[twocik]

I'm trying to reduce the what looks to be a very little bit of chatter I'm seeing and less time at my vibratory bowls. So I thought I'd ask you guys to see if you'd be able to help me out.




6061-T6 stock anywhere from .4" - 1.1" thickness. I'm climb spiral roughing with a 1/2" EM leaving .02" wall stock and finishing this off with a 1/2" 2 FL 1-1/4"LOC carbide zrn coated EM. This finishing end mill to be exact

MSC Item Detail



My finish pass is at .02" woc, I'm using a .2 tangent lead in and out full depth of .4" - 1.1" (5 different parts all with the same cutter) at 15.3 IPM - 3820 RPMs - climb cutting




My question is since I've played around with reducing the feed and rpms slightly lower with very little difference to show. At first I'm thinking it's 1/2" thick that should be thick enough to take whatever I give it, but now I'm starting to rethink this after seeing the speeds & feeds chart for this particular end mill... At the very least it's telling me I need 4500 rpms - 90 IPM - .01 FTP - SFM 589 (can't do the suggested 600 sfm)..... I haven't tested this yet, but If I'm taking such a small finish pass how would something like this turn out on a tormach ?



Last if our rpms, feeds, etc.. are limited and not up to par with the big 50k plus machines, are these high performance end mills even useful for us Tormach users ?

Meaning if we not using them as the manufacture suggest the bits should dull pretty quick right ?


.

[pete from TN]

I do not own a tormach but my CNC'd RF45 is similar. I have a belt drive that can give me 6500 RPM if necessary. I am using the Maritool three flute Carbide uncoated high helix endmills for most of the aluminum cutting I am doing. It is providing me with the best surface finishes I have been able to get on my mill. I also use a .020 finish pass because I feel that the cutter seems to like removing some material on the finish pass. I have had excellent material removal rates and great success with these cutters so far. Honestly tho the thing that improved my surface finishes the most was that I went thru all my collet holders and checked them all for actual runout on the mill. I actually clocked the endmill collet in the holders until I got the runout as little as possible and then I clocked the holder to the spindle. I use an automatic center punch to put two small dots on the side of the spindle body near the holder and then I put another dot on the holders body when I got them aligned as good as I was able to. When I need the cuts to look as good as possible I just take that extra moment to clock the holder to align the marks and then lock it down. It has made a vast improvement in the finishes and the cuts just plain sound better. I was also surprised at how much I could affect the runout just by loosening the collet nut slightly and tapping on the endmill's shaft with a very small brass ball peen hammer. Just loosen and tighten after you tap it a bit and then lock it down when it is the best you can get it.

I think the higher spindle speeds are also a factor as you can feed for a certain chipload without going terribly slow. I am using an 18 IPM feedrate on the 1/2 inch three flute and something north of 20 for my 3/8 three flute. I also find that in a full slotting operation the three flute cutters just sound smoother too... Just some simple suggestions as to what has worked for me. Good luck man... peace

Pete

[BobWarfield]

twocik, your cutter should be fine even doing 5100 rpm and 73 IPM. If you want to reduce the chipload to get a finer finish, I wouldn't go much below 26 IPM and keep the spindle rpms up.

As Pete suggests, a 3 flute should give you an even finer finish.

If that is indeed chatter, and it may not be (for example, it could be runout as Pete suggests), you can tune the spindle speed to minimize it. This only works when you can see the chatter marks well enough to measure their distance apart, but if you can, you can calculate the optimal spindle speed to minimize the chatter.

Eventually I will put a calculator for this into G-Wizard, but for the time being, I described the process over on PM:

Serious chatter when slotting - Practical Machinist - Largest Manufacturing Technology Forum on the Web

If you run that spindle tuning calculation, you will at least minimize the excitation of the chatter.

Another apprach to chatter is tool tuning. If you move the tool stickout by 0.020" or more, you will change the chatter frequency. BTW, doesn't matter which way you move it, in or out.

Cheers,

BW

[twocik]

"If you can, you know the chatter pitch, and you can calculate the optimum spindle speed to minimize the chatter.

You want to use what's called the "tooth passing frequency" to tune your spindle speed.

Let's say the chatter marks are 0.001" apart. Your chatter pitch is then 0.2 * SFM / 0.001 = 52000. Divide that by your four flutes and you get 13000 as the tooth passing frequency. Now any integer fraction of that will work i.e.

1/1 = 13000 rpm
1/2 = 6500 rpm
1/3 = 4333 rpm"






Since we're on this subject, I have a question for you Bob if you have a min. My tool is sticking out of the collet by 1.7725, the tool has a 1.25 loc. Yes I'm about 0.5225" to far out and was curious if you clamp this part of the tool without losing any concentricity causing more runout than what the collet is rated at .0005" ?


I use this end mill for a few different jobs, but only require 1.1" depth. I tried to get the round part of the shank as far as I could get it in the collect without clamping any flutes. The flutes extend .480" which I think is called the relief of the end mill.. I included a picture to show what I'm talking about.



My marks are about .011" apart give or take. I'm not sure I understand where the .2 comes from in your calculation, but the rest makes sense ?







"I actually clocked the endmill collet in the holders until I got the runout as little as possible and then I clocked the holder to the spindle. I use an automatic center punch to put two small dots on the side of the spindle body near the holder and then I put another dot on the holders body when I got them aligned as good as I was able to. When I need the cuts to look as good as possible I just take that extra moment to clock the holder to align the marks and then lock it down. It has made a vast improvement in the finishes and the cuts just plain sound better. I was also surprised at how much I could affect the runout just by loosening the collet nut slightly and tapping on the endmill's shaft with a very small brass ball peen hammer. Just loosen and tighten after you tap it a bit and then lock it down when it is the best you can get it. "




Pete thanks for going thru that. Now with a dial indicator mounted, you're running the needle along the shank of the tool right ? I've done this once before but wasn't sure how great this would work since I'm having to pull the tool out to put an indicator on the smooth part of the shank, then shoving it back in hoping that it doesn't move. Was that your process ?


.

[pete from TN]

The majority of my cutters are not that long of a flute. My cutters are three flute HH maritools and when fully inserted into the collet they still show a little bit of the flat of the shank so I can read directly there with the DTI. Basically I take an endmill, put it in the collet, jog the table over with the Mag base/DTI in it and bear on the shank. Then I turn the spindle by hand to a point where the DTI is showing the least deflection or the tool shank is furthest away from the DTI. Then I jog it back away and tap the other side of the shank a bit. Does not take much really....Then I jog back in and turn the shank again watching the needle. I just keep tweaking the rotary position of the collet and tapping the endmill until I get the absolute least runout I possibly can and then I tighten down the collet nut using a pair of large Adjustable wrenches. Then I take the holder and begin the same process clocking it to the spindle body in the same manner until I get as little runout as possible that way. Place a pin punch in alignment with the pin punch on the spindle and you're good to go. Some holders get damn tight and some not so much but ALL of them benefit in some manner from this process. Another thing to consider is the overall shank of the cutter. My 1/2 inch three flute is purposefully a short length of cut for rigidity's sake. You might try using another cutter for roughing fast and then put that cutter in there properly optimized and run it gingerly.... Good luck.. peace

Pete

[BobWarfield]

Pretty sure the 0.2 is for unit conversion, but I'd have to go back to the PhD thesis I got the formulas from to be sure, LOL.

I went ahead and coded up the calculator. It'll be in the next G-Wizard. For this cut, I get the following chatter minimizing spindle rpm's that are within your spindle's range:

4545 rpm
2272 rpm

The others are too slow or too fast.

I will be surprised if this turns out to have been chatter. Doesn't seem like you're pushing hard enough, but there may be just enough of a resonance there. FWIW, so long as you tee up the same kind of tool holder, same kind of endmill, and the same stickout, it'll be reproducible. So if it is chatter, it is useful to have mapped it.

I wouldn't try to clamp on the flutes. That can't be good for anything. To clock it as Pete says, you'll need some smooth shank for the tip of your DTI. Try leaving 0.100" or so. That ought to give you something to track on. Just to see if much runout is showing.

Best,

BW

[dbrija]

Pretty sure the 0.2 is for unit conversion, but I'd have to go back to the PhD thesis I got the formulas from to be sure, LOL.

I went ahead and coded up the calculator. It'll be in the next G-Wizard. For this cut, I get the following chatter minimizing spindle rpm's that are within your spindle's range:

4545 rpm
2272 rpm

The others are too slow or too fast.

I will be surprised if this turns out to have been chatter. Doesn't seem like you're pushing hard enough, but there may be just enough of a resonance there. FWIW, so long as you tee up the same kind of tool holder, same kind of endmill, and the same stickout, it'll be reproducible. So if it is chatter, it is useful to have mapped it.

I wouldn't try to clamp on the flutes. That can't be good for anything. To clock it as Pete says, you'll need some smooth shank for the tip of your DTI. Try leaving 0.100" or so. That ought to give you something to track on. Just to see if much runout is showing.

Best,

BW

One thing to keep in mind is the actual spindle speed versus what you ask for. Per my spindle tach thread, you get roughly +/-10%, so your calculated ideal frequency won't be what you get (for $40, you can get a lot closer with the tach). FYI if I ask for the max speed of 5140, I get 5400RPM on the tach.

[twocik]

Ok I follow, it's a two step process, tool to collet and then spindle to TTS holder. Never thought of doing this with the spindle, guess nothing is prefect huh.



My tool in the collet reads .0001" runout, however I had to loosen then shove it back inside and retighten the tool again. If I was to shove the tool in right at the end of my loc .480" mark closet to the cutting point shown in my pic, would this be a bad idea ?

Reason I ask is, one coolant, chips, etc.. could now enter inside those two gaps on both sides of the end mill due to the extended flutes, two if I'd gain more runout or loss in rigidity only clamping 2 sides/walls of the shank and not a full circle.....

[twocik]

"4545 rpm
2272 rpm

The others are too slow or too fast.

I will be surprised if this turns out to have been chatter. Doesn't seem like you're pushing hard enough, but there may be just enough of a resonance there. FWIW, so long as you tee up the same kind of tool holder, same kind of endmill, and the same stickout, it'll be reproducible. So if it is chatter, it is useful to have mapped it. "



From what I've read on some of the higher end mill manfactures was to reduce your feed & speed by 30 - 50% on longer reaching end mills. I figured this kind of just makes the mark for that, but if you think I'm not pushing hard enough I guess I got turn things up.


Here's what I'm getting with your rpm calculations

DIA - 0.5"
Flutes - 2FL
RPMs - 4545
IPM - 73
SFM - 595
FPT - 0.008 (man. recommend chip load)



DIA - 0.5"
Flutes - 2FL
RPMs - 2272
IPM - 36
SFM - 298
FPT - 0.0079





Don't clamp flutes, noted. Yea I thought that would be a bad idea

.

[twocik]

?

[pete from TN]

?? :boxing::wee::wave:

[twocik]

Not sure what that's supposed to mean... but guess I'll give the last one a try and see what happens.

[BobWarfield]

"4545 rpm
2272 rpm

The others are too slow or too fast.

I will be surprised if this turns out to have been chatter. Doesn't seem like you're pushing hard enough, but there may be just enough of a resonance there. FWIW, so long as you tee up the same kind of tool holder, same kind of endmill, and the same stickout, it'll be reproducible. So if it is chatter, it is useful to have mapped it. "



From what I've read on some of the higher end mill manfactures was to reduce your feed & speed by 30 - 50% on longer reaching end mills. I figured this kind of just makes the mark for that, but if you think I'm not pushing hard enough I guess I got turn things up.


Here's what I'm getting with your rpm calculations

DIA - 0.5"
Flutes - 2FL
RPMs - 4545
IPM - 73
SFM - 595
FPT - 0.008 (man. recommend chip load)



DIA - 0.5"
Flutes - 2FL
RPMs - 2272
IPM - 36
SFM - 298
FPT - 0.0079





Don't clamp flutes, noted. Yea I thought that would be a bad idea

.

Assuming the ? is meant to be about these two choices (even a few extra characters can go a long ways, LOL), you don't need to make those additional adjustments to G-Wizard's calculations. It already severely derates the feeds and speeds for excessive depth or widths of cut, plus its choice of starting chiploads and surface speeds are relatively conservative.

If you have the latest version, you can use the Gas Pedal to throttle back if you want to be especially conservative and it will do it that way.

Your biggest issues for tool breakage would be (assuming you're using recommended chipload or less):

- Chip clearance. I always make this #1. Most are not nearly paranoid enough about it. It will ultimately defeat any attempt to get by on conservative feeds and speeds.

- Lubrication and chip welding with sticky materials. If you have a suitable mist or flood, that takes care of that. Expensive coatings also work, but you have to make sure they're intact.

- Deflection. If G-Wizard isn't crying about that by turning the deflection number orange, don't sweat it.

But you're just dealing with surface finish, so focus on the runout. If you have G-Wizard, dial the Gas Pedal to the conservative setting which will up your ration of spindle rpm to feedrate. Lastly, a 3 flute will give a better finish too.

Cheers,

BW

[pete from TN]

Honestly was not sure what you were asking there. Not trying to be a wiseass... Good luck man...peace

Pete

[twocik]

Sorry guys I forgot the "anyone have a suggestion" in front of that question mark... Wrote that in a pinch



As for coolant, yes I have 3 hoses that really get those chips out.


The run out on the collet to tool is almost .0001" and same for the collet to spindle measured right below the new ATC ring on the ER-20 .0001". however now that I think about it I should be measuring from the inside of the collet, but think the first test is close enough. I'm thinking if it's not my feed/rpms, then it could be my tools accuracy. I'm looking into different cutters like the smaller high helix 3FL I have already, but this I sure wouldn't do very well for mid to deep slotting.


Anyone that has used a similar cutter 1/2" 2fl 1-1/4 loc feel free to post your speed, feed, etc.. I'm curious to see if other have had the same problem (little ridges) I'm seeing.



Bob I wrote you a PM

[David Bord]

Maybe Im a sissy but is that chipload a bit agressive for a machine of this size? If you dont achieve your desired results on your next try, maybe cut that way way down for your finish pass. Like to .002 to .003

Id recommend looking at G-Wizard for speeds and feed guidance. Im doing the demo now and have been finding it really easy to use and very helpful. They have a great hobbyist special going on now as well.

David

[twocik]

Yea that's where I started for my finishing pass. It takes about 3 more hours in the tumbler (not to mention sizing down some of parts where I don't want it) or me belt sanding it off. I like G-wiz for the few times I used it, but was in the middle of a big move and didn't really get to use it. One thing I didn't like was the adobe package I have to install in order to use it. I asked Bob if the program was a type of application now and if it is then yes most likely I'll buy it.

The S&F calculator I'm using now is a very simple calculator but doesn't give you information like tool defection, frequency tuning, HP required, etc.. Honestly this tool and another long reach tool are the only two I've had problems with and I'm really starting to think it was the tool I bought. The tool tip to tip is within .0001". I've tested everything, except the new feed and speed.



.

[BlueFin]

Anyone that has used a similar cutter 1/2" 2fl 1-1/4 loc feel free to post your speed, feed, etc.. I'm curious to see if other have had the same problem (little ridges) I'm seeing.

I get the same exact lines you are getting with the same type of end mill, Cleveland 1/2" two flute 1 1/4" long. 4500 rpm .020" and 25 IPM, I get a better finish with 3 flute A337 Niagara, but the lines are still there. Following this thread to see what it takes to make it stop

[BobWarfield]

Guys, you are going to get some level of tool marks no matter what. Here are a couple of pretty small parts (About 1" high) magnified 5x:



They were cut with a 3/16" carbide 2 flute in MIC6 aluminum. The difference between the two is the left was an 0.010" width of cut finish pass and the one on the right is as roughed. Still some visible marks there, though obviously one is way better.

If you really want to delve into periodic visible marks, there are tons of sources:

- Chatter

- Some oddity of tool geometry

- Repetitive error or vibration in spindle rotation. A belt drive ought to be a lot smoother than a gear drive on surface finish as the belt cushions the spindle from some vibration.

- Spindle bearings. There is a reason they spend so darned much for good ones.

- Spindle setup and preload.

- Runout of spindle taper. The best spindles have the taper ground while the spindle spins in the bearings that will be used on them machine. I have an article on my site of Frank Mari (Maritool) regrinding tapers on a VMC that is very cool. He also wrote it up on PM. Not for the faint of heart!

- Toolholder runout. BTW, you probably don't think of them in this way, but the ears on the CAT40 facilitate clocking to the same position so the runout is at least predictable.

- Cutter runout, where the cutter was ground slightly off center

- Tool clamping force. You see this all the time on PM. Someone buys a used machine. Crappy surface finish. Run a pull gage. Oh! We need new Belleville's! Fixed, yay!

And probably a ton of other things I haven't mentioned. Deburr and vibe work is really the only answer. For aluminum, a satin finish is achievable very quickly in a blast cabinet. That finish is a nice one for shop pieces. If it gets scratched, another trip to the cabinet fixes it like new.

Cheers,

BW

[twocik]

Yes Bob everything you stated is corrected and I understand it is nearly impossible to machine a part without any marks. However the reason I started this thread was hoping to find a honey spot for this setup. Yes if the tool is going to cause me this much headache on to the next, actually I bought a fast spiral 60° 3 FL from mc master. Should be here next week


I ran that last suggestion on F & S and here's what I got pic attached. Another thing I didn't mention that might help is a vertical lead in and out line on the back side of my part. I've tested both of my axis backlash, X0.0003" Y0.0004" and don't really think this is the cause. I believe it's a feed, speed and tool length issue. So I'm going back into to war with this damn problem now and let you know in a few hours what F & S looks best. :bat: