[balal]

For machining my cavity I tried the facemill 4 round tips instead of HSS or carbide end mills due to the fact that i had to create a big pocket so a facemill will 50mm dia looked the right choice.

I know that facemill are not best for pocketing so I created a bore throughout my cavity so that my facemill's all for tips are not in contact while taking the depth of cut. So i generated a programme which would take the depth in the empth bore in the centre of the workpiece in the empthy bore and then only one side of the mill comes in contact woth the workpiece.
However this was unsucessful even when i took a depth of 0.3, the mill made enormous noise and the surface of the workpiece had deep lines on it. my spindle was at 800 and feed was also 800 mm/min,

waiting for ideas.

[little bubba]

You're looking at a pile of different factors. First, what was the material, second, what was the make and style of the facemill, and third what was the machine.

A super floppy, sloppy piece of crap machine in any material isn't going to work well with 2" facemill. A nice rigid machine with a crappy 80's geometry facemill will do just as bad.

I'm voting for more info.

[dertsap]

noise is what facemills do when pocketing , especially on the initial engagement , if it starts to chatter on engagment it will in general carry thru till the cut is done ,
800 rpm is a little slow i don t know what your cutting but if its anywhere near 4140,i would double up the speed ,you could be dealing with a certain amount harmonics that you ll have to find that sweet spot to get past it , try cutting at .2 and .007 chip load

hard for us to judge with limited info though , is your holders cat40 or 50

90 deg facemills are designed to face or hog , can t expect too good of a finish when hogging
as far as tha lines go dial up the inserts to make sure they are 90 deg and not tapered
but i suspect its a rigidity issue

[balal]

Thanks guys,

taking this further i tried a 0.2mm depth of cut on my medium carbon workpiece. Its hardness would be aprrox 50 on the hardness table.

Also i would llike to mention that the face mill is one which has circular inserts and not pointed ones like triangle or rectanular ones.

When the cutter engaged the workpiece it was cutting with a lot of polish and no load or noise. however once it moves further for example after taking the next depth or going through a radius it starts to make noise and then continues to make noise and also rough the workpiece, i used cold air for the flushing of the chips.

can u guys guide me to a resource where i can learn the fundamentals of this cutter ...

also, what impact does the clearence area of the insert from the face mill have on cutting. that is from the bottom surface of the face mill to the cutting edge of the insert. Is it the maximun amoount of depth cut i can take?

I am using a BT40 Arbour? so the machine is not as strong as Bt 50 ...

I even repeated the excersice with 0.1 mm cut but it never worked?? it still made noise?

waiting!

[dertsap]

sorry when i posted to cut at .2 i meant inches , i dont have much experience with those cutters other than facing , but i do understand they are designed for pocketing and ramp cutting , i would do a google search
how about drilling out the excess material then pocketing the remainder , if you have a U drill ,you would be able to remove a lot of material fast , 1" (25.4mm) u drill , s1800 @5-6 ipm , easily!!

[ViperTX]

Since you are machining steel and the problems that you've indicated....I'm suspecting that either the face mill is too large for your mill's drive motor, or you have some rigidity problems....most likely bearing related....

[fpworks]

I would initially say that it is probably a rigidity problem of some sort. (machine structure, spindle, drawbar, workholding) But like Bubba said, more informatin is needed.

More considerations:

Round inserts tend to allow more aggressive cutting, since they transmit [some] of the load axially into the spindle. Having said that, you should be easily cutting 2 mm per pass on a BT40 machine.

Also, insert cutters just tend to be loud, especially if the inserts are positioned with little rake in the cutter body. (this is typical)

What is the radius of the corners in the pockets you are machining? Are these 90 degree corners, or less/more? If the cutter is close to the radius as your corner, expect chatter. (or select a different sized tool)

When you are moving to the next depth, what ramp angle are you using? The manufacturer of your cutter can tell you the maximum ramp angle. If you don't know, 3 degrees is conservative. Expect more noise during any cut that has a vertical component into the workpiece.

Is your workholding situation for this workpiece optimal? I use large diameter insert cutters only when the workpiece is very well supported.

[dertsap]

round inserts will have a much larger cutting surface than a 90 deg cutter at the same depth ,this with the posible rigidity problem would cause a lot of noise ,insert grade could be an issue ,
if it s only noise and you have no damage to the cutter , i say let er rip ,
i haven t hogged out many pockets in steels that were quiet

[big_mak]

Balal,

As you get deeper into the pocket, your area of contact at the periphery of the pocket will increase, thus the inserts will be cutting the depth of the radius of the inserts when you are cutting the finished profile of the pocket.

Some tooling vendors are now offering these feed mills that can cut up to 3mm/tooth, at a DOC of around 1.5mm. They also recomend that when you get to a wall the your feed rates be reduced. These cutters work on an exagerated principal of chip thinning and are supposed to push the cutting forces axially along the z axis into the spindle.

I'd follow the insert manufacturers recommendations for Cutting speed for the inserts, but if you want to keep your DOC small, crank the living daylights out of the feed rate for most of the pockets, then reduce it to a point where you are comfortable with the results.

You could also make a program to use this face mill to cut the pocket with a slight draft angle, keeping your feedrates constant as your depth of engaement will not increase, then use a ripper cutter, to square up the sides.

This round profile tool, should be extremely productive if apllied properly, even if you have a machine that is not necessarily the most rigid one on the market.

Believe me, I've used this cutter geometry on 40 year old used and abused beasts where the whole head would shift 1mm when you changed directions on X axis.

That current beast is at the bottom of a river now I believe.

Cheers, and keep making chips.