Cycle 272 OCM ROUGHING (#167 / #1-02-1)
ISO programming
G272
Application
Requirements
Before programming the call of Cycle 272, you need to program further cycles:
- CONTOUR DEF / SEL CONTOUR or Cycle 14 CONTOUR
- Cycle 271 OCM CONTOUR DATA
Cycle run
- The tool uses positioning logic to move to the starting point
- The control determines the starting point automatically based on the pre-positioning and the programmed contour
- The control moves to the first plunging depth. The plunging depth and the sequence for machining the contours depend on the plunging strategy Q575.
Depending on the definition in Cycle 271 OCM CONTOUR DATA, parameter Q569 OPEN BOUNDARY, the control plunges as follows:
- Q569 = 0 or 2: The tool plunges into the material in a helical or reciprocating movement. The finishing allowance for the side is taken into account.
- Q569 = 1: The tool plunges vertically outside the open boundary to the first plunging depth
- After reaching the first plunging depth, the tool mills the contour in an outward or inward direction (depending on Q569) at the programmed milling feed rate Q207
- In the next step, the tool is moved to the next plunging depth and repeats the roughing procedure until the programmed contour is completely machined
- Finally, the tool retracts in the tool axis to the clearance height
- If there are more contours, the control will repeat the machining process. The control then moves to the contour whose starting point is positioned nearest to the current tool position (depending on the infeed strategy Q575)
- Finally, the tool moves with Q253 F PRE-POSITIONING to Q200 SET-UP CLEARANCE and then at FMAX to Q260 CLEARANCE HEIGHT
Plunging behavior with Q569 = 0 or 2
The control generally tries plunging with a helical path. If this is not possible, it tries plunging with a reciprocation movement.
The plunging behavior depends on:
- Q207 FEED RATE MILLING
- Q568 PLUNGING FACTOR
- Q575 INFEED STRATEGY
- ANGLE
- RCUTS
- Rcorr (tool radius R + tool oversize DR)
Helical:
The helical path is calculated as follows:
At the end of the plunging movement, the tool executes a semi-circular movement to provide sufficient space for the resulting chips.
Reciprocating
The reciprocation movement is calculated as follows:
At the end of the plunging movement, the tool executes a linear movement to provide sufficient space for the resulting chips.
Notes
- Run a simulation to verify the machining sequence and the contour
- Use tools without a corner radius R2 where possible
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- If the plunging depth is larger than LCUTS, it will be limited and the control will display a warning.
- 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.
If required, use a center-cut end mill (ISO 1641).
Notes on programming
- CONTOUR DEF / SEL CONTOUR will reset the tool radius that was used last. If you run this machining cycle with Q438 = –1 after CONTOUR DEF / SEL CONTOUR, the control assumes that no pre-machining has taken place yet.
- If the path overlap factor Q370 < 1, a value of less than 1 is also recommended for the plunging factor Q579 .
- If you have roughed a figure or a contour before, program the number or the name of the rough-out tool in the cycle. If there was no initial roughing, you need to define Q438=0 ROUGH-OUT TOOL in the cycle parameter during the first roughing operation.
Cycle parameters
Help graphic | Parameter |
---|---|
Q202 Plunging depth? Tool infeed per cut. This value has an incremental effect. Input: 0...99999.9999 | |
Q370 Path overlap factor? Q370 x tool radius = lateral infeed k on a straight line. The control maintains this value as precisely as possible. Input: 0.04...1.99 or PREDEF | |
Q207 Feed rate for milling? Traversing speed of the tool in mm/min for milling Input: 0...99999.999 or FAUTO, FU, FZ | |
Q568 Factor for plunging feed rate? Factor by which the control reduces the feed rate Q207 for downfeed into the material. Input: 0.1...1 | |
Q253 Feed rate for pre-positioning? Traversing speed of the tool in mm/min for approaching the starting position. This feed rate will be used below the coordinate surface, but outside the defined material. Input: 0...99999.9999 or FMAX, FAUTO, PREDEF | |
Q200 Set-up clearance? Distance between lower edge of tool and workpiece surface. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
Q438 or QS438 Number/name of rough-out tool? Number or name of the tool that was used by the control to rough out the contour pocket. You are able to transfer the coarse roughing tool directly from the tool table via the action bar. In addition, you can enter the tool name via the Name in the action bar. The control automatically inserts the closing quotation mark when you exit the input field. -1: The control assumes that the tool last used in Cycle 272 is the rough-out tool (default behavior) 0: If there was no coarse-roughing, enter the number of a tool with the radius 0. This is usually the tool numbered 0. Input: –1...+32767.9 or max. 255 characters | |
Q577 Factor for appr./dept. radius? Factor by which the approach or departure radius will be multiplied. Q577 is multiplied by the tool radius. This results in an approach and departure radius. Input: 0.15...0.99 | |
Q351 Direction? Climb=+1, Up-cut=-1 Type of milling operation. The direction of spindle rotation is taken into account. +1 = climb milling –1 = up-cut milling PREDEF: The control uses the value of a GLOBAL DEF block (If you enter 0, climb milling is performed) Input: -1, 0, +1 or PREDEF | |
Q576 Spindle speed? (optional) Spindle speed in revolutions per minute (rpm) for the roughing tool. 0: The spindle speed from the TOOL CALL block will be used > 0: If a value greater than zero is entered, then this spindle speed will be used Input: 0...99999 | |
Q579 Factor for plunging speed? (optional) Factor by which the control reduces the SPINDLE SPEED Q576 for downfeed into the material. Input: 0.2...1.5 | |
Q575 Infeed strategy (0/1)? (optional) Type of downfeed: 0: The control machines the contour from top to bottom 1: The control machines the contour from bottom to top. The control does not always start with the deepest contour. The machining sequence is automatically calculated by the control. The total plunging path is often shorter than with strategy 2. 2: The control machines the contour from bottom to top. The control does not always start with the deepest contour. This strategy calculates the machining sequence such that the maximum length of the cutting edge is used. The resulting total plunging path is thus often larger than with strategy 1. Depending on Q568, this may also result in a shorter machining time. Input: 0, 1, 2 Tip The total plunging path is the sum of all plunging movements. |
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 272 OCM ROUGHING ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|