Long neck, small diameter tooling speeds and feeds

jraksdhs · Dec 30, 2022

Any trick to using long neck small diameter tooling. Im trying to 2d profile a part with a 4mm(.157) diameter, corner rad endmill that is 50mm(1.900) long. Need to the length to reach the bottom of the part, and the diameter to get into the spec'd corner radii. Normal speeds and feeds dont seem too work, and Ive tried running a much slower SFM and chipload. Im still getting chatter. Im using a quality er 16 collet holder. Material is mild steel. Any tips?

Finegrain · Dec 30, 2022

Try lower than normal speed, but normal or even a bit higher than normal feed. The longer the cutter gets to dwell in one spot, the greater the opportunity to set up harmonics.

Regards.

Mike

crossthread82 · Dec 30, 2022

Is it a Harvey endmill? If so its gonna chatter no matter what you do.

Mtndew · Dec 30, 2022

There isn't a trick really, you just have to find the happy medium where the harmonics all align.
Usually slower rpm and a bit more feed works for me,with light cuts.

Finegrain · Dec 30, 2022

Also use a larger endmill first, knowing you're missing the corners, then remachine with the long 4mm endmill. At least then the chatter will be localized to the corners.

Regards.

Mike

Finegrain · Dec 30, 2022

Finegrain said:
Also use a larger endmill first, knowing you're missing the corners, then remachine with the long 4mm endmill. At least then the chatter will be localized to the corners.

Regards.

Mike

And predrill the corners so the endmill doesn't have to bury itself in the corners.

Regards.

Mike

MCritchley · Dec 30, 2022

On occasions like this sometimes I ask my self what I would do on a Bridgeport to stop the chatter, I’d slow it down to nothing.
We’ve discussed these long reach tools in threads for some time and the general opinion is to start slow. You may want to put in a sharp cutter and start at like 1200 or something and just do something else for an hour while your pocket finishes. If 1200 works, speed it up.

I had a job with a deep .125 corner rad so I got some .220 dia reaching endmills ground up locally for $46 a piece. I kept the flute length short to 1 dia. I was using .236 endmills and couldn’t get rid of the chatter, I guess I had too much contact.

One thing you can do to your stock tool is to back grind the upper flute to have less flute engagement and a less chattering inducing tool pressure.

Marvel · Dec 30, 2022

Make sure you have more than one endmill on hand and this is where I find the RPM and Feed override to be very useful. Light cuts and play with the override settings until it sounds nice.

I had a large part recently with quite a few slots that were .160 wide x 1.875 deep. I used a 5/32" endmill and ended up running it at 3600 RPM, 18 IPM and .015 DOC was the sweet spot.

13engines · Dec 30, 2022

Let me get this straight... you're using a 4mm diameter end mill to do what radius corner(s)?

In other words... what is the diameter of your tool, and what are the radii you're trying to produce? I'm going to guess and hope you're at least one or two sizes down in the radius of your end mill compared to the radii of your corners.

I've had better luck not trying to match the radii too close. (Obviously never same-same) Like sometimes you'll have better luck with a 3/16 end mil instead of a 7/32 trying to make a 1/8R corner. The more sweep you've got going thru the corner the better. And yes... pre-drill it close like was mentioned.

One other thing you can try depending on fit and finish, is pre-drill the corner close, then drill the corner with a 4 or 5fl on size end mill. Have the end mill back away from the wall on the way down just a thou or two. Make the tiny Z move perpendicular to the corner. Best to get a corner radius end mill, but not to much radius, as the bigger the radius the more deflection it will want to produce. You still might have to deal with a little material on either side of the radius of the corner, but at least the very corner is taken care of, and the all-done-corner allows a larger tool to clear the near sides of it, because you can clear away from the cut before you hit the corner fully. Even if you need to run a finish cut clear around the profile with one last tool to make your blends perfect, the fact the nearly all the meat is gone will only help matters. Good luck making your CAM do this.. Might take a little manual intervention after the CAM gives you something to start with.

jraksdhs · Jan 2, 2023

13engines said:
Let me get this straight... you're using a 4mm diameter end mill to do what radius corner(s)?

In other words... what is the diameter of your tool, and what are the radii you're trying to produce? I'm going to guess and hope you're at least one or two sizes down in the radius of your end mill compared to the radii of your corners.

I've had better luck not trying to match the radii too close. (Obviously never same-same) Like sometimes you'll have better luck with a 3/16 end mil instead of a 7/32 trying to make a 1/8R corner. The more sweep you've got going thru the corner the better. And yes... pre-drill it close like was mentioned.

One other thing you can try depending on fit and finish, is pre-drill the corner close, then drill the corner with a 4 or 5fl on size end mill. Have the end mill back away from the wall on the way down just a thou or two. Make the tiny Z move perpendicular to the corner. Best to get a corner radius end mill, but not to much radius, as the bigger the radius the more deflection it will want to produce. You still might have to deal with a little material on either side of the radius of the corner, but at least the very corner is taken care of, and the all-done-corner allows a larger tool to clear the near sides of it, because you can clear away from the cut before you hit the corner fully. Even if you need to run a finish cut clear around the profile with one last tool to make your blends perfect, the fact the nearly all the meat is gone will only help matters. Good luck making your CAM do this.. Might take a little manual intervention after the CAM gives you something to start with.

What I’m trying to do is profile around a part that is 1.750 tall, with a 4mm end because of two features on the part are 4mm inside radii. I have some flexibility in adjusting those inside corners, but it seems that whatever recipe I try I don’t get a good surface finish.

13engines · Jan 2, 2023

If you have 4mm radii you could use a 6 or 7mm cutter. Why 4mm?

Or do you acutally mean you have inside corners at 2mm radius?

jraksdhs · Jan 3, 2023

13engines said:
If you have 4mm radii you could use a 6 or 7mm cutter. Why 4mm?

Or do you acutally mean you have inside corners at 2mm radius?

My apologies. Yes, a 2mm inside corner radius.

13engines · Jan 3, 2023

Like I said earlier - you'll never get a same size cutter to cut a clean corner if it has the same radius. The tool engagement angle at the instance the tool reaches the corner becomes too great for nearly any size tool. You're fighting a losing battle.

Try some of the suggestions already given by me and others. Say after drilling out the corner with a 3.8 or 3.9mm drill, use a 5 or 6mm end mill to empty out as much material as possible. Then take say a 3 or 3.5mm tool and and sweep it thru the corner multiple times stepping down in Z as you go. Or drill out the corner with the 4mm end mill as I mentioned. At your diameter to depth ratio, it will be tough to get a gleaming smooth surface no matter what you try. You might try a 5 or 7fl for a finish pass. Much stiffer.

If you have the ability, change the corner radius to 2.5 or 2.75mm. Then your 4mm tool might just swing it.

Unlike most engineers who design things using standard or whole number radii in corners, when I draw something, I always make the inside corners a little larger then what might be a standard cutter diameter. This allows me to use the largest cutter possible. The few thousandths extra seldom if ever is of any consequence to the design esthetics or function, but makes a world of difference in the ease of manufacture.

Vanaheim · Jan 3, 2023

Is this 2mm radii required for mating another part or is it there because the part designer finds it easier in their solid modeling software to blithely add 2mm radii to every edge?

Ask the designer if you can change to corner radius (and presumably the bottom of the pocket radii) to something cheaper to machine (eg 4mm radii and use a 8mm ball nose). I tend, like the other commentators, rough out the pocket with a larger end mill and finish the sides and bottom edge with a 4 flute ball nose, stepping down the profile cut in small increments to get a chatter free finish.

Come across too many solid model designers who dont have a clue about cost efficient machining. Not unusual to find a 2mm radii in the bottom of a 80mm deep pocket. Would not have made a blind difference to the strength/weight of the part if the bottom corner radii was 8mm. In fact the part would be stronger.

mhajicek · Jan 3, 2023

When I come across features like that I often find it's cheaper to tip the part 90 degrees and finish the corner with a bull endmill with a matching radius.

13engines · Jan 3, 2023

mhajicek said:
When I come across features like that I often find it's cheaper to tip the part 90 degrees and finish the corner with a bull endmill with a matching radius.

I know you have a 5 axis, but how do you tilt a part 90 degrees and still present it to the spindle? :-) Did you mean 45 degrees? If you're talking outside corners I get it. Inside no.

I may be mistaken, but I think the OP is dealing with inside corners in a pocket. Profiling a pocket not an outer periphery. If he's having trouble with chatter on an outside radius, then I think he's got looseness in his machine. If his part is rectangular and aligned with the machine axis, chatter on outside corners at the 45 degree quadrants, is from slow moving and or reversing screws at the apexes of said corners. The sudden lack of cutting pressures, (or excess pressures if suddenly plowing off a sharp tip) can send a cutter and or machine into vibration. I don't understand him having these problems on outside corners with such small cutters, but you never know.

crossthread82 · Jan 3, 2023

13engines said:
I know you have a 5 axis, but how do you tilt a part 90 degrees and still present it to the spindle? :-) Did you mean 45 degrees? If you're talking outside corners I get it. Inside no.

I may be mistaken, but I think the OP is dealing with inside corners in a pocket. Profiling a pocket not an outer periphery. If he's having trouble with chatter on an outside radius, then I think he's got looseness in his machine. If his part is rectangular and aligned with the machine axis, chatter on outside corners at the 45 degree quadrants, is from slow moving and or reversing screws at the apexes of said corners. The sudden lack of cutting pressures, (or excess pressures if suddenly plowing off a sharp tip) can send a cutter and or machine into vibration. I don't understand him having these problems on outside corners with such small cutters, but you never know.

He could also have an ID radius on the outside of the part. If it were a "T" shape he'd have two.

Best bet is to pre drill corner with 4mm drill offset from corner about 0.002". The rough and finish with big tool, then re-machine corners with a tool smaller than 2mm rad like an 1/8" endmill. Step down about .005" axial per pass; rough then take a .001" radial finish pass maybe even a spring pass as well.

13engines · Jan 3, 2023

crossthread82 said:
He could also have an ID radius on the outside of the part. If it were a "T" shape he'd have two.

Ah-ha... good point

crossthread82 said:
Best bet is to pre drill corner with 4mm drill offset from corner about 0.002". The rough and finish with big tool, then re-machine corners with a tool smaller than 2mm rad like an 1/8" endmill. Step down about .005" axial per pass; rough then take a .001" radial finish pass maybe even a spring pass as well.

Yes another good point. On size drill set off a little is better then slight undersized. Think I've done both one time or another.

mhajicek · Jan 3, 2023

Yes, I was thinking of inside corners on the external periphery.

CarbideBob · Jan 4, 2023

Almost 2 inches deep with a .156 endmill doing pockets. 12:1 . This should be easy ...not..

A helical flute endmill will chatter anytime buried inside a pocket and matching rad like this. Think about who and where is cutting when as this rotates.
So, drill... well my drills do not run straight and I end up with mismatch/straightness/blend problems. I do not have drills that can run 12:1 and make holes straight to .001 in the size.
Make a stepped endmill, do a ton of passes to depth .001 stock left and then gently apply my tool. Takes forever and a day.
Straight flute endmill, does not cut very clean.
Plunge cut the corner with a endmill and do some cleanup on the tangent sides afterwards. Complicated coding.
Endmill dia = inside corner and there will be problems at this length/diameter.
To me this a very inserting problem.
Bob

Long neck, small diameter tooling speeds and feeds

Aluminum

Diamond

Aluminum

Diamond

Diamond

Diamond

Hot Rolled

Aluminum

Stainless

Aluminum

Stainless

Aluminum

Stainless

Plastic

Titanium

Stainless

Aluminum

Stainless

Titanium

Diamond

Similar threads