HAAS ST20 G42 cutting a taper

Hi guys,

I've been cutting some shafts today on my ST-20 and I've come across a bit of an anomaly I can't figure out - I'm hoping someone with a bit more experience may be able to shed some light for me!

Program goes as follows:

N100 G00 X34.6;
G01 G42 Z0. F0.12;
X34.8 Z-0.1;
Z-100.;
X35.8;
X36. Z-100.1;
Z-406. ,R0.600;
N200 G00 G40 X42;


Now for some reason on the Z-406 move it cuts a programmed 0.234 mm taper and this is displayed in the "distance to go" positions screen as it counts down to 0 when Z reaches -406. If you remove the G42 line entirely it cuts straight but the 0.1 chamfers are missed due to the tool nose radius.

At first I thought maybe a taper correction was programmed somewhere but I can't see an option for it on the tool offsets or in a settings search for taper. What's also puzzling is that this does not happen on the X34.8 mm diameter, only the X36.0 mm diameter.

Any help would be greatly appreciated!

is .234 a multiple of your compensation value? if so, make sure you have a large enough lead-in and lead-out that compensation can be correctly applied.

Where does Z positioned before executing this code?

Thanks for the reply.

I'm cutting a 45 degree taper with a 0.4 mm tool rad so my compensation value is 0.234 mm which ties in with the taper I am seeing. The Z axis is at 2.0 mm in front of the face prior to the sub routine.

Should I be programming a linear cutting move to X42 on completion of the profile to clear the stock for lead out?

To me it looks like you are cancelling cutter comp in the middle of a cut.

SICDLtd said:

N100 G00 X34.6;
G01 G42 Z0. F0.12;
X34.8 Z-0.1;
Z-100.;
X35.8;
X36. Z-100.1;
Z-406. ,R0.600;
N200 G00 G40 X42;

Click to expand...

Hello SICDLtd,
If you're going to apply TNR Comp via the Z0 move, the tool in X would have to be at least at X34.132 to be able to cut the 0.1 chamfer, but starting the cut right on the corner of the chamfer is not a good idea.

A better method would be to start slightly clear of the face in Z as follows:

N100 G00 X35.6 Z0.5;
G01 G42 X34.4 Z0.1 F0.12;
X34.8 Z-0.1;
etc.

or start further down the face in X as follows:

N100 G00 X34.0 Z0.5;
G01 G42 Z0. F0.12;
X34.6
X34.8 Z-0.1;
etc.

Also, when using automatic radius cutting in Linear Interpolation, follow the Z move with at least a small X move as follows:

X36. Z-100.1;
Z-406. ,R0.600;
X38.0 (This represents only a 0.4 radial X move)
N200 G00 G40 X42;

You're using a Feed Rate of 0.12; accordingly, when cutting the 0.1 chamfer you will loose detail because it will be consumed in less than one rotation of the spindle. Use a finer Feed Rate on the chamfers and revert back to F0.12 on the longer cuts.

Regards,

Bill

Thank you for your reply Bill - it was very helpful.

Over the weekend I tried adding an a move in X after the -406 in Z which solved the taper cutting issue. It seems that the control is cancelling the cutter comp on the Z-406 move as FrankieB implied whereas the manual and the programming examples within it suggest that it should have been cancelled on the rapid to X42.

I have also taken on board your comments regarding the start position and feed.

SICDLtd said:

Should I be programming a linear cutting move to X42 on completion of the profile to clear the stock for lead out?

Click to expand...

Bingo! Always add a straight G1 move in X before cancelling G42.

SICDLtd said:

Thank you for your reply Bill - it was very helpful.

Over the weekend I tried adding an a move in X after the -406 in Z which solved the taper cutting issue. It seems that the control is cancelling the cutter comp on the Z-406 move as FrankieB implied whereas the manual and the programming examples within it suggest that it should have been cancelled on the rapid to X42.

I have also taken on board your comments regarding the start position and feed.

Click to expand...

Hello SICDLtd,
I think you will find that it has more to do with not following your G01 Radius feature applied in Z with an X move than cancelling TNR Comp with G00, as cancelling TNR Comp with G00 is quite legal.

I believe the following will work:

X36. Z-100.1;
Z-406. ,R0.600;
X38.0 (This represents only a 0.4 radial X move)
N200 G00 G40 X42.0;

as will the following work

X36. Z-100.1
Z-405.4
G02 X37.2 Z-406.0 I0.6 K0.0
N200 G00 G40 X42.0

Something that you won't often use, as more often than not you clear the work before cancelling TNR Comp, but in the two examples shown in the following pictures, where TNR Comp is cancelled at the end of an element where workpiece exists following, you can specify that material exists by the inclusion of an I and K (for a lathe) address describing the geometry of the next element.



With no I and K specified, over-cutting of the next element occurs when TNR Comp is cancelled.



With I and K specified, the TNR finishes tangent to the next element before TNR Comp is cancelled.

Regards,

Bill

SICDLtd said:

N100 G00 X34.6;
G01 G42 Z0. F0.12;
X34.8 Z-0.1;
Z-100.;
X35.8;
X36. Z-100.1;
Z-406. R0.600;
G01 X42.
N200 G00 G40 X44;

Click to expand...

The problem is in the comp-off block.
The Z-406. R.6 is a .6mm radius at the end, and the control expects a wall to blend to.
But, you are telling it to not only blend, but cancel comp in one fell swoop.

I did not test out your profile and really do not know what exactly are you doing, but the above is just from how I'd do it something similar.....