Fundamentals

The control provides cycles for frequently used figures. You can program these figures as pockets, islands, or boundaries.

  • These figure cycles offer the following benefits:
  • You can conveniently program the figures and machining data without the need to program an individual path contour.
  • Frequently needed figures can be reused.
  • If you want to program an island or an open pocket, the control provides you with more cycles for defining the figure boundary.
  • The Boundary figure type enables you to face-mill your figure.

With a figure, you can redefine the OCM contour data and cancel the definition of a previously defined Cycle 271 OCM CONTOUR DATA or of a figure boundary.

For defining figures, the control provides the following cycles:

For defining figure boundaries, the control provides the following cycles:

Tolerances

The control allows you to store tolerances in the following cycles and cycle parameters:

Cycle number

Parameter

1271 OCM RECTANGLE

Q218 FIRST SIDE LENGTH,

Q219 2ND SIDE LENGTH

1272 OCM CIRCLE

Q223 CIRCLE DIAMETER

1273 OCM SLOT / RIDGE

Q219 SLOT WIDTH,

Q218 SLOT LENGTH

1278 OCM POLYGON

Q571 REF-CIRCLE DIAMETER

You can define the following tolerances:

Tolerances

Example

Manufacturing dimension

Dimensions

10+0.01-0.015

9.9975

DIN EN ISO 286-2

10H7

10.0075

DIN ISO 2768-1

10m

10.0000

 
Tip

Pay attention to capitalization when entering tolerances.

  1. Proceed as follows:
  2. Start the cycle definition
  3. Define the cycle parameters
  4. Select TEXT in the action bar
  5. Enter a nominal dimension including tolerance
 
Tip

If you program an incorrect tolerance, the control interrupts machining with an error message.