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

Requirement

  • Opt. Contour Milling (#167 / #1-02-1) software option

Description of function

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.

The control provides the following cycles for figure definition:

The control provides the following cycles for figure boundary definition:

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

1274 OCM CIRCULAR SLOT

Q219 SLOT WIDTH

1278 OCM POLYGON

Q571 REF-CIRCLE DIAMETER

You can define the following tolerances:

Tolerances

Example

Manufacturing dimension

DIN EN ISO 286-2

10H7

10.0075

DIN ISO 2768-1

10m

10.0000

Nominal dimension

10+0.01-0.015

9.9975

You can enter nominal dimensions with the following tolerances:

Combination

Example

Manufacturing dimension

a+-b

10+-0.5

10.0

a-+b

10-+0.5

10.0

a-b+c

10-0.1+0.5

10.2

a+b-c

10+0.1-0.5

9.8

a+b+c

10+0.1+0.5

10.3

a-b-c

10-0.1-0.5

9.7

a+b

10+0.5

10.25

a-b

10-0.5

9.75

Proceed as follows:

  1. Start the cycle definition
  2. Define the cycle parameters
  3. Select NAME in the action bar
  4. Enter a nominal dimension including tolerance
 
Tip
  • The control produces the workpiece to comply with the mean tolerance value.
  • If you program a tolerance that does not comply with the DIN standard or if you indicate tolerances incorrectly when programming nominal dimensions (e.g., by entering blanks), the control aborts execution and displays an error message.
  • Ensure correct upper and lower case when entering the DIN EN ISO and DIN ISO tolerances. Entering space characters is not allowed.