chatter on bore out

[kendo]

I just ran my pinzbohr mini adjustable boring head at .7518 dia
I used G85 bore in/bore out to do it
I watched close as the tool bored in and it was making a great finish, but when it bored out, it squealed and chattered the finish all to he11

anybody know why it did that?

I'm new to boring holes to tight tolerance so I could use some help on this one

I milled the hole 1st and left .005 per side for the boring head
1200 RPM
and 10 IPM
1/2" plate of 6061 - .7518 thru hole
thanks a bunch for any help

Kenny

[Geof]

You probably know that one way to avoid chatter on a boring tool is to keep a fairly good depth of cut and feed. That is okay when you are boring in but a lot of times a boring tool will chatter on the way out because it is not really cutting just rubbing so there is no load on the tool and nothing to stop it starting to vibrate and things go from bad to worse.

There are boring cycles where you stop the spindle at the bottom with an orient spindle command, then move the X or Y axis so the tool is not touching and pull the tool out.

[kendo]

thanks Geof,
I was gonna explore the cycle you mention on monday morning

but, the machine has to know that whenn it orients the spindle to say 0 degrees, which way the boring bar is pointed in order to back off the right direction, correct?

[Geof]

You have to know which way the boring tip is facing after the spindle is oriented so that you program the correct move away.

[losiman]

I run alot of 2-8" bores holding .005" or tighter. We run custom built tooling with Sandvik cartridges. For cast steel, ductile, and cast iron we take .015"-.025" per side, and we G85 nearly all bores. So possibly deeper finish cut will help. Also as mentioned, try bore cycle where spindle stops, orients, X or Y moves say .005-.010 then rapids out. Good luck.

[ikneb]

Why not helical bore it with an endmill

[Geof]

Originally Posted by ikneb Why not helical bore it with an endmill

It depends on what the tolerance is:

Holding +/-0.0002" on both diameter and concentricity with a boring head is not unreasonable; actually you can probably get better than this without too much difficulty.

When interpolating +/-0.0002" is getting optimistic and very often an interpolated hole will be out-of-round by this amount or more because it is created by motion of two linear axes each with their own inherent inaccuracies, and much more importantly backlash.

[3axisrookie]

+-.001 I would mill bore. Anything smaller I use a boring bar.

Maybe you're taking too much of a cut and getting some deflection? That's what I would try first.

[Mitsui Seiki]

Make sure your insert is screwed tight.

[ikneb]

I have milled bores as close as +/-.0005 on a 15 year old Johnford and as close as +/-.0001 on my Hardinges.
I folow some rules when I need to be that close
1:use an endmill that less than 1/2 the hole dia.
2:arc on and off
3:do 3 or more passes
4:if its a helical bore feed the endmill the depth per rotation past the hole

[cam53]

Originally Posted by 3axisrookie +-.001 I would mill bore. Anything smaller I use a boring bar. Maybe you're taking too much of a cut and getting some deflection? That's what I would try first.

try G86 cycle ,that a bore stop out of the hole,i use this all the time works for me.

[mattpatt]

I have a FADAL 3016, using Fanuc 0i controller.

When I use G85 everything is as it should be. Bore in, bore out.

When I want to use G86, what is the exact procedure?

If I use what works with G85, but just change to G86, the tool bores in, then stop and rapids out. Then the spindle orients. The problem is that the spindle rapids out before it has come to a comple stop. I haven't actually cut using the G86 cycle yet, I just tested it in the air. I haven't set any X,Y coordinates for it to move to before rapiding out. Maybe that's the problem?

Here's my code for G85:

N135 X28.5 Y-40.2 Z27. (1st Bore)
N140 G98 G85 Z0. R27. F50
N145 X220.5 (2nd Bore)
N150 G80

I changed it to:

N135 X28.5 Y-40.2 Z27. (1st Bore)
N140 G98 G86 Z0. R27. F50
N145 X220.5 (2nd Bore)
N150 G80

But the results were as I explained above.

Can any one explain where I'm going wrong? Probably something very simple.

Thanks.

Matt.