Home shop guy w/G-wizard still breaking endmill...

[kvom01]

Or, G-Wizard broke my tool.

The cut I was trying to make is an angled cut 3" long in that piece of 1/2" CRS. At the end, the side cut is 3/16". Endmill was brand-new OSG 4-flute carbide. I set it up to cut in 2 passes .25 DOC. Plugging into G-wizard for the maximum radial engagement, the program gives me:

2353 RPM
308 SFM
Chipload .003
Feedrate 28

However, because of the discussion in an earlier thread on chip thinning, checking that box ups the feedrate to 46 RPM.

So I ran the program at 46 IPM climb milling with the result pictured above (all 4 flutes snapped off). This happened on the second of two parts. I should probably have stopped as the finish was quite poor, but as these parts are just brackets they aren't critical. I used a tangent leadin, so no plunge cutting was done.

That 46 IPM looked scary before I started, but I decided to give it a try as a learning experience, sacrificing the $15 endmill as part of my education.

Any help on interpreting similar g-wizard output for future work would be appreciated. I'm thinking that in addition to the feed rate, cutting the full depth with just the side flutes might have been better.

The second operation on these parts was to have been a facing op across 75% of the piece with a DOC of .300" Using that same end ill with a .25" radial engagement, G-wizard recommends 26 IPM with no chip thinning. Does this sound about right? I'll have to use a 7/16 now which would bring the feed down to 23 IPM.

I could have done these parts with HSS both manualls and CNC, but I really need to get better with the F&S on the CNC mill using carbide.

 

[Tonytn36]

Awful long end mill for that feed, imho... my guess is the break was because the end mill was flexing sideways, which is worse when climbing.

 

[ewlsey]

Awful long end mill for that feed, imho... my guess is the break was because the end mill was flexing sideways, which is worse when climbing.

What he said.

In the gwizard cut optimizer thing there is a field for tool stickout. It defaults to 1. Yours looks like it is at least 3.

 

[[email protected]]

Good 1/2" carbide endmills cost a lot more than $15, and I think that is atleast part of your problem. As alluded to, another part of the problem is how far the tool is sticking out. Even if that's all you had, you should be choked up to as close to the flutes as you can. Looking at the picture, you probably should've stopped as soon as it made the sounds that it looks like it made!

If it was me, I would'a ran a 1/2" 6 flute, 1.25 LOC from Lakeshore Carbide to do the same thing at 4580 RPM, full depth, .030" stepover at 120 IPM. Those are extremely safe numbers and is something you can walk away from if you have something else to do. Same thing for your facing cut at .300 deep, although you could get away with a lot more.

 

[Fred T]

I would have been running a little closer to 12 ipm, because of stick out and the fact that .003 per flute is kind of a lot for a little end mill like that. I use the old formula. 4xcs/d. carbide is three to five times, the results and a little common sense does not hurt either!

Good luck
Fred T

 

[Dave K]

At 15 dollars for an endmill, I'm guessing it's a high speed mill and not carbide? If so, that surface speed is pretty fast sounding to me.
A 300 surface speed sound more like what I would run a coated variable flute carbide endmill.
You just might be asking a little too much for that endmill. If you have more of those and want to try it again, I'd cut that down to maybe around a 90 or 100 sfm.


Oops, sorry. Didn't see that you mentioned it is indeed carbide. Even with that, I usually run about 160 surface speed, which is still quite a bit slower than what you posted.

 

[Glenn Wegman]

What is the vise mounted to?

It looks like it is bolted to something that is sticking up off of the table.

Keep in mind that G-Wizard may provide info for the cutter itself, and does not take into consideration the machine or setup.

Knee mills are FAR less rigid than a bed mill or VMC, and if you have a knee mill with the vise up 6" off the table bolted to a tilting table, the rigidity will basically suck, which will kill even a good carbide end mill.

What's also a bit puzzling is the colorless chips that look to be the size from a file or hacksaw.

Well, maybe not so puzzling, as it most likely chattered the edge right off immediately and then ground it's way through until it broke from deflection.

 

[BobWarfield]

KVOM, let's follow through and confirm all the parameters for this cut.

You say you have a 1/2" 4 Fl Carbide EM. You're cutting 0.25" deep and the max radial engagement is 3/16", though it sounds like it starts shallower on the angled cut.

So if I crank all that in and ignore the cut being shallower, I get a different answer. Without chip thinning I see:

2353 rpm @ 28.237 IPM

When I check the chip thinning I now see:

2353 rpm @ 29.164 IPM

That's a lot less than the 46 IPM you got. 29 makes more sense because you're running 37% radial engagement, so there shouldn't be that much chip thinning.

Some other parameter must be different.

But now let's see how G-Wizard might have helped. The issue of the tool stickout has been raised. I suspect if you'd had 1" of stickout, you'd have gotten away with the cut because G-Wizard predicts tool deflection of 0.0003", which is no biggie.

However, if we crank up the stickout to the 3" that folks are suggesting from the picture, and leave it at 46 IPM, we now get 0.0078" and the deflection value is lit in an angry orange.

That would've been a sure warning you were about to do something you probably wouldn't like, so it's worthwhile to type that stickout in even if you don't plan on using the cut optimizer.

Stickout is a weird thing. Doesn't take much to radically change the deflection, even on a 1/2" carbide endmill which seems pretty rigid to the naked eye, LOL. FWIW, the Cut Optimizer would've suggested no more than
0.050" depth of cut with the 3" stickout and all other things being equal.

Something else is up with how you're doing your settings though because that 46 IPM is a blooper and shouldn't have come up. That's a chipload of 0.0049, which is trending towards aggressive for that EM.

With the 3" stickout if you'd run the 29 IPM I got, your deflection would've been 0.0049, which is still an awful lot to ask for from the EM. Might very well still have broken.

Sorry you broke the tool. Hopefully the stickout thing and tool deflection calculation will be something to look at going forward to save a future incident.

The pic makes the cut look pretty chattery too. Not sure if you'd been able to hear that or not, depends how much noise the spindle makes. Can't hear much over my gearheaded mill!

Best,

BW
CNC Cookbook: Blog

 

[kvom01]

Thanks again for all the comments. I'll get there eventually.

The vises are mounted on the cast iron tilt table because the spindle will not descend close enough for small parts if the vise is on the table. The tilt table weighs about 80 lbs and is bolted down tight. I surface ground it to ensure that the top is parallel to the base. The mill is a bed mill (Novakon NM-200), not a knee mill. Max RPM is 4000, 3HP, max feed 75 IPM (limited by Mach3, not the steppers).

I have an older beta version of GW. I was waiting to see how useful it would be for me before I shell out for the paid version, and my version doesn't have the stickout button. Seems that had I clicked on one of the Rough/Finish buttons the optimizer would have popped up. It's good to know about the effects there, because as was said, those mills look awfully rigid. It looks as if the 46 IPM chip thinning feed rate is a bug in this earlier version. I guess I need to pay Bob (will send a PM). I will also watch Bob's videos before I make another run in steel.

That endmill actually cost me $25, bought here on PM in a batch of 4 different sizes for $60. Does that make it better quality? ;-)

The CNC parts I'm making are generally one-offs (building a live steam loco), I'm retired, and milling time is not a big deal. Generally I'll be happy if the tool and the part both survive their experience. ;-) I have a lot more experience with HSS mills and have never broken one on this mill, but prior to the loco build almost everything I made was aluminum or brass.

 

[Polaraligned]

Unless you need a 3/16" EM, I would use a 1/2" EM as the "go-to" EM for general machining on parts that size. The Mari-Tool TiALN coated Varimills are fantastic and I can bury one in a piece of steel like that. I will stall my 2hp spindle motor before that EM breaks a sweat. Look at the video on the MariTool website.

 

[kvom01]

Since posting this morning, I've ordered the GW license from Bob (hopefully he'll wake up and activate it today) and viewed the 2 GW F&S videos. So I think I ought to be good to go for the next try. The carbide cutters I have left are relatively long, so I''' need to optimize for the stickout/deflection.

Polar. the Maritool EMs look interesting. I may order one. I think I'll stick with double ended cutters in the future, and I very rarely need deep cuts, so shorter flute lengths are preferable.

I was using a 3/16 cutter on the other problem in order to get all of the parts to fit on one piece of stock. For aluminum I have some large 2-flute HSS cutters if I need to face a larger part.

Most of the parts for this loco "could work" made of brass or aluminum, but they need weight on the wheels for traction, so I'm using steel for almost everything.

 

[ipmmiller]

Unless you need a 3/16" EM, I would use a 1/2" EM as the "go-to" EM for general machining on parts that size. The Mari-Tool TiALN coated Varimills are fantastic and I can bury one in a piece of steel like that. I will stall my 2hp spindle motor before that EM breaks a sweat. Look at the video on the MariTool website.

I second that polaraligned, those Mari VH tialn's are the buisness in any steel,run as fast as you like...not a whimper.