Cycle 485 MEASURE LATHE TOOL

ISO programming

G485

Application

 
Machine

Refer to your machine manual!

Machine and control must be specially prepared by the machine manufacturer for use of this cycle.

Cycle 485 MEASURE LATHE TOOL is available for the measurement of turning tools with a tool touch probe from HEIDENHAIN. The probe contact must have a cuboid shape. The control measures the tool in a fixed programmed sequence.

Cycle run

  1. The control positions the turning tool to the clearance height.
  2. The turning tool is oriented based on the entries in TO and ORI.
  3. The control moves the tool to the measuring position in the main axis; the traverse movement is interpolated in the main and secondary axes.
  4. Then the turning tool moves to the measuring position in the tool axis.
  5. The tool is measured. Depending on the definition of Q340, either tool dimensions are changed or the tool is locked
  6. The measuring result is transferred to the result parameter Q199.
  7. After the measurement has been performed, the control positions the tool in the tool axis to the clearance height.
Result parameter Q199:

Result

Meaning

0

Tool dimensions within the tolerance LTOL / RTOL

Tool is not locked

1

Tool dimensions outside the tolerance LTOL / RTOL

Tool is locked

2

Tool dimensions outside the tolerance LBREAK / RBREAK

Tool is locked

The cycle uses the following entries from toolturn.trn:

Abbr.

Entries

Dialog

ZL

Tool length 1 (Z direction)

Tool length 1?

XL

Tool length 2 (X direction)

Tool length 2?

DZL

Delta value of tool length 1 (Z direction), is added to ZL

Oversize in tool length 1?

DXL

Delta value of tool length 2 (X direction), is added to XL

Oversize in tool length 2?

RS

Cutting edge radius: If contours were programmed with radius compensation RL or RR, the control takes the cutter radius into account in turning cycles, and performs tool tip radius compensation

Cutting edge radius?

TO

Tool orientation: From the tool orientation, the control determines the position of the tool cutting edge and, depending on the selected tool type, additional information such as the tool angle direction, position of the tool reference point, etc. This information is necessary, for example, for calculating the tool tip radius compensation, milling cutter radius compensation, plunge angle, etc.

Tool orientation?

ORI

Spindle orientation angle: Angle of the indexable insert to the main axis

Angle of spindle orientation?

TYPE

Type of turning tool: Roughing tool ROUGH, finishing tool FINISH, threading tool THREAD, recessing tool RECESS, button tool BUTTON, recess-turning tool RECTURN

Type of turning tool

Tool orientation (TO) that is supported for the following types of turning tools (TYPE)

Tool orientation (TO) that is supported for the following types of turning tools (TYPE)

TYPE

Supported TO
with possible limitations

Non-supported TO

ROUGH,

FINISH

  • 1
  • 7
  • 2, only XL
  • 3, only XL
  • 5, only XL
  • 6, only XL
  • 8, only ZL
  • 18
  • 4
  • 9

BUTTON

  • 1
  • 7
  • 2, only XL
  • 3, only XL
  • 5, only XL
  • 6, only XL
  • 8, only ZL
  • 4
  • 9

RECESS,

RECTURN

  • 1
  • 7
  • 8
  • 2
  • 3, only XL
  • 5, only XL
  • 4
  • 6
  • 9

THREAD

  • 1
  • 7
  • 8
  • 2
  • 3, only XL
  • 5, only XL
  • 4
  • 6
  • 9

Notes

 
Notice
Danger of collision!
If you set stopOnCheck (no. 122717) to FALSE, the control does not evaluate the result parameter Q199 and the NC program is not stopped if the breakage tolerance is exceeded. There is a danger of collision!
  1. Set stopOnCheck (no. 122717) to TRUE
  2. You must then take steps to ensure that the NC program stops if the breakage tolerance is exceeded
 
Notice
Danger of collision!
If the tool data ZL / DZL and XL / DXL deviate by more than ±2 mm from the real tool data, then there is a danger of collision.
  1. Enter the approximate tool data closer than ±2 mm
  2. Run the cycle carefully
  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • Before you begin the cycle, you must run a TOOL CALL with the tool axis Z.
  • If you define YL and DYL with a value outside of ±5 mm, the tool won't reach the tool touch probe.
  • The cycle does not support SPB-INSERT (angular offset). You must enter the value 0 in SPB-INSERT, otherwise the control will generate an error message.

Note regarding machine parameters

  • The cycle depends on the optional machine parameter CfgTTRectStylus (no. 114300). Refer to your machine manual.

Cycle parameters

Help graphic

Parameter

Q340 Tool measurement mode (0-2)?

Use of the measured values:

0: The measured values are entered in ZL and XL. If values are already entered in the tool table, they will be overwritten. DZL and DXL will be reset to 0. TL will not be changed

1: The measured values ZL and XL are compared with the values from the tool table. These values will not be changed. The control then calculates the deviations of ZL and XL, and enters these in DZL and DXL. If the delta values are larger than the permissible wear or breakage tolerance, the control locks the tool (TL = Tool Locked). In addition, the deviation is also entered in the Q parameters Q115 and Q116

2: The measured values ZL and XL as well as DZL and DXL are compared with the values from the tool table, but are not changed. If the values are larger than the permissible wear or breakage tolerance, the control locks the tool (TL = Tool Locked).

Input: 0, 1, 2

Q260 Clearance height?

Enter the position in the spindle axis at which there is no danger of collision with the workpiece or fixtures. The clearance height is referenced to the active workpiece preset. If you enter such a small clearance height that the tool tip would lie below the top of the probe contact, the control automatically positions the tool above the top of the probe contact (safety zone from safetyDistStylus).

Input: –99999.9999...+99999.9999

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

Example

11 TOOL CALL 12 Z

12 TCH PROBE 485 MEASURE LATHE TOOL ~

Q340=+1

;CHECK ~

Q260=+100

;CLEARANCE HEIGHT