Heidenhain control?

We have a Tos Varnsdorf bridge mill with Heidenhain control (fun stuff). I'm trying to figure out the best way to program the following:
(fanuc control)
*90 DEGREE COUNTER SINK TOOL*
;
G00X16.7875Y0.0S450M03
G43H55Z8.0M08
G98G82Z6.43R6.8P200F2.3
X16.7236Y1.4631Z6.477R6.587
X16.5325Y2.9151Z6.43
X15.7751Y5.7417
X15.2146Y7.0947Z6.45
X14.5384Y8.3938Z6.43
X12.142Y9.4424
X9.6289Y13.7515Z6.45
X14.5384Y-8.3938Z6.43
X15.7751Y-5.7417
X16.7236Y-1.4631Z6.45
G80M9
;
;
To make the above program for the heidenhain control, the program will be...???
;
N75 W-20M91
N80 X+16.7875Y0.Z+10.M03
N85 G83 P01 -0.25 P02 -.37 P03 -.37 P04 .2 P05 20.3
N90 Z+8.M8
N95 Z+7.05 M99
?
?
Not sure how to simply alter the R plane or Z plane in the heidenhain control. Anyone help?

What model of Heidenhain is it?
Have you downloaded the free programming manual for your control from the Heidenhain website?

Quote:

---

Originally Posted by rylanrouge

To make the above program for the heidenhain control, the program will be...???
;
N75 W-20M91
N80 X+16.7875Y0.Z+10.M03
N85 G83 P01 -0.25 P02 -.37 P03 -.37 P04 .2 P05 20.3
N90 Z+8.M8
N95 Z+7.05 M99
?
?
Not sure how to simply alter the R plane or Z plane in the heidenhain control. Anyone help?

---

So with the HDH G83 cycle N95 Z+7.05 is the start height (R plane), G83 P01 is the incremental distance from the start height to the work piece surface and G83 P02 is the incremental drill depth from the work piece surface. The line with M99 calls the drill cycle.

Here is where you have to be careful when you change the Z start point you also have to change the G83 P01 value. This is because everything in the G83 cycle is incremental.
So for example if you change Z+7.05 to Z+10.05 you'll have to change P01 from -0.25 to -3.25 otherwise your hole will be 3" to short.

This is an old style cycle but still good and useful.

Also G83 is the same as HDH clear-code Cycle 1