Stiffness of small mill

ss_user · Dec 15, 2019

Hi all,
At present I'm limping along doing prototyping on a Cincinnati contourmaster (tracer with ball screws) converted to servos. The spindle has had new bearings once that I know of, 10-12 years ago.
At present I'm doing most of my cutting with .25 3 and 4 flute carbide. (dry)
I can just barely get away with slotting at 2200 rpm and 11 ipm with a doc of .05" or .025 x .7 doc. Not much for MRR. Anything more and it screeches. IRRC it used to have way less problems but then I was cutting at slower spindle speeds with HSS cutters and flood coolant. Spindle speed range is ~ 215 to 5650. Tool holding is a 40 taper with 1" of taper contact and an ER20 collet or solid .375, .625 and .75 single set screw tool holders.
In your experience with BP size machines what are reasonable expectations.

It has the 3 bearing spindle configuration common on BP's. Upgrades being considered are:
(1) go to 5 bear1ng config
(2) go 3 bearing or 5 bearing conventional or SiC
(3) spend real money and go to SK custom spindle
(4) change out 1 Hp for 2 Hp spindle motor

Comments, WAG's, SWAG's greatly appreciated.
TIA

13engines · Dec 15, 2019

In your example, what material? That feed rate is verging on too slow. But more you get chatter? Hmmm. The "I can just barely get away with slotting" sentence doesn't make any sense at all. doc of .05" or .025 x .7 doc. What?? Care to rewrite? Is one of those meant to be width of cut? If so then you're not slotting. That's called periphery milling. It may be in a slot, but not the same thing.

How long are the tools being used? The stick-out length or length to diameter ratio of your tools has the greatest affect on chatter then about anything.

I don't understand it when you say 1" of contact in your 40 taper spindle? Where's that coming from?

The fact that you had less troubles with HSS is indicative of rigidity problems. HSS tends to give where's carbide doesn't. Have you checked the adjustment of the machine gibs? Lack of rigidity is not only relegated to spindles. It's the whole setup as a system.

eaglemike · Dec 15, 2019

Be sure it's not cutter and cutting conditions limiting your ability to cut.
You have a 40 taper, so the bearings are of decent size for smaller cutters. I'm not sure what you mean by 1" of taper contact though.
You are RPM limited. You don't have flood coolant, so that can be a bit of a limitation. I used to use mist coolant from a Kool-Mist nozzle with a 30 taper machine, and that worked okay. If you have enough shop air, there are cold air nozzles out there that will make life better.
What control is on the machine? If it's up to using high speed machining tool paths, you need less power and rigidity.
Depending on how that machine has been used, the bearings might be an issue, or the machine might need a rebuild. A lot isn't clear at this point.

ss_user · Dec 15, 2019

13engines said:
In your example, what material? That feed rate is verging on too slow. But more you get chatter? Hmmm. The "I can just barely get away with slotting" sentence doesn't make any sense at all. doc of .05" or .025 x .7 doc. What?? Care to rewrite? Is one of those meant to be width of cut? If so then you're not slotting. That's called periphery milling. It may be in a slot, but not the same thing.

How long are the tools being used? The stick-out length or length to diameter ratio of your tools has the greatest affect on chatter then about anything.

I don't understand it when you say 1" of contact in your 40 taper spindle? Where's that coming from?

The fact that you had less troubles with HSS is indicative of rigidity problems. HSS tends to give where's carbide doesn't. Have you checked the adjustment of the machine gibs? Lack of rigidity is not only relegated to spindles. It's the whole setup as a system.

Ah! Mea culpa. Or as I heard many time as a child. "The best laid plans of mice and men gang aft a-gley.. I clearly take in in the neck for not being explicit enough. So ... more words. The slotting with protest is .25 carbide end mill uncoated or TiAlN coated. Stickout is 1" with a flute length of 0.75.(ER20) In a side cutting condition the doc is .7, axial is .025 both are generally at spindle rpm of 2200. Once in a while I go up one step to 3200. Things do not get quieter. Total tool length is 2.5". The tool holding setup is something you are unlikely to have seen. Visualize a 40 taper that is 1" from the gage line to the upper end. Held in place by a large bronze nut. Remember this is 1960 or before technology. Machine was at Boeing in '63, way older than most of you. :-)

To respond to the gibbs question: no I've not tried adjusting them, color me chicken.
I used to run this machine with 165 v on the servos, a bit over the rating. Speed was nice but with iron on iron one is really pushing the limits. There just ain't no free lunch.
Thanks for you comments. :-)
Onward and hopefully upward.

ps. comment from other poster on cold air blast is interest and probably useful. Chip clearance is manual at this point but still something useful to think about.

Dave

eaglemike · Dec 15, 2019

I'm still looking for the material. Did I miss it?
If the tool is rubbing, you are going to have problems.

DMF_TomB · Dec 16, 2019

ss_user said:
Ah! Mea culpa. Or as I heard many time as a child. The slotting with protest is .25 carbide end mill uncoated or TiAlN coated. Stickout is 1" with a flute length of 0.75.(ER20) In a side cutting condition the doc is .7, axial is .025 both are generally at spindle rpm of 2200. Once in a while I go up one step to 3200. Things do not get quieter. Total tool length is 2.5". The tool holding setup is something you are unlikely to have seen. Visualize a 40 taper that is 1" from the gage line to the upper end. Held in place by a large bronze nut.

Dave

.
.25 carb end mill sticking out 1" is 4x length to dia ratio which is on the high side of sticking out. when you 2x length stickout it flexes 2x2x2 or 8x more. length sticking out effects things alot
.
2200 rpm at 7.0ipm feed is about 144 sfpm .0011 ipt feed if 3 flute(.25hp if 0.7DOC and .05WOC at 53lbs of cutting force) for 1018 steel thats pushing it a bit even at .025 WOC my calculations show thats a lot of depth and width of cut for end mill dia and stickout length. without exact details on part material cannot calculate hp and cutting forces. obviously harder metal alloys cause more problems
.
not being able to run faster rpm and feed usually a end mill vibrating problem. usually 1hp mill is limited to about 0.5hp at the spindle due to loss from belts and gears. probably mostly a tooling limit assuming its not the part vibrating too. its possible its a machine vibrating thing too, obviously some machines are a lot more rigid than others. some machines dont like a lot of side cutting force that you get with high DOC and moderate WOC. there is a reason they dont put higher hp motors on mills as mill itself cannot handle the higher cutting forces without high vibration. some machines vibration resonate at certain rpm, they start vibrating alot, literally at certain rpm vibration can increase over 10x more

ss_user · Dec 16, 2019

Good point on material. Indeed the machine cuts Al much better than steel but I pretty much live in a world of steel. A bit of O1 and 4140 but mostly A36 for first try and 8620 for real and hours several hours of machine time per part. A reasonable portion of it with me squirting air to clear chips. Maybe I should go back to HSS and coolant (really messy on an open machine).
I've done a bit of roughing with vertical plunging for major amounts of extraneous material.

I will try 1/4" carbide at higher speeds. Not much to risk with inexpensive tools.

I bought a couple of Maritool AlCrN coated end mills to try but that is a future project; and means rigging coolant ... again.

Maybe I'm just expecting too much out of the machine. The ultimate goal is to get the Mazak V5 running again but that implies either tearing down the whole top of the machine to fix the belleville stack or jury rigging some other way to retain tooling.
I'm coming up on my 82nd birthday so not a spring chicken anymore. The mind is still kinda OK. Body not so much. :-)

Thanks for the kind replies; off to the shop to try playing with cutting parameters. Of course some things are simply beyond physical reality.

eaglemike · Dec 16, 2019

Mari has some 6 flute 1/4 inch finishers that work very well on 17-4 H900. This is about Rc45 if you are not familiar with that material. Your .025 cut width would be very reasonable, I'm running 12% with a 5 flute version, .02 corner radius, 95 inches per minute, 9100 rpm. Tool lasts a fairly long time. My machine is a lowly (grin here) 30 taper.
If your machine movement is smooth, and the control is decent, try some high speed paths. If you aren't familiar with that, it's keeping the cutter width engagement constant as possible.
Good luck!

mhajicek · Dec 16, 2019

That 1" of spindle contact screams at me. Doubling it to 2" should multiply your rigidity in that interface by 8. I'd either modify the spindle to fix that or replace the spindle with a proper one.

TeachMePlease · Dec 16, 2019

eaglemike said:
Mari has some 6 flute 1/4 inch finishers that work very well on 17-4 H900. This is about Rc45 if you are not familiar with that material. Your .025 cut width would be very reasonable, I'm running 12% with a 5 flute version, .02 corner radius, 95 inches per minute, 9100 rpm. Tool lasts a fairly long time. My machine is a lowly (grin here) 30 taper.
If your machine movement is smooth, and the control is decent, try some high speed paths. If you aren't familiar with that, it's keeping the cutter width engagement constant as possible.
Good luck!

Uhh, I always thought H900 was just high 30s, like 38ish?

mhajicek · Dec 16, 2019

TeachMePlease said:
Uhh, I always thought H900 was just high 30s, like 38ish?

It's about HRC 40-45 depending on source.

Edit:
Here's a source saying it can range from HRC40 to 48:
Alloy 17-4 H900 (Alloy 630, UNS S17400) stock available at Penn Stainless Products | Penn Stainless Products

DMF_TomB · Dec 16, 2019

1) A36 steel usually machines like 1018 although some A36 has hard spots of slag big enough to damage cutter suddenly
.
2) HSS is not as rigid at carbide. in general you take less depth and width of cut go slower rpm and feed cause it will bend and break easier
.
3) be careful with some cutting parameters which end mill might last less than 10 minutes and or suddenly fail go red hot and melt
.
4) usually if end mill is noisy you lower depth and width of cut, then lower rpm and feed so its not as noisy and end mill lasts a reasonable time like 60 minutes of cutting and no sudden tool failures.
.
5) many a end mill sticking out of tool holder over 3x (3 times dia stickout) cannot run anywhere near rpm and feed of a end mill that is less than 2x stickout. when you get up to 4x or 1" stickout for 1/4" dia end mill thats a lot when trying to rough a lot. when you go from 1/2" to 1" stickout it flexes 2x2x2 or 8x more or in general you reduce depth and width of cut so its removes 1/8 the cubic inches per minute of chips and often have to run slower rpm and feed

Fal Grunt · Dec 16, 2019

13engines said:
I don't understand it when you say 1" of contact in your 40 taper spindle? Where's that coming from?

If it is like my Cinci, it is essentially a STUB 40 taper.

I have redone the bearings on my Cinci, and they are not equivalent to what you would expect in a 40 taper machine. They are more like an R8 bridgeport. NOS bearings off ebay took about a year to source and around $500.

I made money for several years off my Cinci, then I bought another machine. I made money of that machine for several years and kept adding machines. Finally I bought a Brother. I can tell you I do not for a second regret buying the Brother. I do regret the countless hours and dollars screwing around trying to improve the old machines to make them easier/better to use. I still use them, they still make me money, but if I had it to do over again... I think I would have tried to buy a CNC sooner.

eaglemike · Dec 16, 2019

TeachMePlease said:
Uhh, I always thought H900 was just high 30s, like 38ish?

I've seen it 43-46 in my applications over the years. Typically 44-46, pretty much every time. It's not bad to machine. H1150 would be easier, about Rc33.
If the corner goes, it's over. I'm having good luck with the Mari endmills. I order 100 at a time, as the .02 corner radius is a special. Frank is good people.

mhajicek · Dec 16, 2019

eaglemike said:
I order 100 at a time, as the .02 corner radius is a special. Frank is good people.

I'm using Helical, .020" radius is a standard off-the-shelf.

eaglemike · Dec 16, 2019

mhajicek said:
I'm using Helical, .020" radius is a standard off-the-shelf.

5 fl, 1/4, 45 degree with the coating? or 6 fl? His pricing is better than others I've found, even though it takes a couple of weeks to get them.

mhajicek · Dec 16, 2019

eaglemike said:
5 fl, 1/4, 45 degree with the coating? or 6 fl? His pricing is better than others I've found, even though it takes a couple of weeks to get them.

Helical Tool

I put in 1/4" diameter, .020" corner radius, for cutting SS with HFM, got 43 results.

I'm not saying Maritool cutters are in any way inferior (I haven't done a comparison), just that these are what I'm using with good results. Lots of options off the shelf that work well in 17-4 H900 and Ti6Al4V-ELI.

Mateomicro · Dec 16, 2019

This is a Bridgeport type mill. Not sure how to make things more stiff than the usual cutter minimum stick out and quill as close to being all the way up as you can. I am thinking this is not a spindle problem but a iron problem. These are nice machines but just not a good pick for fast or cuts over .050" if you are going for precision. I may have misunderstood you but seems the type of mill is your problem.

DavidScott · Dec 16, 2019

Sounds to me you need to use good stub mills projecting out of the holder as little as possible. I don't use 1/4" mills with 3/4" loc because you can't take much of a cut with them, and I machine mostly aluminum.

Fal Grunt · Dec 16, 2019

A stub with a high helix to reduce cutting forces may help.

Air blast would help improve finish and tool life.

It’s a 50-60 year old tracer, your not going to be able to run speeds and feeds of modern machines. On my old Cinci I would run heavy slow cuts with larger tools in side locks, then skim with a real light finish pass.

Stiffness of small mill

Aluminum

Stainless

Stainless

Aluminum

Stainless

Diamond

Aluminum

Stainless

Diamond

Diamond

Diamond

Diamond

Titanium

Stainless

Diamond

Stainless

Diamond

Plastic

Diamond

Titanium

Similar threads