Fundamentals of touch probe cycles 0, 1 and 420 to 431

Recording the results of measurement

For all cycles in which you automatically measure workpieces (with the exception of Cycles 0 and 1), you can have the control record the measurement results in a log. In the respective touch probe cycle you can define if the control is to

  • Create no measuring log
  • Save the measuring log to a file
  • Interrupt program run and display the measuring log on the screen

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

 
Tip

Use the HEIDENHAIN data transfer software TNCremo if you wish to output the measuring log over the data interface.

Outputting a measuring log to the screen:

If you execute Cycles 42x and 43x in combination with Cycle 441 FAST PROBING and want to output a measuring log to the screen, you must program parameter Q400=1 in Cycle 441. Otherwise the control will not interrupt and the measuring log will not be displayed on the screen.

Saving the measuring log:

If you want to save the measuring log to a file, the control by default saves the data as an ASCII file. The control will save the file in the directory that also contains the associated NC program.

Example

Log file for touch probe cycle 421:

Measuring log for touch probe cycle 421 Hole measuring

Date: 30-06-2005

Time: 6:55:04

Measuring program: TNC:\GEH35712\CHECK1.H

Type of dimension (0 = MM / 1 = INCH): 0

Nominal values:

Center in reference axis:

50.0000

Center in minor axis:

65.0000

Diameter:

12.0000

Given limit values:

Maximum limit for center in reference axis:

50.1000

Minimum limit for center in reference axis:

49.9000

Maximum limit for center in minor axis:

65.1000

Minimum limit for center in minor axis:

64.9000

Maximum dimension for hole:

12.0450

Minimum dimension for hole:

12.0000

Actual values:

Center in reference axis:

50.0810

Center in minor axis:

64.9530

Diameter:

12.0259

Deviations:

Center in reference axis:

0.0810

Center in minor axis:

-0.0470

Diameter:

0.0259

Further measuring results: Measuring height:

-5.0000

End of measuring log

Measurement results in Q parameters

The control saves the measurement results of the respective touch probe cycle in the globally effective Q parameters Q150 to Q160. Deviations from the nominal values are saved in parameters Q161 to Q166. Note the table of result parameters listed with every cycle description.

During cycle definition, the control also shows the result parameters for the respective cycle in a help graphic . The highlighted result parameter belongs to that input parameter.

Classification of results

For some cycles you can inquire the status of measuring results through the globally effective Q parameters Q180 to Q182.

Parameter value

Measuring status

Q180 = 1

Measurement results are within tolerance

Q181 = 1

Rework is required

Q182 = 1

Scrap

The control sets the rework or scrap marker as soon as one of the measuring values is out of tolerance. To determine which of the measuring results is out of tolerance, check the measuring log, or compare the respective measuring results (Q150 to Q160) with their limit values.

In Cycle 427 the control assumes by default that you are measuring an outside dimension (stud). However, you can correct the status of the measurement by entering the correct maximum and minimum dimension together with the probing direction.

 
Tip

The control also sets the status markers if you have not defined any tolerance values or maximum/minimum dimensions.

Tolerance monitoring

With most cycles for workpiece inspection, you can have the control perform tolerance monitoring. This requires that you define the necessary limit values during cycle definition. If you do not wish to monitor for tolerances, simply leave the default value 0 for this parameter set this parameter unchanged.

Tool monitoring

With some cycles for workpiece inspection, you can have the control perform tool monitoring. The control then monitors whether

  • the tool radius should be compensated for due to the deviations from the nominal value (values in Q16x)
  • the deviations from the nominal value (values in Q16x) are greater than the tool breakage tolerance.

Tool compensation

Requirements:

  • Active tool table
  • Tool monitoring must be switched on in the cycle: Set Q330 unequal to 0 or enter a tool name. Select the tool name input via Name in the action bar.
 
Tip
  • HEIDENHAIN recommends using this function only if the tool to be compensated for is the one that was used to machine the contour as well as if any necessary reworking will also be done with this tool.
  • If you perform several compensation measurements, the control adds the respective measured deviation to the value stored in the tool table.

Milling cutter

If you reference a milling cutter in parameter Q330, the appropriate values will be compensates for as follows:

The control always compensates for the tool radius in the DR column of the tool table, even if the measured deviation lies within the given tolerance.

You can inquire whether re-working is necessary via parameter Q181 in the NC program (Q181=1: rework required).

Turning tool

Only applies to Cycles 421, 422, 427.

If you reference a turning tool in parameter Q330, the appropriate values in row DZL and DXL, respectively, will be corrected. The control also monitors the breakage tolerance, which is defined in column LBREAK.

You can poll whether re-working is necessary via parameter Q181 in the NC program (Q181=1: rework required).

Compensating for an indexed tool

If you want to automatically correct the values for an indexed tool with a tool name, program the following:

  • QS0 = "TOOL NAME"
  • FN 18: SYSREAD Q0 = ID990 NR10 IDX0; specify the number of the QS parameter in IDX
  • Q0= Q0 +0.2; add the index of the basic tool number
  • In the cycle: Q330 = Q0; use the indexed tool number

Tool breakage monitoring

Requirements:

  • Active tool table
  • Tool monitoring must be switched on in the cycle (set Q330 unequal to 0)
  • RBREAK must be greater than 0 (in the entered tool number in the table)
  • Tool parameters

The control will output an error message and stop the program run if the measured deviation is greater than the breakage tolerance of the tool. At the same time, the tool will be deactivated in the tool table (column TL = L).

Reference system for measurement results

The control transfers all measurement results, which reference the active coordinate system, or as the case may be, the shifted or/and rotated/tilted coordinate system, to the result parameters and the log file.