VERICUT Users' Forum

calpay2009

Member

Registered: 2009-01-27

Posts: 4

Heid.MillPlus Drilling Cycles - How to get the previous Z

I want to make the previous Z coordinate, the part surface for drilling cycles.

We have our codes like the below. The Z in the N1905 is the tool stopping over the hole center and then it makes a drilling move with 0.15mm (which is in the line N1909) downwards starting from the Z coordinate in the line N1905.

N1905 Z0.513 F30
N1906
N1907 G26 I2=3
N1908
N1909 G81 Y0 Z-0.15 B1.5 F1.9
N1910 G79 X0 Y1.1965
N1911 G1 Z1.613 F200

if you want to check the controller click here : http://www.ucgenyazilim.com/dosya/CEM.zip

SergeV

Senior Member

From: Irvine, CA

Registered: 2004-10-08

Posts: 507

Website

Re: Heid.MillPlus Drilling Cycles - How to get the previous Z

The problem is that the Z axis is not called with the G79. In the VERICUt contol, the Part Surface level is defined by the Z with G79.

from the Heidenhain MillPlus manual:
The first G79-block, which follows a defined fixed cycle, must contain a tool axis coordinate.

But if it works on your machine as you describe, you can correct the VERICUT control to support it.

To fix this, in the control file:

Configuration > Word/Address
expand under Register
Expand Z *
Select the condition: (G79) and (MOTION_PLANE XY), select the macro SteCyclePartSurface
right-click, Copy
Select the last condition * *, select ZAxisMotion
right-Click, Paste

Save your control. This should process correctly.