Cycle 241 SINGLE-LIP D.H.DRLNG enables you to machine holes using a single-lip deep hole drill. It is possible to enter a deepened starting point. You can define the direction of rotation and the rotational speed for moving into and retracting from the hole.
Application
Cycle sequence
- The control positions the tool in the spindle axis at rapid traverse FMAX to the entered Safety clearance Q200 above the workpiece SURFACE COORDINATE Q203
- Depending on the Position behavior when working with Q379, the control will either switch on the spindle with the programmed speed at the Safety clearance Q200 or at a certain distance above the coordinate surface
- The control executes the approach motion depending on the direction of rotation defined in the cycle with a spindle that rotates clockwise, counterclockwise, or is stationary
- The tool drills to the hole depth at the feed rate F, or to the maximum plunging depth if a smaller infeed value has been entered. The plunging depth is decreased after each infeed by the decrement. If you have entered a dwell depth, the control reduces the feed rate by the feed rate factor after the dwell depth has been reached
- If programmed, the tool remains at the hole bottom for chip breaking.
- The control repeats this procedure (steps 4 to 5) until the total hole depth is reached
- After the control has reached this position, it will automatically switch off the coolant and set the speed to the value defined in Q427 ROT.SPEED INFEED/OUT
- The control positions the tool to the retract position at the retraction feed rate. To find out the retract position value in your particular case, please refer to: Position behavior when working with Q379
- If programmed, the tool moves to 2nd set-up clearance at FMAX
Notes
- Enter depth as negative
- 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 only be executed 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. The 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: 0...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. 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 the DEPTH Q201. "...": Path of a user macro that is to be executed instead of an M function. All instructions in the user macro are executed automatically. Input: 0...999 | |
Q435 Dwell depth? 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 %? Factor by which the control reduces the feed rate after reaching Q435 DWELL DEPTH. Input: 0.0001...100 | |
Q202 Maximum plunging depth? 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? Value by which the control decreases Q202 Feed depth after each infeed. This value has an incremental effect. Input: 0...99999.9999 | |
Q205 Minimum plunging depth? 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.
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 CYCL DEF 241 SINGLE-LIP D.H.DRLNG ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 CYCL CALL |
User macro
The user macro is another NC program.
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 an NC program.
Macros work in the same manner as NC programs that are called with the PGM CALL function, for example. You define a macro as an NC program with the file type *.h.
- 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.
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.
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, e.g. 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
- SURFACE COORDINATE Q203 =0
- SET-UP CLEARANCE Q200 =2
- STARTING POINT Q379 =2
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:
The starting point of drilling is calculated as follows: 0.2 x Q379=0.2*2=0.4; the starting point is 0.4 mm or inches above the deepened starting point. So if the deepened starting point is at –2, the control starts the drilling process at –1.6.
The following table shows various examples for calculating the start of drilling:
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
- SURFACE COORDINATE Q203 =0
- SET-UP CLEARANCEQ200 =2
- STARTING POINT Q379 =2
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:
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 deepened start point. So if the deepened 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:
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 |