Cycle 241 SINGLE-LIP D.H.DRLNG

ISO programming

G241

Application

Cycle 241 SINGLE-LIP D.H.DRLNG machines holes with a single-lip deep hole drill. It is possible to enter a recessed starting point. The control performs moving to drilling depth with M3. You can change the direction of rotation and the rotational speed for moving into and retracting from the hole.

Cycle run

  1. The control positions the tool in the spindle axis at rapid traverse FMAX to the entered SET-UP CLEARANCE Q200 above SURFACE COORDINATE Q203.
  2. Depending on the positioning behavior, the control will either switch on the spindle with the programmed speed at SET-UP CLEARANCE Q200 or at a certain distance above the coordinate surface.
  3. Position behavior when working with Q379

  4. The control executes the approach motion depending on the direction of rotation defined in Q426 DIR. OF SPINDLE ROT. with a spindle that rotates clockwise or counterclockwise, or is stationary.
  5. The tool drills with M3 and Q206 FEED RATE FOR PLNGNG to the drilling depth Q201 or dwell depth Q435 or the plunging depth Q202:
    • If you have entered Q435 DWELL DEPTH, the control reduces the feed rate by Q401 FEED RATE FACTOR after the dwell depth has been reached and remains there for Q211 DWELL TIME AT DEPTH.
    • If a smaller infeed value has been entered, the control drills to the plunging depth. With each infeed, the plunging depth is reduced by Q212 DECREMENT.
  6. If programmed, the tool remains at the hole bottom for chip breaking.
  7. After the control has reached this position, it will automatically switch off the coolant, set the speed to the value defined in Q427 ROT.SPEED INFEED/OUT and, if required, change again the direction of rotation defined in Q426.
  8. The control positions the tool to the retract position at Q208 RETRACTION FEED RATE.
  9. Position behavior when working with Q379

  10. If programmed, the tool moves to the 2nd set-up clearance at FMAX.

Notes

 
Notice
Danger of collision!
If you enter the depth in a cycle as a positive value, the control reverses the calculation of the pre-positioning. The tool moves at rapid traverse in the tool axis to set-up the clearance below the workpiece surface! There is a danger of collision!
  1. Enter depth as negative
  2. Use the machine parameter displayDepthErr (no. 201003) to specify whether the control should display an error message (on) or not (off) if a positive depth is entered
  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • This cycle monitors the defined usable length LU of the tool. If the LU value is less than the DEPTH Q201, the control will display an error message.

Notes on programming

  • Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0.
  • The algebraic sign for the DEPTH cycle parameter determines the working direction. If you program DEPTH=0, the cycle will not be executed.

Cycle parameters

Help graphic

Parameter

Q200 Set-up clearance?

Distance between tool tip and Q203 SURFACE COORDINATE. This value has an incremental effect.

Input: 0...99999.9999 or PREDEF

Q201 Depth?

Distance between Q203 SURFACE COORDINATE and bottom of hole. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q206 Feed rate for plunging?

Traversing speed of the tool in mm/min while drilling

Input: 0...99999.999 or FAUTO, FU

Q211 Dwell time at the depth?

Time in seconds that the tool remains at the hole bottom.

Input: 0...3600.0000 or PREDEF

Q203 Workpiece surface coordinate?

Coordinate on the workpiece surface referenced to the active preset. 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

Q379 Deepened starting point?

If there is already a pilot hole then you can define a deepened starting point here. It is incrementally referenced to Q203 SURFACE COORDINATE. The control moves at Q253 F PRE-POSITIONING to above the deepened starting point by the value Q200 SET-UP CLEARANCE. This value has an incremental effect.

Input: 0...99999.9999

Q253 Feed rate for pre-positioning?

Defines the traversing speed of the tool when re-approaching Q201 DEPTH after Q256 DIST FOR CHIP BRKNG. This feed rate is also in effect when the tool is positioned to Q379 STARTING POINT (not equal 0). Input in mm/min.

Input: 0...99999.9999 or FMAX, FAUTO, PREDEF

Q208 Feed rate for retraction?

Traversing speed of the tool in mm/min when retracting from the hole. If you enter Q208=0, the control retracts the tool at Q206 FEED RATE FOR PLNGNG.

Input: 0...99999.999 or FMAX, FAUTO, PREDEF

Q426 Rot. dir. of entry/exit (3/4/5)?

Rotational speed at which the tool is to rotate when moving into and retracting from the hole.

3: Spindle rotation with M3

4: Spindle rotation with M4

5: Movement with stationary spindle

Input: 3, 4, 5

Q427 Spindle speed of entry/exit?

Rotational speed at which the tool is to rotate when moving into and retracting from the hole.

Input: 1...99999

Q428 Spindle speed for drilling?

Desired speed for drilling.

Input: 0...99999

Q429 M function for coolant on?

>=0: Miscellaneous function M for switching on the coolant. The control switches the coolant on when the tool has reached the set-up clearance Q200 above the starting point Q379.

"...": Path of a user macro that is to be executed instead of an M function. All instructions in the user macro are executed automatically.

User macro

Input: 0...999

Q430 M function for coolant off?

>=0: Miscellaneous function M for switching off the coolant. The control switches the coolant off if the tool is at Q201 DEPTH.

"...": Path of a user macro that is to be executed instead of an M function. All instructions in the user macro are executed automatically.

User macro

Input: 0...999

Q435 Dwell depth? (optional)

Coordinate in the spindle axis at which the tool is to dwell. If 0 is entered, the function is not active (default setting). Application: During machining of through-holes some tools require a short dwell time before leaving the bottom of the hole in order to transport the chips to the top. Define a value smaller than Q201 DEPTH. This value has an incremental effect.

Input: 0...99999.9999

Q401 Feed rate factor in %? (optional)

Factor by which the control reduces the feed rate after reaching Q435 DWELL DEPTH.

Input: 0.0001...100

Q202 Maximum plunging depth? (optional)

Infeed per cut. The DEPTH Q201 does not have to be a multiple of Q202. This value has an incremental effect.

Input: 0...99999.9999

Q212 Decrement? (optional)

Value by which the control decreases Q202 PLUNGING DEPTH after each infeed. This value has an incremental effect.

Input: 0...99999.9999

Q205 Minimum plunging depth? (optional)

If Q212 DECREMENT is not 0, the control limits the plunging depth to this value. This means that the plunging depth cannot be less than Q205. This value has an incremental effect.

Input: 0...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 CYCL DEF 241 SINGLE-LIP D.H.DRLNG ~

Q200=+2

;SET-UP CLEARANCE ~

Q201=-20

;DEPTH ~

Q206=+150

;FEED RATE FOR PLNGNG ~

Q211=+0

;DWELL TIME AT DEPTH ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+50

;2ND SET-UP CLEARANCE ~

Q379=+0

;STARTING POINT ~

Q253=+750

;F PRE-POSITIONING ~

Q208=+1000

;RETRACTION FEED RATE ~

Q426=+5

;DIR. OF SPINDLE ROT. ~

Q427=+50

;ROT.SPEED INFEED/OUT ~

Q428=+500

;ROT. SPEED DRILLING ~

Q429=+8

;COOLANT ON ~

Q430=+9

;COOLANT OFF ~

Q435=+0

;DWELL DEPTH ~

Q401=+100

;FEED RATE FACTOR ~

Q202=+99999

;MAX. PLUNGING DEPTH ~

Q212=+0

;DECREMENT ~

Q205=+0

;MIN. PLUNGING DEPTH

12 CYCL CALL

User macro

User macros are separate NC programs.

A user macro contains a sequence of multiple instructions. With a macro, you can define multiple NC functions that the control executes. As a user, you create macros as NC programs.

Macros work in the same manner as NC programs that are called (e.g., with the NC function CALL PGM). Define a macro as an NC program with the file type *.h or *.i.

  • HEIDENHAIN recommends using QL parameters in the macro. QL parameters have only a local effect for an NC program. If you use other types of variables in the macro, then changes may also have an effect on the calling NC program. In order to explicitly cause changes in the calling NC program, use Q or QS parameters with the numbers 1200 to 1399.
  • Within the macro, you can read the value of the cycle parameters.
  • Variables: Q, QL, QR, QS parameters and named parameters

Example of a user macro for coolant

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.

0 BEGIN PGM KM MM

1 FN 18: SYSREAD QL100 = ID20 NR8

; Read the coolant level

2 FN 9: IF QL100 EQU +1 GOTO LBL "Start"

; Query the coolant level; if coolant is active, jump to the Start LBL

3 M8

; Switch coolant on

7 CYCL DEF 9.0 DWELL TIME

8 CYCL DEF 9.1 V.ZEIT3

9 LBL "Start"

10 END PGM RET MM

Position behavior when working with Q379

Especially when working with very long drills (for example, single-lip deep hole drills or overlong twist drills), there are several things to remember. The position at which the spindle is switched on is very important. If the tool is not guided properly, overlong drills might break.

It is therefore advisable to use the STARTING POINT Q379 parameter. This parameter can be used to influence the position at which the control turns on the spindle.

Start of drilling

The STARTING POINT Q379 parameter takes both SURFACE COORDINATE Q203 and the SET-UP CLEARANCE Q200 parameter into account. The following example illustrates the relationship between the parameters and how the starting position is calculated:

STARTING POINT Q379=0

  • The control switches on the spindle at the SET-UP CLEARANCE Q200 above the SURFACE COORDINATE Q203
     

STARTING POINT Q379>0

  • The starting point is at a certain value above the deepened starting point Q379. This value can be calculated as follows: 0.2 x Q379; if the result of this calculation is larger than Q200, the value is always Q200.

  • Example:

  • SURFACE COORDINATE Q203 =0
  • SET-UP CLEARANCE Q200 =2
  • STARTING POINT Q379 =2
  • The starting point of drilling is calculated as follows: 0.2 x Q379=0.2*2=0.4; the starting point of drilling is 0.4 mm or inch above the recessed starting point. So if the recessed starting point is at –2, the control starts the drilling process at –1.6 mm.

  • The following table shows various examples for calculating the start of drilling:

Start of drilling at deepened starting point

Q200

Q379

Q203

Position at which pre-positioning is executed with FMAX

Factor 0.2 * Q379

Start of drilling

2

2

0

2

0.2*2=0.4

-1.6

2

5

0

2

0.2*5=1

-4

2

10

0

2

0.2*10=2

-8

2

25

0

2

0.2*25=5 (Q200=2, 5>2, so the value 2 is used.)

-23

2

100

0

2

0.2*100=20 (Q200=2, 20>2, so the value 2 is used.)

-98

5

2

0

5

0.2*2=0.4

-1.6

5

5

0

5

0.2*5=1

-4

5

10

0

5

0.2*10=2

-8

5

25

0

5

0.2*25=5

-20

5

100

0

5

0.2*100=20 (Q200=5, 20>5, so the value 5 is used.)

-95

20

2

0

20

0.2*2=0.4

-1.6

20

5

0

20

0.2*5=1

-4

20

10

0

20

0.2*10=2

-8

20

25

0

20

0.2*25=5

-20

20

100

0

20

0.2*100=20

-80

Chip removal

The point at which the control removes chips also plays a decisive role for the work with overlong tools. The retraction position during the chip removal process does not have to be at the start position for drilling. A defined position for chip removal can ensure that the drill stays in the guide.

STARTING POINT Q379=0

  • The chips are removed when the tool is positioned at the SET-UP CLEARANCE Q200 above the SURFACE COORDINATE Q203.
     

STARTING POINT Q379>0

  • Chip removal is at a certain value above the deepened starting point Q379. This value can be calculated as follows: 0.8 x Q379; if the result of this calculation is larger than Q200, the value is always Q200.

  • Example:

  • SURFACE COORDINATE Q203 =0
  • SET-UP CLEARANCEQ200 =2
  • STARTING POINT Q379 =2
  • The position for chip removal is calculated as follows: 0.8 x Q379=0.8*2=1.6; the position for chip removal is 1.6 mm or inches above the recessed start point. So if the recessed starting point is at –2, the control starts chip removal at –0.4.

  • The following table shows examples of how the position for chip removal (retraction position) is calculated:

Position for chip removal (retraction position) with deepened starting point

Q200

Q379

Q203

Position at which pre-positioning is executed with FMAX

Factor 0.8 * Q379

Return position

2

2

0

2

0.8*2=1.6

-0.4

2

5

0

2

0.8*5=4

-3

2

10

0

2

0.8*10=8 (Q200=2, 8>2, so the value 2 is used.)

-8

2

25

0

2

0.8*25=20 (Q200=2, 20>2, so the value 2 is used.)

-23

2

100

0

2

0.8*100=80 (Q200=2, 80>2, so the value 2 is used.)

-98

5

2

0

5

0.8*2=1.6

-0.4

5

5

0

5

0.8*5=4

-1

5

10

0

5

0.8*10=8 (Q200=5, 8>5, so the value 5 is used.)

-5

5

25

0

5

0.8*25=20 (Q200=5, 20>5, so the value 5 is used.)

-20

5

100

0

5

0.8*100=80 (Q200=5, 80>5, so the value 5 is used.)

-95

20

2

0

20

0.8*2=1.6

-1.6

20

5

0

20

0.8*5=4

-4

20

10

0

20

0.8*10=8

-8

20

25

0

20

0.8*25=20

-20

20

100

0

20

0.8*100=80 (Q200=20, 80>20, so the value 20 is used.)

-80