middle and make the slot cut at it's chip load, then when you begin to unwind the rest of the pocket you can go at a 50% faster feed rate. You don't bind yourself to one feed rate for the slot cut all the way through milling the pocket.
I leave the finish cut to you.
The math I used may be confusing. Slot cut divide by 120, rough cut divide by 80, You add
50% of 80 to get 120. I'm trying to keep the total cutting pressure ( chip load x percent of end mill in the cut x feed rate ) the same for the two types of cut. I hope this makes sense.
I've had good luck using this, and it's pretty productive.
When sharpening the tool just grind off the dull end and re-point. You still have a full size cutter and its original cutting geometry.
08-12-2011, 09:17 PM #9
current Excel speed and feed calculator
thank you, i will study everybody recommendations
my latest Excel speed and feed and depth of cut calculator
1) using logic statements (IF THEN OTHERWISE) to override formula on depth of cut increase with end mill shorter than 1.5 times diameter
2) feed and chip thickness max limit currently set at 0.015" chip thickness
3) DOC limit even when Machinabilty rating of aluminum or plastic is used to limit max recommended depth of cut to 1.5 times diameter. Plastic can take very large depth of cuts
4) color coded cells so grey cells are not to be changed, blue are cells for inputting cutting parameters, yellow for end milling and green for side or radial milling, orange is for calculating DOC % for a particular DOC
5) added a row for calculating horsepower and metal removal rates for partial end mill width cuts
6) added a end mill shank diameter column that reduces DOC recommendations for shanks smaller than cutting diameter and a logic function that does not increase DOC if shank is bigger that cutting diameter
7) added a formula to reduce DOC as flutes increase. 10 flutes increases hp requirements 10x times so a partial reduction in DOC seems a good ideal so to not overload cutting with high vibration from too high a load. For example a 3" shell mill 10 flute with a R8 shank cannot take the load of a 3" shell mill with a NMTB 40 taper so some sort of formula taking into account shank diameter and number of flutes seems a good ideal.
8) added a column on end mill shank material as solid carbide end mill is more rigid than a carbide insert end mill with a steel shank.
Excel calculator is a work in progress. It is free, easily adapts and software is free if using the free Open Office Calc program.
08-12-2011, 09:39 PM #10
........yes deflection will increase ( with decrease in finish) but end mill does not usually break. i found when using in formula decrease to the power of 3 decreases max recommended depth of cuts too much. end mill can take the DOC but vibration does increase. understanding all the Physical laws is difficult. i am sure there is a reason longer end mill can deflect without breaking but vibration will limit tool life.
also taking into account a shank diameter smaller than cutter diameter and also increased number of flutes and the horsepower increase (vibration) requires thought on formulas. For example a 3" diameter end mill with a 3" shank can take far more than a 3" shell mill with a 3/4" shank.
as i have told Engineers before the Laws of the Universe do not care if big bosses does not like them. sometimes Engineers want to ignore for example part expansion in dimension from higher temperatures. but the Laws of the Universe do not care what an Engineer wants, they are what they are.
......... but it can be difficult figuring out the theory and the why things happen
08-13-2011, 02:47 AM #11
My understanding has alway been that an end mill's rigidity doubles with every diameter you reduce the overhang. For example, if you have a 1/4" end mill sticking out 1.00" and then you reduce it to 3/4" stick out (reduction of 1 diameter) then you just doubled the tools rigidity.
Last edited by BKGUY; 08-13-2011 at 02:49 AM. Reason: Spelling
08-13-2011, 08:18 AM #12
08-13-2011, 08:44 AM #13
08-13-2011, 09:28 PM #14
1/4" end mill and stainlless and aluminum
what i get using current excel calculator formulas
1/4" carbide end mill and machining stainless
1" stickout DOC 0.007"
3/4" stickout DOC 0.012"
1/2" stickout DOC 0.027"
1/4" carbide end mill machining aluminum
1" stickout DOC 0.058"
3/4"stickout DOC 0.103"
1/2"stickout DOC 0.232"
because i use the machinability rating in the feed formula
Stainless is about 0.35
Aluminum is about 3.0
........ machinabilty rating is a rough horsepower ratio to machine a cubic inch of material per minute so in general stainless requires 9x the power to machine and thus DOC is reduced and as cutter will deflect more trying to take a large DOC that might be easily done with a softer material.
........this is why some people trying to take deep depth of cuts might get away with it for some metals but might have much more trouble with harder materials
dstryr liked this post
08-14-2011, 10:24 AM #15
Lately when machining stainless I'll go Full DOC with a 1/4 or 3/8 em (2xd deep). and us a 5-10% step over to keep the endmill from only wearing on the bottom...Gotta use the whole length of the cutter...
08-14-2011, 11:54 AM #16
update so far on depth of cut calculator
updated Excel Speed and Feed, DOC and Horsepower calculator
1) after testing a 1/2" HSS EM sticking out 1" with 2 flutes can cut 0.117" in steel and it will cut 0.029" DOC when sticking out 2" so
if 2x more sticking out reduced DOC 2x2x2=8 then i would only be able to cut 0.015" thus it follows more the 2x longer 1/4 DOC rule. maybe because a end mill has flutes cut into it that it does not follow the 2to 3rd power rule but more the 2 to 2nd power rule
2) Feed of Dia/120 does not work well with larger diameter cutter and with all alloys i use
Thickness Factor (100 is max) x Diameter x (Machinability Rating + Calibration Factor) + 0.0005 (minimum feed no matter what dia) / shank diameter
and also formula has feed override to limit feed to 0.012"
if no override then 3" dia cutter feed is 0.066" thick chip at 6.3" DOC 2 flute with aluminum
by using flute number to lower DOC
by using ratio of shank dia to cutter dia to lower feed i get
3" dia cutter 10 flute and 3/4" shank i now get
DOC 0.176 and 0.004" thick chip at 100% max feed
with stainless (and different Machinabilty rating number)
DOC 0.021" and 0.0014" thick chip at 100% max feed
.......formula with 10 flute, 3" dia cutter with a 2" shank say roughly a 40 taper then i get with stainless
DOC 0.146" and 0.0098 thick chip at 100% max feed and also taking 47 hp at 300 SFPM (382rpm)..... so you maybe understand why the reduction with a 3/4" shank and 3" dia mill compared to 2" shank and 3" diameter mill
....... without some sort of reduction the numbers go way more than a cutter can take if you do not watch the shank diameter.
3) i will now use 3 now for carbide shank material. this will increase DOC 3x for a solid carbide end mill compared to a carbide insert on steel shank end mill but i hesitate to increase DOC 3x for solid carbide because it is brittle and will loose a cutting edge more easily with a vibration that a HSS cutter could tolerate..... so shank material is in formula next to shank diameter
because a 1" dia 1" shank EM can take a higher DOC than a 1" dia 5/8" shank EM
4) calculator has row for side (radial) milling to as well as normal end milling. side milling rows show high DOC and a partial or small stepover and calculates chip thickness for chip thinning that happens at small stepovers.
like i said Excel speed and feed, DOC, Hp calculator is a work in progress. as i notice things with different dia cutters and shank diameters and different materials being cut i modify formulas.
.........For example feed or chip thickness limit i added because a feed with a chip thickness over 0.012" leaves a rough surface...... although with cutter corner radius i suppose you could use high feed and get a good finish
08-14-2011, 01:13 PM #17
08-15-2011, 03:01 AM #18
I chose depth of cut first, and then figure width of cut using G-Wizard's Cut Optimizer to choose a cut width that keeps deflection within limits.
Most of the tooling mfg's discourage more than 0.001" deflection on carbide (HSS will take more as it is less brittle). It's hard to get much accuracy with more than that anyway. G-Wizard scales that figure back on small EM's because they can't take as much deflection.
That 0.001" is a roughing number. Try for more like 0.0002" when finishing.
There's two issues with the deflection. First, eventually you'll deflect far enough to break the tool. That's usually going to be much more than these limits. Second, deflection denotes vibration and chatter. Those are the effects that are more likely to chip, break, or otherwise kill your tool life. Imagine a spindle with 0.001" runout or more. That's effectively what a cut with so much deflection is to the cutter. Not a happy thing.
Why chose depth over width of cut? So you can get more of the flute involved instead of just the end of the cutter, so you can avoid as many levels as you can when pocketing or profiling, and so you can take advantage of chip thinning to speed up your work. The cutter will experience better chip clearing and cooling with lower widths--that's part of the foundation of the HSM toolpaths, the other part being constant loads instead of overloads in the corners.
Optimizing all these factors is a pain, but it makes a difference.
08-15-2011, 08:38 AM #19
Be honest with yourself, make a list of them, as obscure as they may be, address them all and you will get somewhere, and have something useful.
Try generating a table of speeds and feeds for the same cutter, then work out the one that has the least number of chips per cubic inch removed.
08-15-2011, 08:42 AM #20
length to DOC progression (shorten to 1/3)
for end milling (not side / radial milling)
effects of end mill length to depth of cut, that is if shortening stickout by 1/3 does end mill depth of cut increase by 3x3=9 or 3x3x3=27"
1/2" HSS end mill 2" stickout max recommended DOC 0.029" in 1018 Steel
0.029 x 9 = 0.261"
0.029 x 27=0.783"
so if to 3rd power with end mill 0.66" stickout you can take a DOC 0.783" if it stuck out that far?
if to the 2nd power 0.261" DOC in steel with a 1/2" stub length end mill sticking out 0.66"
....... because i use Excel calculator i can change a parameter like stickout and press enter and everything recalculates in a millisecond. if i change things like end mill diameter to 3" or end mill length stickout reduced to 1 diameter (1/2" dia EM sticking out 1/2") i was getting some crazy DOC figures. formulas now are closer to what really happens. DOC increase with shorter stickout i stop at 1.5 dia length (1/2 dia then 3/4" stickout)
something else to consider and i added to the formulas is reducing feed automatically for too many flutes on too small a cutter.
for example 1/4" rotary file with 12 teeth...... good luck upping the feed 6x more than a 2 fluter as the flutes will clog with chips and friction will quickly destroy an end mill.
....... also why my calculator reduces DOC for more flutes too. keeping the same DOC AND upping FEED 6x when going from a 2 flute to 12 flute 1/4" end mill you will put 6x more horsepower on to the shank and more easily snap it off.