Fundamentals of touch probe cycles 14xx (#17 / #1-05-1)

Application

The touch probe cycles contain the following:

  • Consideration of active machine kinematics
  • Semi-automatic probing
  • Monitoring of tolerances
  • Consideration of 3D calibration
  • Simultaneous measurement of rotation and position
Explanation of terms

Designation

Short description

Nominal position

Position in the drawing (e.g., position of a hole)

Nominal dimension

Dimension in the drawing (e.g., hole diameter)

Actual position

Measured position (e.g., position of a hole)

Actual dimension

Measured dimension (e.g., hole diameter)

I-CS


I-CS: Input Coordinate System

W-CS


W-CS: Workpiece Coordinate System

Object

Object to be probed: circle, stud, plane, edge

Evaluation

Measurement results in Q parameters

The control saves the measurement results of the respective touch probe cycle in the globally effective Q parameters Q9xx. You can use the parameters in your NC program. Note the table of result parameters listed with every cycle description.

Preset and tool axis

The control sets the preset in the working plane based on the touch probe axis that you defined in your measuring program.

Active touch probe axis

Preset setting in

Z

X and Y

Y

Z and X

X

Y and Z

Notes

  • If you want to probe objects in a consistent machining plane or probe objects while TCPM is active, you can program any required shifts as basic transformations in the preset table.
  • Rotations can be written to the basic transformations of the preset table as basic rotations or as axial offsets from the first rotary table axis, seen from the workpiece.

Protocol

The measured results are recorded in the TCHPRAUTO.html file and stored in the Q parameters programmed for this cycle.

The measured deviations are the differences between the measured actual values and the mean tolerance value. If no tolerance has been specified, they refer to the nominal dimension.

The unit of measurement of the main program can be seen in the header of the log.

Notes

  • The probing positions are based on the programmed nominal coordinates in the I-CS.
  • See your drawing for the nominal positions.
  • Before defining a cycle, you must program a tool call in order to define the touch-probe axis.
  • The 14xx touch probe cycles support SIMPLE and L-TYPE styli.
  • In order to achieve optimal accuracy results with an L-TYPE stylus, HEIDENHAIN recommends that you perform probing and calibration at the same speed. Note the setting of the feed override if it is active during probing.
  • If the workpiece touch probe does not deflect exactly horizontally or vertically, measuring results may deviate.
  • If you want to use not only the measured rotation, but also a measured position, make sure to probe the surface perpendicularly, if possible. The larger the angular error and the bigger the ball-tip radius, the larger the positioning error. If the angular errors in the initial angular position are too large, corresponding position errors might be the result.
  • If you use the touch probe cycles to correct the offset of a rotary axis, the control adds the values to the current value. Corrections can lead to values outside of the modulo range –360° to +360°. If a rotary axis already has an offset outside of the modulo range, you can reduce the value with PRESET CORR and the entry 0 in the modulo range.

Note regarding machine parameters

  • In the optional machine parameter trackAsync (no. 122503), the machine manufacturer defines whether the control orients the spindle for probing during prepositioning. This can save time during automatic probing procedures. In addition, the control takes the calibrated center offset of L-shaped style into account for the spindle tracking speed. This means that the speed at the ball tip is at most the rapid traverse of the probe FMAX, which increases safety during probing.

Semi-automatic mode

If the probing positions relative to the current datum are unknown, you can execute the cycle in semi-automatic mode. In this mode, you can determine the starting position by manually pre-positioning before performing the probing operation.

For this purpose, precede the value for the required nominal position with "?". You can do this by selecting Name in the action bar. Depending on the object, you need to define the nominal positions that determine the probing direction, see "Examples".

 
Tip

Depending on the object, you need to define the nominal positions that determine the probing direction,

Cycle sequence

Proceed as follows:

  1. Run the cycle
  2. The control interrupts the NC program.
  3. A window opens.
  4. Use the axis-direction keys to position the touch probe to the desired touch point
  5. or

  6. Position the touch probe to the desired point using the electronic handwheel
  7. Change the probing direction in the window, if necessary

  1. Select the NC Start key
  2. The control closes the window and performs the first probing operation.
  3. If CLEAR. HEIGHT MODE Q1125 = 1 or 2, then the control opens a message in the FN 16 tab, Status workspace. This message indicates that the mode for traversing to the clearance height is not possible.
  4. Move the touch probe to a safe position

  1. Select the NC Start key
  2. Cycle or program execution is resumed. You may then need to repeat the entire process for further touch points.
 
Notice
Danger of collision!
The control will ignore the programmed values 1 and 2 for Traverse to clearance height when running in semi-automatic mode. Depending on the position of the touch probe, there is danger of collision.
  1. In semi-automatic mode, manually traverse to a clearance height after every probing operation.
 
Tip

Programming and operating notes:

  • See the drawing for these nominal positions.
  • Semi-automatic mode is only executed in the machine operating modes, not in the simulation.
  • If you did not define a nominal position for a touch point in any direction, the control generates an error message.
  • If you did not define a nominal position for a single direction, the control will capture the actual position after probing the object. This means that the measured actual position will subsequently be applied as the nominal position. Consequentially, there is no deviation for this position and thus no position compensation.

Examples

Important: Specify the nominal positions from the drawing!

In the following three examples, the nominal positions from this drawing will be used.

Alignment using two holes

In this example, you will align two holes. Probing is done in the X axis (main axis) and in the Y axis (secondary axis). This means that it is mandatory to define the nominal position from the drawing for these axes! A nominal position for the Z axis (tool axis) is not necessary as you will not measure in this direction.

  • QS1100 = Nominal Position 1 of the main axis is provided, but the workpiece position is not known
  • QS1101 = Nominal Position 1 of the secondary axis is provided, but the workpiece position is not known
  • QS1102 = Nominal Position 1 in tool axis is unknown
  • QS1103 = Nominal Position 2 of the main axis is provided, but the workpiece position is not known
  • QS1104 = Nominal Position 2 of the secondary axis is provided, but the workpiece position is not known
  • QS1105 = Nominal Position 2 in tool axis is unknown

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.

11 TCH PROBE 1411 PROBING TWO CIRCLES ~

QS1100= "?30"

;1ST POINT REF AXIS ~

QS1101= "?50"

;1ST POINT MINOR AXIS ~

QS1102= "?"

;1ST POINT TOOL AXIS ~

Q1116=+10

;Diameter 1 ~

QS1103= "?75"

;2ND POINT REF AXIS ~

QS1104= "?50"

;2ND POINT MINOR AXIS ~

QS1105= "?"

;2ND POINT TOOL AXIS ~

Q1117=+10

;DIAMETER 2 ~

Q1115=+0

;GEOMETRY TYPE ~

Q423=+4

;NO. OF PROBE POINTS ~

Q325=+0

;STARTING ANGLE ~

Q1119=+360

;ANGULAR LENGTH ~

Q320=+2

;SET-UP CLEARANCE ~

Q260=+100

;CLEARANCE HEIGHT ~

Q1125=+2

;CLEAR. HEIGHT MODE ~

Q309=+0

;ERROR REACTION ~

Q1126=+0

;ALIGN ROTARY AXIS ~

Q1120=+0

;TRANSFER POSITION ~

Q1121=+0

;CONFIRM ROTATION

Alignment through an edge

In this example, you will align an edge. Probing is done in the Y axis (secondary axis). This means that it is mandatory to define the nominal position from the drawing for these axes! Nominal positions for the X axis (main axis) and for the Z axis (tool axis) are not required because you will not measure in these directions.

  • QS1100 = Nominal Position 1 in main axis is unknown
  • QS1101 = Nominal Position 1 of the secondary axis is provided, but the workpiece position is not known
  • QS1102 = Nominal Position 1 in tool axis is unknown
  • QS1103 = Nominal Position 2 in main axis is unknown
  • QS1104 = Nominal Position 2 of the secondary axis is provided, but the workpiece position is not known
  • QS1105 = Nominal Position 2 in tool axis is unknown

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.

11 TCH PROBE 1410 PROBING ON EDGE ~

QS1100= "?"

;1ST POINT REF AXIS ~

QS1101= "?0"

;1ST POINT MINOR AXIS ~

QS1102= "?"

;1ST POINT TOOL AXIS ~

QS1103= "?"

;2ND POINT REF AXIS ~

QS1104= "?0"

;2ND POINT MINOR AXIS ~

QS1105= "?"

;2ND POINT TOOL AXIS ~

Q372=+2

;PROBING DIRECTION ~

Q320=+0

;SET-UP CLEARANCE ~

Q260=+100

;CLEARANCE HEIGHT ~

Q1125=+2

;CLEAR. HEIGHT MODE ~

Q309=+0

;ERROR REACTION ~

Q1126=+0

;ALIGN ROTARY AXIS ~

Q1120=+0

;TRANSFER POSITION ~

Q1121=+0

;CONFIRM ROTATION

Alignment via the plane

In this example, you will align a plane. In this case, it is mandatory to define all three nominal positions from the drawing. For angle calculations, it is important that all three axes are taken into account when probing.

  • QS1100 = Nominal Position 1 of the main axis is provided, but the workpiece position is not known
  • QS1101 = Nominal Position 1 of the secondary axis is provided, but the workpiece position is not known
  • QS1102 = Nominal Position 1 of the tool axis is provided, but the workpiece position is not known
  • QS1103 = Nominal Position 2 of the main axis is provided, but the workpiece position is not known
  • QS1104 = Nominal Position 2 of the secondary axis is provided, but the workpiece position is not known
  • QS1105 = Nominal Position 2 of the tool axis is provided, but the workpiece position is not known
  • QS1106 = Nominal Position 3 of the main axis is provided, but the workpiece position is not known
  • QS1107 = Nominal Position 3 of the secondary axis is provided, but the workpiece position is not known
  • QS1108 = Nominal Position 3 of the tool axis is provided, but the workpiece position is not known

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.

11 TCH PROBE 1420 PROBING IN PLANE ~

QS1100= "?50"

;1ST POINT REF AXIS ~

QS1101= "?10"

;1ST POINT MINOR AXIS ~

QS1102= "?0"

;1ST POINT TOOL AXIS ~

QS1103= "?80"

;2ND POINT REF AXIS ~

QS1104= "?50"

;2ND POINT MINOR AXIS ~

QS1105= "?0"

;2ND POINT TOOL AXIS ~

QS1106= "?20"

;3RD POINT REF AXIS ~

QS1107= "?80"

;3RD POINT MINOR AXIS ~

QS1108= "?0"

;3RD POINT TOOL AXIS ~

Q372=-3

;PROBING DIRECTION ~

Q320=+2

;SET-UP CLEARANCE ~

Q260=+100

;CLEARANCE HEIGHT ~

Q1125=+2

;CLEAR. HEIGHT MODE ~

Q309=+0

;ERROR REACTION ~

Q1126=+0

;ALIGN ROTARY AXIS ~

Q1120=+0

;TRANSFER POSITION ~

Q1121=+0

;CONFIRM ROTATION

Evaluation of tolerances

Cycles 14xx also allow you to check tolerance bands. This includes the checking of the position and size of an object.

You can define the following tolerances:

Tolerance

Example

DIN EN ISO 286-2

10H7

ISO 2768-1

10m

Nominal dimension

10+0.01-0.015

You can enter nominal dimensions with the following tolerances:

Combination

Example

Manufacturing dimension

x+-y

10+-0.5

10.0

x-+y

10-+0.5

10.0

x-y+z

10-0.1+0.5

10.2

x+y-z

10+0.1-0.5

9.8

x+y+z

10+0.1+0.5

10.3

x-y-z

10-0.1-0.5

9.7

x+y

10+0.5

10.25

x-y

10-0.5

9.75

If you program a tolerance entry, the control will monitor the tolerance band. The control writes the following statuses to the return parameter Q183: Pass, rework, or scrap. If a compensation of the preset is programmed, the control corrects the active preset after probing

The following cycle parameters allow input values with tolerances:

  • Q1100 1ST POINT REF AXIS
  • Q1101 1ST POINT MINOR AXIS
  • Q1102 1ST POINT TOOL AXIS
  • Q1103 2ND POINT REF AXIS
  • Q1104 2ND POINT MINOR AXIS
  • Q1105 2ND POINT TOOL AXIS
  • Q1106 3RD POINT REF AXIS
  • Q1107 3RD POINT MINOR AXIS
  • Q1108 3RD POINT TOOL AXIS
  • Q1116 DIAMETER 1
  • Q1117 DIAMETER 2

Program this as follows:

  1. Start the cycle definition
  2. Enable the Name selection option in the action bar
  3. Program nominal position/dimension incl. tolerance
  4. In the cycle, QS1116="+8-2-1" is defined, for example.
 
Tip
  • If you program a tolerance that does not comply with the DIN standard or if you indicate tolerances incorrectly when programming nominal dimensions (e.g., by entering blanks), the control aborts execution and displays an error message.
  • Ensure correct upper and lower case when entering the DIN EN ISO and DIN ISO tolerances. Entering space characters is not allowed.

Cycle sequence

If the actual position is outside the tolerance, the control behaves as follows:

  • Q309 = 0: The control does not interrupt program run.
  • Q309 = 1: In the case of scrap or rework, the control interrupts program run with a message.
  • Q309 = 2: In the case of scrap, the control interrupts program run with a message.

If Q309 = 1 or 2, proceed as follows:

  1. A window appears. The control displays all of the nominal and actual dimensions of the object.
  2. Press the CANCEL button to interrupt the NC program

  1. or

  2. Press NC Start to resume NC program run
 
Tip

Please note that the deviations returned by the touch probe cycles are based on the mean tolerance in Q98x and Q99x. If Q1120 and Q1121 are defined, then the values are equivalent to the values used for the compensation. If no automatic evaluation is active, then the control saves the values (based on the mean tolerance) in the intended Q parameter, allowing you to process these values.

Example

  • QS1116 = diameter 1, tolerance specified
  • QS1117 = diameter 2, tolerance specified

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.

11 TCH PROBE 1411 PROBING TWO CIRCLES ~

Q1100=+30

;1ST POINT REF AXIS ~

Q1101=+50

;1ST POINT MINOR AXIS ~

Q1102=-5

;1ST POINT TOOL AXIS ~

QS1116="+8-2-1"

;DIAMETER 1 ~

Q1103=+75

;2ND POINT REF AXIS ~

Q1104=+50

;2ND POINT MINOR AXIS ~

QS1105=-5

;2ND POINT TOOL AXIS ~

QS1117="+8-2-1"

;DIAMETER 2 ~

Q1115=+0

;GEOMETRY TYPE ~

Q423=+4

;NO. OF PROBE POINTS ~

Q325=+0

;STARTING ANGLE ~

Q1119=+360

;ANGULAR LENGTH ~

Q320=+2

;SET-UP CLEARANCE ~

Q260=+100

;CLEARANCE HEIGHT ~

Q1125=+2

;CLEAR. HEIGHT MODE ~

Q309=2

;ERROR REACTION ~

Q1126=+0

;ALIGN ROTARY AXIS ~

Q1120=+0

;TRANSFER POSITION ~

Q1121=+0

;CONFIRM ROTATION

Transferring the actual position

You can determine the actual position in advance and define it as the actual position for the touch probe cycle. Then, both the nominal position and the actual position will be transferred to the object. Based on the difference, the cycle calculates the required compensation values and applies tolerance monitoring.

Program this as follows:

  1. Define the cycle
  2. Enable the Name selection option in the action bar
  3. Program the nominal position with tolerance monitoring as needed
  4. Program "@"
  5. Program actual position
  6. In the cycle, QS1100="10+0.02@10.0123" is defined, for example.
 
Tip

Programming and operating notes:

  • If you program @, no probing will be carried out. The control only accounts for the actual and nominal positions.
  • You must define the actual position for all three axes: main axis, secondary axis, and tool axis. If you define only one axis with its actual position, an error message will be generated.
  • Actual positions can also be defined with Q Q1900-Q1999

Example

This feature allows you to do the following:

  • Determine a circular pattern based on multiple different objects
  • Align a gear based on its center and the position of a tooth

The nominal positions are defined here with tolerance monitoring and actual position.

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.

5 TCH PROBE 1410 PROBING ON EDGE ~

QS1100="10+0.02@10.0123"

;1ST POINT REF AXIS ~

QS1101="50@50.0321"

;1ST POINT MINOR AXIS ~

QS1102="-10-0.2+0.2@Q1900"

;1ST POINT TOOL AXIS ~

QS1103="30+0.02@30.0134"

;2ND POINT REF AXIS ~

QS1104="50@50.534"

;2ND POINT MINOR AXIS ~

QS1105="-10-0.02@Q1901"

;2ND POINT TOOL AXIS ~

Q372=+2

;PROBING DIRECTION ~

Q320=+0

;SET-UP CLEARANCE ~

Q260=+100

;CLEARANCE HEIGHT ~

Q1125=+2

;CLEAR. HEIGHT MODE ~

Q309=+0

;ERROR REACTION ~

Q1126=+0

;ALIGN ROTARY AXIS ~

Q1120=+0

;TRANSFER POSITION ~

Q1121=+0

;CONFIRM ROTATION