Cycle 441 FAST PROBING (#17 / #1-05-1)

ISO programming

G441

Application

You can use touch probe cycle 441 to globally specify various touch probe parameters (e.g., the positioning feed rate) for all subsequently used touch probe cycles.

 
Tip

In this cycle, no machine movements will be performed.

Program interruption Q400=1

Parameter Q400 INTERRUPTION allows interrupting the cycle run and displaying the obtained results.

Program interruption by Q400 is effective in the following touch probe cycles:

  • Touch probe cycles for checking the workpiece: 421 to 427, 430 and 431
  • Cycle 444 PROBING IN 3-D
  • Touch probe cycles for measuring the kinematics: 45x
  • Touch probe cycles for calibrating: 46x
  • Touch probe cycles 14xx

Cycles 421 to 427, 430 and 431:

The control displays the results obtained during a program interruption in an FN 16 monitor output.

Cycles 444, 45x, 46x, 14xx:

The control automatically shows the results obtained during a program interruption in an HTML log in the path: TNC:\TCHPRlast.html. You can open the HTML log in the Document workspace.

Notes

  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • END PGM, M2, M30 reset the global settings of Cycle 441.
  • Cycle parameter Q399 depends on your machine configuration. Your machine manufacturer is responsible for the setting of whether the touch probe can be oriented through an NC program.
  • Even if your machine has separate potentiometers for rapid traverse and feed rate, you can control the feed rate with the feed rate potentiometer only, even with Q397=1.
  • If Q371 is unequal to 0 and the stylus does not move in cycles 14xx, the control will terminate the cycle. The control returns the touch probe to the clearance height and saves the workpiece status 3 in Q parameter Q183. The NC program continues.
  • Workpiece status 3: Stylus does not move

  • If you execute this cycle in combination with Cycles 42x or 43x and want to output a measuring log to the screen, you must program Q400=1. Otherwise the control will not interrupt and the measuring log will not be displayed on the screen.

Note regarding machine parameters

  • The machine parameter maxTouchFeed (no. 122602) allows the machine manufacturer to limit the feed rate. You define the maximum absolute feed rate in this machine parameter.

Cycle parameters

Help graphic

Parameter

Q396 Positioning feed rate?

Define the feed rate at which the touch probe will be moved to the specified positions.

Input: 0...99999.999

Q397 Pre-pos. at machine's rapid?

Define whether the control, when prepositioning the touch probe, traverses at FMAX feed rate (machine's rapid traverse):

0: Pre-position at the feed rate from Q396

1: Pre-position at the machine's rapid traverse FMAX

Input: 0, 1

Q399 Angle tracking (0/1)?

Define whether the control will orient the touch probe before every probing operation:

0: Do not orient the spindle

1: Orient the spindle before every probing operation (increased accuracy)?

Input: 0, 1

Q400 Automatic interruption?

Define whether the control will interrupt program run and output the measurement results on the screen following a touch probe cycle:

0: Do not interrupt program run even if, in the specific touch probe cycle, the output of measurement results on the screen is selected

1: Interrupt program run and output measurement results on the screen. You can then resume the NC program run with NC Start.

Input: 0, 1

Program interruption Q400=1

Q371 Touch point not reached? (optional)

Define how the control behaves when the stylus does not move within the DIST value of the touch probe table.

0: The control interrupts the NC program with an error message saying that the touch point cannot be reached. This is standard behavior.

1: The control displays a warning and terminates the touch probe cycle. The NC program continues. Is effective only in the 14xx cycles.

2: The control displays no warning and terminates the touch probe cycle. The NC program continues. Is effective only in the 14xx cycles.

Input: 0, 1, 2

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 TCH PROBE 441 FAST PROBING ~

Q396=+3000

;POSITIONING FEEDRATE ~

Q397=+0

;SELECT FEED RATE ~

Q399=+1

;ANGLE TRACKING ~

Q400=+1

;INTERRUPTION ~

Q371=+0

;TOUCH POINT REACTION