Cycle 205 UNIVERSAL PECKING
ISO programming
G205
Application
With this cycle, you can drill holes with decreasing infeed. The cycle may be executed with or without chip breaking. When the plunging depth is reached the cycle performs chip removal. If there is already a pilot hole then you can enter a deepened starting point. In this cycle, you can optionally define a dwell time at the bottom of the hole. This dwell time is used for chip breaking at the bottom of the hole.
Related topics
- Cycle 200 DRILLING for simple holes
- Cycle 203 UNIVERSAL DRILLING optionally with decreasing infeed, dwell time and chip breaking
- Cycle 241 SINGLE-LIP D.H.DRLNG optionally with recessed starting point, dwell depth, direction of rotation and speed when entering and leaving the hole
Cycle run
- The control positions the tool in the tool axis at FMAX to the entered SET-UP CLEARANCE Q200 above the SURFACE COORDINATE Q203.
- If you program a recessed starting point in Q379, the control moves at the positioning feed rate Q253 F PRE-POSITIONING to the set-up clearance above the recessed starting point.
- The tool drills at the programmed Q206 FEED RATE FOR PLNGNG to the plunging depth.
- If you have programmed chip breaking, the control retracts the tool by the retraction value Q256.
- Upon reaching the plunging depth, the control retracts the tool in the tool axis at the retraction feed rate Q208 to the set-up clearance. The set-up clearance is above the SURFACE COORDINATE Q203.
- The tool then moves at Q373 FEED AFTER REMOVAL to the entered advanced stop distance above the plunging depth last reached.
- The tool drills at the feed in Q206 to the next plunging depth. If a decrement Q212 is defined, the plunging depth is decreased after each infeed by the decrement.
- The control repeats this procedure (steps 2 to 7) until the total drilling depth is reached.
- If you entered a dwell time, the tool remains at the hole bottom for chip breaking. The control then retracts the tool at the retraction feed rate to the set-up clearance or the 2nd set-up clearance. The 2nd set-up clearance Q204 will only come into effect if its value is greater than the set-up clearance Q200.
After chip removal, the depth of the next chip breaking is referenced to the last plunging depth.
Example:
- Q202 PLUNGING DEPTH = 10 mm
- Q257 DEPTH FOR CHIP BRKNG = 4 mm
The control performs chip breaking at 4 mm and 8 mm. Chip removal is performed at 10 mm. Chip breaking is next performed at 14 mm and 18 mm, etc.
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 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.
This cycle is not suitable for overlong drills. For overlong drills, use Cycle 241 SINGLE-LIP D.H.DRLNG.
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.
- If you enter advance stop distances Q258 not equal to Q259, the control will change the advance stop distances between the first and last plunging depths at the same rate.
- If you use Q379 to enter a deepened starting point, the control will change the starting point of the infeed movement. Retraction movements are not changed by the control; they are always calculated with respect to the coordinate of the workpiece surface.
- If Q257 DEPTH FOR CHIP BRKNG is greater than Q202 PLUNGING DEPTH, the operation is executed without chip breaking.
Cycle parameters
Help graphic | Parameter |
---|---|
Q200 Set-up clearance? Distance between tool tip and workpiece surface. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
Q201 Depth? Distance between workpiece surface and bottom of hole (depends on parameter Q395 DEPTH REFERENCE). 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 | |
Q202 Plunging depth? Tool infeed per cut. This value has an incremental effect. The depth does not have to be a multiple of the plunging depth. The control will go to depth in one movement if:
Input: 0...99999.9999 | |
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 | |
Q212 Decrement? Value by which the control decreases the plunging depth Q202. 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 | |
Q258 Upper advanced stop distance? Safety clearance above the last plunging depth to which the tool returns at Q373 FEED AFTER REMOVAL after first chip removal. This value has an incremental effect. Input: 0...99999.9999 | |
Q259 Lower advanced stop distance? Safety clearance above the last plunging depth to which the tool returns at Q373 FEED AFTER REMOVAL after the last chip removal. This value has an incremental effect. Input: 0...99999.9999 | |
Q257 Infeed depth for chip breaking? Incremental depth at which the control performs chip breaking. This procedure is repeated until DEPTH Q201 is reached. If Q257 equals 0, the control will not perform chip breaking. This value has an incremental effect. Input: 0...99999.9999 | |
Q256 Retract dist. for chip breaking? Value by which the control retracts the tool during chip breaking. This value has an incremental effect. Input: 0...99999.999 or PREDEF | |
Q211 Dwell time at the depth? Time in seconds that the tool remains at the hole bottom. Input: 0...3600.0000 or PREDEF | |
Q379 Deepened starting point? (optional) 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? (optional) Defines the tool traversing speed when positioning from Q200 SET-UP CLEARANCE to Q379 STARTING POINT (not equal to 0). Input in mm/min. Input: 0...99999.9999 or FMAX, FAUTO, PREDEF | |
Q208 Feed rate for retraction? (optional) Traversing speed of the tool in mm/min when retracting after the machining operation. If you enter Q208 = 0, the control retracts the tool at the feed rate specified in Q206. Input: 0...99999.9999 or FMAX, FAUTO, PREDEF | |
Q395 Diameter as reference (0/1)? (optional) Select whether the entered depth is referenced to the tool tip or the cylindrical part of the tool. If the control is to reference the depth to the cylindrical part of the tool, the point angle of the tool must be defined in the T-ANGLE column of the tool table TOOL.T. 0 = Depth referenced to tool tip 1 = Depth referenced to the cylindrical part of the tool Input: 0, 1 | |
Q373 Post-chip-removal approach feed? (optional) Traversing speed of the tool when approaching the advanced stop distance after chip removal. 0: Move at FMAX >0: Feed in mm/min Input: 0...99999 or FAUTO, FMAX, FU, FZ |
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 205 UNIVERSAL PECKING ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
7 CYCL CALL |
Chip removal and chip breaking
Chip removal
Chip removal depends on cycle parameter Q202 PLUNGING DEPTH.
When the value entered in cycle parameter Q202 is reached, the control performs chip removal. This means that the control always moves the tool to the retraction height, irrespective of the deepened starting point Q379. This height is calculated from Q200 SET-UP CLEARANCE + Q203 SURFACE COORDINATE
Example:
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 205 MM | |||
1 BLK FORM 0.1 Z X+0 Y+0 Z-20 | |||
2 BLK FORM 0.2 X+100 Y+100 Z+0 | |||
3 TOOL CALL 203 Z S4500 | ; Tool call (tool radius 3) | ||
4 L Z+250 R0 FMAX | ; Retract the tool | ||
5 CYCL DEF 205 UNIVERSAL PECKING ~ | |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
6 L X+30 Y+30 R0 FMAX M3 | ; Approach drilling position, spindle ON | ||
7 CYCL CALL | ; Cycle call | ||
8 L Z+250 R0 FMAX | ; Retract the tool | ||
9 M30 | ; End of program run | ||
10 END PGM 205 MM |
Chip breaking
Chip breaking depends on cycle parameter Q257 DEPTH FOR CHIP BRKNG.
When the value entered in cycle parameter Q257 is reached, the control performs chip breaking. This means that the control retracts the tool by the value defined in Q256 DIST FOR CHIP BRKNG. Chip removal starts once the tool reaches the PLUNGING DEPTH. The entire process is repeated until Q201 DEPTH is reached.
Example:
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 205 MM | |||
1 BLK FORM 0.1 Z X+0 Y+0 Z-20 | |||
2 BLK FORM 0.2 X+100 Y+100 Z+0 | |||
3 TOOL CALL 203 Z S4500 | ; Tool call (tool radius 3) | ||
4 L Z+250 R0 FMAX | ; Retract the tool | ||
5 CYCL DEF 205 UNIVERSAL PECKING ~ | |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
6 L X+30 Y+30 R0 FMAX M3 | ; Approach drilling position, spindle ON | ||
7 CYCL CALL | ; Cycle call | ||
8 L Z+250 R0 FMAX | ; Retract the tool | ||
9 M30 | ; End of program run | ||
10 END PGM 205 MM |