ISO programming
G272
G272
Use Cycle 272 OCM ROUGHING to define the technology data for roughing.
In addition, you can use the OCM cutting data calculator. The calculated cutting data help to achieve high material removal rates and therefore increase the productivity.
Positioning logic in OCM cycles
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.
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.
If required, use a center-cut end mill (ISO 1641).
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? 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? 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)? 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.
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 ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|