angelw, I'm assuming that is all in metric.
Yes.
That X-1.6 in line 3 threw me off though. Is that facing past X0 for manual TNR comp?
Yes. The Tool Nose Radius used in this example program is 0.8mm. Accordingly, for the TNR to face right to X0.0, it has to go past X0.0 by the TNR, hence the X diameter coordinate of -1.6.
Even if TNR Comp is going to be used at the control (not compensated for in the Part Program) in the machining of the profile shape, its a nonsense to use Control TNR Comp when facing a perpendicular to centre line face of a work-piece for the following reasons:
1. There is no compensation to be calculated if using a typical facing tools such as a RH OD Turning tool.
2. When you reach X0.0, its typical to feed away from the face a small amount. This action in itself will prevent the X Centre of the TNR actually reaching X0.0 when using Control TNR Comp; you would still have to program X-1.6 irrespective of TNR Comp being used, or not.
3. When facing from Outside to Centre, the TNR Comp G code will be different to when OD turning towards the chuck and you need to be mindful of changing from G41 (for the face) to G42 for the OD Turning.
Also wondering what program that is.
My own.
I'm a bit confused by the G0 G1 G2 G3 that I see. It's making me thing it's going to rapid all the way Z-. It's still not clicking for me at this time. I'm going to come back in a few.
These are preparatory codes that set the control to Rapid Traverse, Linear Interpolate, CW Circular Interpolate and CCW Circular Interpolate respectively. If you study the code in the example program, the only Rapid Move specified in the Profile Definition is the First Block (the P Block). Forgetting about roughing for the moment, if you were to simply take a Finish Cut on the specified profile, you would first Rapid to X28.400 and start the Finish operation form there. As the Tool was initially positioned at Z3.0 with the
G00 X82.400 Z3.000
block that precedes the First G71 Block, the move to X28.400 would be through fresh air; no Rapid move to Z-.
From your other Thread on Tool movement, I glean that your control is a Mitsubishi M70. The Multi-repetitive cycles of the M70 control are similar to the Fanuc two Block Format, with the addition of a couple addresses.
With a Fanuc Control there is Type I and Type II G71/G72 cycles. Type I only allows monotonous direction of X coordinates (no pocketing) for the G71 cycle; Type II allow noncontinuous X coordinates (pocketing). Whether Type I, or II is initiated is dependent on whether the P Block of the Profile Description has just a one, or two axis move. With the Mitsubishi M70 control, a H address is used in the First G71 Block to specify Pocketing (H1), or not (H0). Also with the M70 Control, another Profile Shape Program Number can be specified with an address A in the Second G71 Block. If omitted, the current program is used (most usual).
Example:
G00 X82.400 Z3.000
G01 Z0.15 F1.0
(ROUGH FACE STARTS HERE)
G01 X-1.6 F0.25
G01 Z1.0
G00 X82.000
(ROUGH FACE FINISHES HERE)
G71 U4.0 R0.5
G71 A100 P100 Q101 U0.5 W0.15 F0.25
G70 A100 P100 Q101
--------
--------
--------
Shape Program
O100
N100 G00 X28.400
G01 Z0.000
G03 X40.000 Z-5.800 I0.000 K-5.800
G01 Z-20.469
G01 X76.602 Z-38.770
G03 X80.000 Z-42.871 I-4.101 K-4.101
G01 Z-55.000
N101 G01 X82.400
G00 Z3.000
Regards,
Bill