Cycle 224 DATAMATRIX CODE PATTERN

ISO programming

G224

Application

Use Cycle 224 DATAMATRIX CODE PATTERN to convert text to a so-called DataMatrix code. This code will be used as a point pattern for a previously defined fixed cycle.

Cycle sequence

cyc224
  1. The control automatically moves the tool from its current position to the programmed starting point. This point is always located in the lower left corner.
  2. Sequence:

    • Move to 2nd set-up clearance (spindle axis)
    • Approach the starting point in the working plane
    • Move to SET-UP CLEARANCE above the workpiece surface (spindle axis)
  3. Then, the control moves the tool in the positive direction of the secondary axis to the first point 1 in the first row
  4. From this position, the control executes the last defined fixed machining cycle
  5. Then, the control moves the tool in the positive direction of the principal axis to point 2 for the next operation.
  6. This procedure will be repeated until all machining operations in the first row have been completed. The tool is located above the last point 3 of the first row
  7. Then, the control moves the tool in the negative direction of the principal and secondary axes to the first point 4 of the next row
  8. Then, the next points are machined
  9. These steps are repeated until the entire DataMatrix code has been completed. Machining stops in the lower right corner 5
  10. Finally, the control retracts the tool to the programmed 2nd set-up clearance

Notes

 
Notice
Danger of collision!
If you combine Cycle 224 with one of the machining cycles, the Safety clearance, coordinate surface and 2nd set-up clearance that you defined in Cycle 224 will be effective for the selected machining cycle. There is a danger of collision!
  1. Check the machining sequence using a graphic simulation
  2. Carefully test the NC program or program section in SINGLE BLOCK mode of Program run operating mode.
  • This cycle can only be executed in the FUNCTION MODE MILL machining mode.
  • Cycle 224 is DEF-active. In addition, Cycle 224 automatically calls the last defined machining cycle.
  • The control uses the special character % for special functions. If you want to use this character in a DataMatrix code, enter it twice in the text (e.g., %%).

Cycle parameters

Help graphic

Parameter

cyc224_1

Q225 Starting point in 1st axis?

Coordinate in the lower left corner of the code in the main axis. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q226 Starting point in 2nd axis?

Coordinate in the bottom left corner of the data matrix code in the secondary axis. This value has an absolute effect.

Input: –99999.9999...+99999.9999

QS501 Text input?

Enter the text to be converted within quotation marks. Variables can be assigned.

Outputting variable texts in DataMatrix codes

Input: Max. 255 characters

Q458 Cell size/Pattern size(1/2)?

Specify how the DataMatrix code is described in Q459:

1: Distance between cells

2: Pattern size

Input: 1, 2

cyc224_2

cyc224_3

Q459 Size for pattern?

Definition of the distance between cells or the pattern size:

If Q458=1: Distance between the first and second cell (between cell centers)

If Q458=2: Distance between the first and last cell (between cell centers)

This value has an incremental effect.

Input: 0...99999.9999

Q224 Angle of rotation?

Angle by which the entire pattern is rotated. The center of rotation lies in the starting point. This value has an absolute effect.

Input: –360.000...+360.000

Q200 Set-up clearance?

Distance between tool tip and workpiece surface. This value has an incremental effect.

Input: 0...99999.9999 or PREDEF

Q203 Workpiece surface coordinate?

Coordinate on the workpiece surface referenced to the active datum. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q204 2nd set-up clearance?

Distance in the tool axis between tool and workpiece (fixtures) at which no collision can occur. This value has an incremental effect.

Input: 0...99999.9999 or PREDEF

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 CYCL DEF 224 DATAMATRIX CODE PATTERN ~

Q225=+0

;STARTNG PNT 1ST AXIS ~

Q226=+0

;STARTNG PNT 2ND AXIS ~

QS501=""

;TEXT ~

Q458=+1

;SIZE SELECTION ~

Q459=+1

;SIZE ~

Q224=+0

;ANGLE OF ROTATION ~

Q200=+2

;SET-UP CLEARANCE ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+50

;2ND SET-UP CLEARANCE

12 CYCL CALL

Outputting variable texts in DataMatrix codes

In addition to specified characters you can also output certain variables in DataMatrix codes. Precede the variable with %.

You can use the following variable texts in Cycle 224 DATAMATRIX CODE PATTERN:

  • Date and time
  • Names and paths of NC programs
  • Count values

Date and time

You can convert the current date, the current time, or the current calendar week into a DataMatrix code. Enter the value %time<x> in cycle parameter QS501. <x> defines the format (e.g., 08 for DD.MM.YYYY.)

 
Tip

Keep in mind that you must enter a leading 0 when entering the date formats 1 to 9 (e.g., %time08).

The following formats are available:

Input

Format

%time00

DD.MM.YYYY hh:mm:ss

%time01

D.MM.YYYY h:mm:ss

%time02

D.MM.YYYY h:mm

%time03

D.MM.YY h:mm

%time04

YYYY-MM-DD hh:mm:ss

%time05

YYYY-MM-DD hh:mm

%time06

YYYY-MM-DD h:mm

%time07

YY-MM-DD h:mm

%time08

DD.MM.YYYY

%time09

D.MM.YYYY

%time10

D.MM.YY

%time11

YYYY-MM-DD

%time12

YY-MM-DD

%time13

hh:mm:ss

%time14

h:mm:ss

%time15

h:mm

%time99

Calendar week

Names and paths of NC programs

You can convert the name or path of the active or called NC program into a DataMatrix code. Enter the value %main<x> or %prog<x> in cycle parameter QS501.

The following formats are available:

Input

Meaning

Example

%main0

Full path of the active NC program

TNC:\MILL.h

%main1

Directory path of the active NC program

TNC:\

%main2

Name of the active NC program

MILL

%main3

File type of the active NC program

.H

%prog0

Full path of the called NC program

TNC:\HOUSE.h

%prog1

Directory path of the called NC program

TNC:\

%prog2

Name of the called NC program

HOUSE

%prog3

File type of the called NC program

.H

Count values

You can convert the current count value into a DataMatrix code. The control displays the current count value in Program Run on thePGM tab of the Status workspace.

Enter the value %count<x> in cycle parameter QS501.

The number after %count indicates how many digits the DataMatrix code contains. The maximum is nine digits.

  • Example:
  • Programming: %count9
  • Current count value: 3
  • Result: 000000003
  • Operating information
  • In the Simulation, the control only simulates the count value you define directly in the NC program. The count value from the Status workspace in the Program Run operating mode is ignored.