End Mill pulling to side question please

[ImanCarrot]

I've recently started machining things on a turret mill and am still finding my way about the beast (I usualy do Diamond Machining).

If I was cutting a slot using a 3mm end mill from South to North say (clockwise rotation), would the tool "pull" itself slightly to the East (ie to the right)? I can't see how it wouldn't due to the cutting happening on the NE portion of the slot and the SW bit... surely the material would "grab" the tool and try to drag it sideways?

If it does... how do folk compensate for this wandering?

Or have I got it wrong???

[Geof]

I don't align my machines to the cardinal points so I cannot answer your question as it is phrased. I can tell you however, that a clockwise turning tool will deflect to the left when looked at along the direction of tool travel.

With small tools the deflection is mostly due to the tool bending with larger tools machine deflection also comes into the picture. The holder can also influence it; I have found collet holders to be less rigid than setscrew holders for sideways tool deflection.

It is not possible to totally remove the deflection so normally you would compensate. For instance make sure your cutting direction means the cutter deflection makes the part bigger or the hole smaller; climb milling does this. When cutting a slot use a cutter smaller than the slot and take a first cut right down the center then clean up the sides to width.

Just for fun sometime to see how much deflection is possible even on a big VMC put a dial gauge on the table with the probe against the spindle and then push as hard as you can on the spindle. You may be surprised at how much you can deflect things.

[miljnor]

Just for fun sometime to see how much deflection is possible even on a big VMC put a dial gauge on the table with the probe against the spindle and then push as hard as you can on the spindle. You may be surprised at how much you can deflect things.

hopefully your talking manual milling machines

I thought I had a problem with a lathe because it was deflecting .0005 to .001 thou, but a friend gave me the same spiel as you Geof but the Haas tech said no way and now the thing doesn't show more than .0001 deflection on a push. (and I am a pretty big guy at 200lbs)

will try a VMC now and see what happens but I think I've done this before and was surprised to see any deflection but don't remember it being more than a few .0001. But then HAAS is not the most rigid machine on the planet either.

[ImanCarrot]

Thanks Geof, as always insightful info! I shall try that.

So if I was making a square pocket for example with the end mill tool spinning clockwise and cutting round the inside in a clockwise direction too, I would expect the left hand side and top to have more material removed than programmed and the right hand side and bottom less material?

What causes that then? I would have thought the reverse. I trust your info though (have read other posts by yourself), just can't get me head round it. It probably wont affect anything I'm making at the moment, but when something bugs me it won't go out of my head.

[Geof]

Originally Posted by miljnor hopefully your talking manual milling machines I thought I had a problem with a lathe because it was deflecting .0005 to .001 thou, but a friend gave me the same spiel as you Geof but the Haas tech said no way and now the thing doesn't show more than .0001 deflection on a push. (and I am a pretty big guy at 200lbs) will try a VMC now and see what happens but I think I've done this before and was surprised to see any deflection but don't remember it being more than a few .0001. But then HAAS is not the most rigid machine on the planet either.

I have done both but what was in my mind was my VF2 because I did it not long ago. So I went out and did it again.

0.0005" deflection but as I was doing it I realised I am a dummy; I was pulling on a long tool holder in the spindle, not pushing, and I had braced myself with my foot against the table. So I was seeing combined deflection; spindle one way table the other at a load of at least 100lbs.

So that is not really surprising.

[thkoutsidthebox]

I don't understand why a circular shaped tool, spinning around the center point of its diameter, deflects at all?
Especially if it has two cutting faces on opposite sides, would the forces not cancel/balance each other out?

[Geof]

Originally Posted by ImanCarrot Thanks Geof, as always insightful info! I shall try that. So if I was making a square pocket for example with the end mill tool spinning clockwise and cutting round the inside in a clockwise direction too, I would expect the left hand side and top to have more material removed than programmed and the right hand side and bottom less material? What causes that then? I would have thought the reverse. I trust your info though (have read other posts by yourself), just can't get me head round it. It probably wont affect anything I'm making at the moment, but when something bugs me it won't go out of my head.

I am not sure you should trust me, see immediately previous post from me.

If you are inside, tool spinning clockwise and following a clockwise path you are conventional milling and the deflection will cause the tool to cut slightly outside the programmed path all the way round.

Make yourself a sketch showing the force vectors on the tool.

[Geof]

Originally Posted by thkoutsidthebox I don't understand why a circular shaped tool, spinning around the center point of its diameter, deflects at all? Especially if it has two cutting faces on opposite sides, would the forces not cancel/balance each other out?

Only one, or fewer than half the total number of teeth, are cutting at any one time. As I mentioned draw a sketch showing the force vectors and it should be clear.

[msomerville]

Originally Posted by thkoutsidthebox I don't understand why a circular shaped tool, spinning around the center point of its diameter, deflects at all? Especially if it has two cutting faces on opposite sides, would the forces not cancel/balance each other out?

If you were cutting on both sides of the tool it would take at least most of the deflection out.

[Geof]

Originally Posted by msomerville If you were cutting on both sides of the tool it would take at least most of the deflection out.

When the tool is travelling vertically, i.e., plunging it will cut on all teeth. When the tool is travelling horizontally and facing it has only a small arc of engagement, when slotting it has a full semicircle of engagement but there is no way you can get teeth cutting on both sides.

[DareBee]

Originally Posted by thkoutsidthebox I don't understand why a circular shaped tool, spinning around the center point of its diameter, deflects at all? Especially if it has two cutting faces on opposite sides, would the forces not cancel/balance each other out?

When slotting solid you are actually in contact with 180 degrees of the cutter - yes the force on both sides more or less cancel out but the force along the top edge in direction of travel is the diorection that the cutter deflects.

This deflection issue is why I only use carbide for .25 (6mm) and smaller cutters. Cheap carbide cutters are barely more money than HSS.
Also take light fast cuts (try .2 - .3mm DOC)

[handlewanker]

Hi all, to clarify brother carrot's dilemma, consider cutting a 6mm or 1/4" wide keyway in the middle of a mild steel shaft.
The tendancy would be to dive in full depth, 3mm or 1/8" deep, and feed along the shaft to the end of the desired keyway length.
You will get deflection to the left of the cutter, as it normally runs clockwise looking down on top of the spindle end.
As the cutter tooth rotates it feeds against the material on it's left side going forward and away from the material on it's right side.
If you were drilling straight down then the cut would be central and equal on both cutting edge ends.
It is normal to cut keyways and deep slots by shallow cuts and reversing the cut at each end till the depth of slot is reached.
Cutting from one end only, and returning to the beginning and repeating the cut will leave a series of steps in one face of the slot.
This becomes worse for long series cutters when machining deep cavities, requiring an allowance for full face milling to clean up the sides of the cavity.
This tendency should be taken in consideration when running an end mill round the outside of a job, as it will tend to dig in at the end of the cut when the forward feed stops.
Allowance is usually made to do a finishing cut at reduced feed with the full face of the cutter.
Cutting on a full face will always leave a ripple finish on the job and is the least efficient way of material removal, and least accurate, usually resorted to when a profile is being milled in one set-up.
This is one of the reasons why when milling in a CNC mode with carbide cutters, a high speed and shallow cut is used, so that the material is reduced to a powdery swarf by many small cuts, as opposed to large chips generated by HSS cutters running much slower, and so gives hardly any deflection to the tool, almost a grinding action, which by the nature of the cutting edge it actually is.
Ian.