Endmill Breakage Feeds/Speeds/Depth of Cut

I'm fairly new to programming and am seeking some advise to prevent breaking small endmills. I've been trying to cut a pocket in steel with a 1/8" four flute endmill x 1/2" LOC Carbide endmill. I know I'm shy with spindle RPM with a max of only 4200 RPM but set up the feeds to accomodate a .001 feed per tooth cut. Problem is the equations I've used to calculate my feeds based on spindle RPM and tooth load don't say squat about depth of cut.

My problem is that I can only take very a very light depth of cut, .020 or less, otherwise I'm destined to break an the endmill. How is depth of cut, especially for small slender endmills, factored into figuring out feeds and speeds used.
Your insight and experience appreciated. Learning the hard and expensive way by breaking carbide is getting old.

ATMO, assuming garden variety steel like 1020 or something, you need to reduce your feed down to around .0003 to .0005 per tooth for an 1/8" end mill with a 1/2" LOC. An 1/8" endmill with a 1/2" LOC is a whispy affair. If you can rough out the pocket with a bigger cutter, do so. If you can use a stub length cutter, do so. If you're plunging into the part with the cutter, stop and drill a hole to use as a start position.

I'm fairly new to programming and am seeking some advise to prevent breaking small endmills. I've been trying to cut a pocket in steel with a 1/8" four flute endmill x 1/2" LOC Carbide endmill. I know I'm shy with spindle RPM with a max of only 4200 RPM but set up the feeds to accomodate a .001 feed per tooth cut. Problem is the equations I've used to calculate my feeds based on spindle RPM and tooth load don't say squat about depth of cut.

Click to expand...

you wont be able to do much with that size cutter going that deep, especially if its carbide, you are already at 4 times diameter for loc.
what you need to do is either
1. use 2 1/8 cutters, use 1 to rough out the pocket going say .04 deep on each lap of the pocket, then finish to size
or... this is the better option and the one I'd use
2. use a 1/4 dia cutter to rough out the pocket, then relive the corners by plunging at the corners about .004" clear of the profile with your 1/8 cutter, then finish the profile.

The other thing to remember is that although carbide is very wear resistant, it does not 'flex' very well, so it could be the increased cutter loads when entering the corners is causing the cutter to break... HSS cutters sometimes work better in this situation because they can 'flex' more than carbide

Hope this gives some handy hints

Boris

.500 LOC ?
is that the same as .500 DOC ?

if so... WOW thats deep for .125 em...
You crazy man!!!

Ussually i setup .001 per tooth on a HSS .500 dia em... with a .125 DOC

So... if you are at 1/4 the diameter of the em... i would cut the speeds to 1/4 as well...

maybe .0002-.0003 per flute...
.125 DOC...

At 4200 rpm that would be a feed of 3.36 ipm to 5.04 ipm

Try that with the .125 doc...

Might be slow, but you will save the em ...

Boris and Solar, you guys need to read more carefully what was posted, he said he was taking a 0.020" DOC with a 1/2" LOC endmill, and even with that still breaking endmills.

As Anvil pointed out, you don't want to use a long LOC endmill if you can avoid it as it makes the endmill less stiff. Can you use a shorter (1/8" or 1/4") LOC endmill?

Also, are you trying to cut a 1/16" radius (perfect fit with a 1/8" endmill) in the corners of the pocket? If so this could be causing the breakage, you need to make the corner radius slightly more than than twice the endmill diameter to avoid chattering problems.

If I was starting from scratch on this setup, I would go for 300 sfm for carbide in mild steel and calculate the best RPM as:

RPM = 4 x 300 sfm/.125" = 9600 RPM

However, you can't spin that fast, so we set the RPM at your max, 4200.

I use the following formulas and guides to calculate the chip load per tooth and thus feed rate. These were borrowed from Stan Dornfeld's posts on various forums.

PT CUT DEPTH NOTES

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

FEED/SPEED FORMULAS and NOTES

RPM = 4 x SFM / (Tool Diameter)

Chip Load = Tool Diameter/FIN
FIN - Slot,120 Rough,85, Finish,70 Plunge,500

Feed Rate = RPM x Chip Load/Tooth x Num. Teeth

In your case:

Chip Load = .125"/120 = 0.001" (when slotting)

Feed Rate = 4200 x 0.001" x 4 = 16.8

Cut Depth = .3 x .125" = .0375"

I find these numbers give you the maximum point you could run with, I generally start with my feed rate half of what is predicted and speed up from there until the cutter or machine complains. I would expect that if you use an quality endmill with less LOC you should be able to machine in the ballpark of the numbers above.

Paul T.

thanks paul...

first, what is LOC ?
and his max rpm is 4,200 not 4,800 by the way...

Anyway...

wont the em break more easily if he cuts with just the tip ?

Seems like a deeper DOC would help ... no ?

LOC?

i think he means flute length

G_99

I would rough the pocket out with a 1/4 or 3/16 then go with 1/8 plunge corners and profile to clean up.

Solar, LOC stands for Length Of Cutter, its the full length of the cutting edge on the side of the endmill and thus the maximum possible DOC.

I find the rules I showed above work pretty well as a starting point, thus for full slotting in steel 30% puts him at .0375" DOC as a starting point.

I would say if he can't make those numbers as a starting point, something is wrong, and as Anvil pointed out his current endmill being too flimsy with its long LOC is definitely a concern. The other possibility would be excessive runout of the spindle or tool holder, runout becomes an issue with these smaller diameter cutters, if your runout is on the order of your chip load (.001" in this case) you are asking for trouble.

Paul T.

i see, thanks...

I'm with Boris. Usually no reason to rough out a pocket with that small an e.m. Drill an 1/8" hole in each corner, or a few thou smaller if the finish is really important in the corner. Rough out with a 1/4" e.m., then "pick out" the corners with the 1/8" e.m.

IF you can use a 1/2 or bigger to do the hogging, use it...I have used 1/8" EM in 304 SS 2" deep to cut a slot in a cam...no problem...

I appreciate everyone's feedback. I'm cutting a profile into steel plate a tad under 1/4" thick. I'm cutting the pocket by slotting the profile at about 0.020" DOC @ 5 IPM at a time until I cut through to the other side. By doing this the center of the pocket is basically a plug that drops out and really doesn't need to be turned into chips. The smallest internal corner radius is slightly larger than 1/8" endmill, thus the small tool selected to cut the entire profile. My real problem is that I arrived at these numbers by trail and error. I'm looking for smarter way.

I like Paul T DOC guildline as this is exactly what I was looking for. I'm troubled though since the recommended numbers he gave I know for a fact will snap my endmill. Anything deeper than 0.020" and faster than about 6" IPM will break the tool.

The quesion of tool runout is a very good one. The spindle is tight and the tool is held by a DA collet chuck in a 30 taper tool holder. I will check the runout. The cutter is made by Hertel and is coated. Not top of the line but far from Chinese junk as well. No flood coolant but I do have an air nozzle clearing chips.

Others have suggested reducing the chip load. Again I would appreciate a source for how these numbers were achieved. Ultimately I would like to set up the parameters and watch the tool do what it's suppose to.

Is this 1018 mild steel or something else?

You don't need the 1/2" LOC endmill for this job, its adding a lot of flimsyness, switch to a 1/4" LOC and your breakage may go away. Also as suggested above, roughing out the pocket with a 1/4" EM and finishing with the 1/8" will probably be faster, even though it makes more chips.

Paul T.

OK now cutting out sections can be tricky, often when the section being removed pops free it can grab the endmill and break it. It is sort of like running a bandsaw blade back into the kerf...plus that long of an endmill is going flex while your cutting.

DA collet holders IMHO are not the best for holding endmills. Also your machine,holder, tool may not be rigid enough to run optimum rpm/feed...for a puny fadal with anything over say 3/8 endmill typically 150sfm was about top you could get away with on the kind of beat up machines we had.

I have also found that a "normal" endmill, what some call a "finisher" (as opposed to a rougher)...will tend to vibrate at high depths of cut...high LOC is ok if the cutter is only cutting on the side..but when you bury it it starts to hum, and that's bad.(also if it is flexing the cutting end is wandering all over the place when you change cut direction) Any kind of rougher that will fit in the internal profile may work nicer than a "finisher" I have used some designed for aluminum in M42 because they were the only 1/8" rougher I could find anywhere..and it beat the heck out of trying to carve a slot with a normal endmill.

I have also found thru trial and error that for a lot of internal profiles you are going to carve with a small endmill, that you can "drill" to depth with the endmill just fine as long as you feed say .001 per rev (running 150sfm with carbide endmill) This will often save a toolchange which makes the part run much faster. In a blind profile you are going to have to somehow go from a drill point in a pilot hole to the endmill anyway..so it seemed to work fine for me just using the endmill at .001 IPR feed to plunge.


Also I typically ran one tool as rough, and another as finish for close tolerance work, and when you break the rougher, and you will, move the finisher back to it's spot, and put the new tool in as finisher. (this was before I discovered the 1/8" carbide roughers)

Got a picture of the pocket?

A few things from the peanut gallery...

1. If you are cutting the periphery, and letting the slug fall free, you can cut a relief pocket where end mill will finish up, and -nearly- cut the floor free, for that last few thousands that the end mill will finish cutting the slug free.
IOW, I do this a lot, I pre-cut a pocket where the endmill will finish, and also precut almost to the bottom upstream of where the EM will finish.
So that that last little bit of a cut is really light, and once the slug pops free, it -can't- possibly jam against the EM.
Since I did that, we have cut out many tens of thousands of pockets, leaving the slug to fall loose at the end of the cut. Before, it -usually- caused a spectacular crash!

2. Stepping into the pocket, alternate your tool offset from the cutting ceterline.
IOW, we cut a part with a .25' EM. the finish passs is going to be .125" offset. The first cut into the part is shallow, and offset .140" this allows the next pass to cutting air on one side partially, and it cuts much better then following the same path as the first pass. Try digging out a strip mine as you go deeper.

3. If this is production, make your finish pass cut that -last- section loose, to free the slug. That way the rough pass won't let it rattle and jam into the cutter during the finish pass, or worse, get couhgt under it as it ramps in for the finish pass.

4. Failing all of that, I have cut the centers into chunks with a zig zag roughing pass, and with enough coolant pressure, blew them out of the way. For a 1/4" EM, I would checkerboard the center slug into .4" slugs, and they really couldn't jam up, since they had .25 clearance on the back side by the time they came free.
Pete

What i did with my first and only Mill contouring job was...

I took EM passes of .150 deep, untill there was .1 material left...

Then i flipped the part over... And used a Large EM to face that last .1 off... thats how i free up the part, from the stock...

That way you dont break your EM becuase its not sunk down in the material... its just facing the top .1

see

Others have suggested reducing the chip load. Again I would appreciate a source for how these numbers were achieved. Ultimately I would like to set up the parameters and watch the tool do what it's suppose to.

Click to expand...

If you don't have one already, get a copy of the Machinist Handbook. They have speeds & feeds info within them in addition to all kinds of other info for the machine trades. It will be the best $100 you ever spend. Also, if you have a J&L catalog, they ususually have speeds and feeds info in the tech section. You can find lots more on the web. One of the members here produces a speeds & feeds software program that could be helpful to you.

When slotting, I pretty much stick to no more than 1/2 of cutter diameter for DOC and will often reduce that. Bottom line is, always use the biggest cutter you can to rough out the pocket and reduce size only when necessary.

Related to pockets, I never ramp or plunge into a pocket in hard materials unless I can't drill a start hole. You can tell most CAM software to drill and use a start hole when pocketing. Plunging eats more end mills than anything.

Thanks again,

Plunging doesn't seem to be much of a problem. It's the side load on the endmill that seems to be overloading the cutter and breaking at the top of the flutes. A shorter LOC tool would definitely help I'm sure.

As I stated before I'm new at this and I will add this is just a hobby thing for me. I laid everything out in CAD and then manually picked off all the transition points, arc centers, and punched them into the control by hand. Not a complicated part and wound up with maybe 35 lines of code. Programing for different cutter dia , rougher, finish pass would have been just that much more work. still lots to learn I know.

I do have Machinery's Handbook and have the basic feeds/speeds/rpm equations programed into my HP which makes hand calculations a snap. I also recall getting a speed/feed calculator shareware off the web that also provided depth of cut but for the life of me I can no longer find it. Plenty of others with no DOC feature. Unless I glossed over something I never found anything in the handbook that states what DOC works with these equations. So I've been basically inching the knee up for each pass getting a feel for how deep I can go untill the cutter complains or snaps.

I have done similar profile cuts in this same plate material with 1/4" endmill in DA collet holders and haven't had any issues. It's obvious the weakest link is the cutter. I just don't know how predict DOC for wimpy cutters.

I sell a pro version on my website, but since you're a hobbyist, try Googling for ME Consultant 2.0, which is free. It factors in depth and width of cut when doing end milling feed and speed calculations.

The program limits you to a depth of cut of 1.5 times tool diameter. It has no way to account for the decreased strength of extra-long end mills.