Horn mini bore chatter chatte chatter !

Hello,

I'm trying to do a I assumed simple internal profiling, initial hole is 12.75mm (0.50197")(taped to M14 x 1.25 latter) by 50 mm long and I'm profiling two 15 mm diameter recess, one from Z-42.5mm (-1.67323 ") to Z-26.5mm (-1.04331") and a the other from Z-17mm (-0.66929") to Z0mm in low carbon steel (should be easy right ?)

I'm using a Horn Mini boring bar (carbide shank) reference B111.0012.03 it's the 56mm (2.20472") reach one with internal coolant with a 8mm diameter (0.31496") held in a VDI30 16 mm E2S holder (the kind that clamps the tool via a split not via set screw so in theory less vibration) on a HAAS SL10 and the insert is a R111.0200.02 TN35 (internal profiling coated)

Horn has (IMO) poor documentation when it come to feeds and speeds they mention 241m/min cutting speed (790 sfm) and a feed going from 0.05mm/T to 0.01mm/T (0.00197"/T to 0.00039"/T) for very rigid to not rigid setup.

I started out with a 150m/min cutting speed (492sfm) with a 0.01 mm/T feed (0.00197"/T) and it chattered at a high pitch and consequently I got insert chipping... changed the insert (15 euros.. grrr) and went with 75 m/min cutting speed (246sfm) with the same feed and it made absolutely no difference !

Could this be more of a centerline issue ?
I can try t slightly rotate the tool holder in the E2S holder so as to lower or raise the tool tip position in relation to the centerline, but for a ID I should raise it rather than lower it ?

I think the SFM is less important than the feed. You say you tried .01mm but then say it is .00197” which is .05mm in feed? Which did you actually run? Of course running on center is important. So if you’re not do it

draw on paper how the ID cut looks like axially and it will be immediately apparent why it is important for the tool to be above the center line and not below and why it is exactly the opposite for OD turning

by how much above (or below) will be dictated by the rigidity of the setup and DOC

Shop Supply Guru said:

I think the SFM is less important than the feed. You say you tried .01mm but then say it is .00197” which is .05mm in feed? Which did you actually run? Of course running on center is important. So if you’re not do it

Click to expand...

Ooops my mistake, it was 0.01 mm/T ie 0.00039"/T (imperial is very awkward for me but I know many of you feel the same way about the metric system :-) )

jz79 said:

draw on paper how the ID cut looks like axially and it will be immediately apparent why it is important for the tool to be above the center line and not below and why it is exactly the opposite for OD turning

by how much above (or below) will be dictated by the rigidity of the setup and DOC

Click to expand...

Ok so if working on the feed yields no result I'll try to nudge the tool above the CL and see if that works, how much though ?
About 0.05 mm ?
Assuming I even find a reliable way of measuring this.... bellow centerline is easier, you see if going to CL with the tool on a practice scrap leaves a "nub" and how big but above is trickier IMO

So you have D=8mm carbide boring bar with 56mm hang out (7:1 L/D ratio) and attempting to plunge 2mm wide insert at once. I'd be surprised if you didn't get chatter!

Setting the boring bar clearly above center can help somewhat. 3% of diameter (about 0.4mm in your case) above center has negligible effect on cutting angles but you need to calculate the actual diameter you get with that.

Does the contoured shape need to have 90-degree corners on both side? If not move to insert that does not have 2mm wide contact with the workpiece.

I agree with MattiJ's post above. A 2 mm wide grooving bar at a 7:1 L/D ratio will be prone to chatter, even though it's carbide. If possible, I would change to a profiling insert, or at least a narrower width grooving insert.
If that's not possible, there are other things you can try...
You didn't mention if you were getting chatter when you feed up in the X, or feeding across in the Z direction. If it's only in the Z direction, you can try feeding away from the spindle instead of towards the spindle. This can help. Another trick that sometimes works is to flip your bar upside down and change your program to work in the negative X direction. This sends the cutting force down into the base of the machine instead of lifting the turret.
Good luck.