Where do we use button inserts?

sinha · Sep 19, 2018

I am asking this question because I have never used round inserts.
My intuition says that, because it has wider engagement, it would cause a lot of radial thrust on the workpiece.
Consequently, it perhaps cannot be used for heavy cutting, specially when workpiece rigidity is an issue.
On the other hand, when put on a neutral holder, it can circumvent interference issues while machining a pocket on a lathe.
So, where do we use it? What are the usual cutting parameters (DOC and mm/rev feedrate) for machining mild steel?

guest · Sep 19, 2018

I've used them on both grooving tools and face mills. The thing I liked was you could rotate the insert to get to a sharp edge, and depending on the cut you could get several turns before you had to change it out.

On grooving they are about the only geometry that works for hemispherical grooves. The face mill I used was on an old K&T vertical. That machine didn't much care about tool pressure, it marched through just about anything I had the balle to attempt.

Speeds and feeds are normal carbide numbers.

sinha · Sep 19, 2018

Ever used it for turning ?

D Dubeau · Sep 19, 2018

I use 10mm button inserts in a 1" shank holder for undercuts in the mill. Just a normal holder that has a portion of the shank machined away to allow undercutting. I also made a holder for the lathe to take the same inserts so I could turn things like constant radius grooves and such. Think tube bender dies.

Doesn't see a lot of use, but has been a life saver on a lot of jobs over the years.

706jim · Sep 19, 2018

We used them on an old Valenite "Cyclomill" roughing cutter. I believe about 3/8 diameter with a positive geometry.
They could be rotated about 4 times before needing replacement. A scalloped side cut surface was the result requiring a finish pass with something conventional.

Qwan · Sep 19, 2018

People use them for cutting corner radii in pockets if they do not want to step down a cutter using a smaller corner radius.
Also, can work well for undercuts as D Dubeau mentioned.
Before dedicated high feed cutters were available, some people used them as such but if you have a high feed application you really should purchase an actual high feed cutter.

NaRbO · Sep 19, 2018

We use them a lot for mold work. A lot of hard mold steels, use them for roughing and semi finishing. The round inserts are much stronger and can handle the hard steels better. Great for semi finishing on larger mold cavities because you can take a larger stepdown and stepover compared to a ball and still get a decent finish. Having said that we are starting to move more to the high feed stuff, also works well on the hard stuff. But for semi finishing the button is still great because it gives you a true radius to work with unlike the high feed inserts.

jjxtrider · Sep 19, 2018

I've used 1/2 buttons mostly in manual lathes for seal grooves, round belt conveyors or putting radius in corners of shafts and rollers . We mostly switched to lolipop style in Top Notch or grooving tools(.156, .188,.236,.250, & .312) for in the cnc lathes since the big radius isn't needed to get truer diameters with much less rattling from too much tool pressures. Feeds and speeds were actually low sfm but high feeds to get some sort of chip control. I don't see a whole lot of uses in lathes with cnc's but are nice in manuals . Mills would be more benefits, but thus far our radius's have been done by large corner rads in standard insert in facemills or indexables.

.

guest · Sep 19, 2018

sinha said:
Ever used it for turning ?

Only on grooves. For normal profiling I usually use garden variety negative C,W,V etc.

mikiemus · Sep 19, 2018

sinha said:
I am asking this question because I have never used round inserts.
My intuition says that, because it has wider engagement, it would cause a lot of radial thrust on the workpiece.
Consequently, it perhaps cannot be used for heavy cutting, specially when workpiece rigidity is an issue.
On the other hand, when put on a neutral holder, it can circumvent interference issues while machining a pocket on a lathe.
So, where do we use it? What are the usual cutting parameters (DOC and mm/rev feedrate) for machining mild steel?

Done it in lathes. Large diameters! Also facing large diameters succesfully. Facing makes the load go towards the chuck. Insert diameter makes it possible to 'normal' depths of cut, but huge feed rates. Everything pends on how rigid your part is, and the material. Softer, lighter to cut, the better. Plastic to Aluminium. Harder materials need support from diameter (like, Dia > length). Rest is just normal speeds for the specific material. This all is only for coarse, and very coarse machining. Maybe you want high feed rates for finishing, but radial load might cause a problem. Just play around with it, and you get it. Start with heavy facing. Really fun! :-)

TRussell · Sep 19, 2018

sinha said:
Ever used it for turning ?

They work great in an interupted cut. I have used them a few times turning square stock round.

Jaxian · Sep 19, 2018

Interesting you should ask. I just ordered a small one after seeing a video where someone was turning small diameters and able to go both directions without having to switch tools for the undercut.

They were turning a metal wine glass and it looked like such a good idea I ordered one to play around with it. Sorry but I can't for the life of me find the video. Putting in Turn Wine Glass on YouTube gets a thousand videos of woodworkers.

EDIT: It was a SRDCN2525M10 25x150mm

Tonytn36 · Sep 19, 2018

Use them in PCD in aluminum a LOT for roughing because you can run very aggressive feed rates with a decent finish.

Jashley73 · Sep 19, 2018

These days, the choices for round carbide inserts for turning, are getting slimmer, and slimmer. Mostly used for copy-turning, or large-roll turning. Be that as it may, you can still lay down some aggressive/high feed rates with a round insert in turning. The problem is that the low lead angle, generates a lot of radial pressure, so you have to make sure the part is securely clamped if you're going to try it.

However, for hard-steel, and super-alloy turning, they're frequently the 1st choice recommendation because of their inherent strength. There's lots of options for round inserts in ceramic & CBN grades.

sinha · Sep 20, 2018

Thank you guys a lot for sharing your experience. You have given information I was exactly looking for. Thanks again for your time.

SND · Sep 20, 2018

Roughing High temp nickel alloys, inconel, hastelloy and such. Negative leads also work pretty good. Strong edge and prevents a built up to form ahead of the insert and chip it.

angelw · Sep 20, 2018

sinha said:
Ever used it for turning ?

Hello Sinha,
Plenty of times. The scallop height using a 0.8mm TNR and a feed rate of 0.25mm p/r is 0.0098mm. The same scallop height using a 6.0 radius button insert is achieved with a feed rate of 0.6856mm p/r. What you can't have in DOC using a Button Insert, can be made up with feed rate.

If you were to try and emulate the DOC of, say, a DNMG insert, the feed rate would have to be quite low and the great engagement of the circumference of the Button Insert would result in profound chatter; accordingly, light DOCs are in order. At a feed rate of 0.6856mm and a DOC of around 0.5mm. swarf control would be hideous, but at light DOCs, feed rates of 3.0mm p/r will give good chip control in most steels. One job I recall well, 35 minutes was taken out of a 50 minute cycle time using a 12 diameter Button tool on a deep, wide face groove, using a DOC of 0.5mm and a feed rate of 3.0 p/r. Each cut was made in the X axis, with each cut being in the inverse direction of that which preceded it; a light feed rate was used at the end of each X axis cut to plunge in Z for the next cut.

The above system also gives you many new cutting edges by rotating the insert to present a new sector to the work.

Regards,

Bill

sinha · Sep 21, 2018

Thank you Bill for explaining so nicely, though I could not fully understand the machining scheme in the last example. Maybe I need to read it more carefully.

Hazzert · Sep 21, 2018

sinha said:
Thank you Bill for explaining so nicely, though I could not fully understand the machining scheme in the last example. Maybe I need to read it more carefully.

It is the same principal as a high feed mill on a VMC, the low lead angle allows much higher linear feedrates at a much reduced depth of cut at the expense of higher tool pressure in the X(radial) direction as mentioned by another poster.

The groove in Bill's example was cut by feeding in on the Z axis, feeding in on the X axis, feeding in on the Z axis and then out on the X axis repeating until complete with the tool never retracting out of the material.

Jaxian · Sep 21, 2018

Ok, found the example. The turning in question starts at about the 3:30 mark. Feeds both ways and never stops the cut no tool change. Seems very efficient. Will be looking forward to trying it when the tool arrives shortly.

Cnc Lathe Cup Machining - YouTube

Where do we use button inserts?

Titanium

guest

Guest

Titanium

Hot Rolled

Titanium

Cast Iron

Cast Iron

Aluminum

guest

Guest

Aluminum

Aluminum

Stainless

Diamond

Titanium

Titanium

Diamond

Diamond

Titanium

Stainless

Stainless

Similar threads