Cycle 208 BORE MILLING

ISO programming

G208

Application

With this cycle, you can mill holes. In this cycle, you can define an optional, pre-drilled diameter. You can also program tolerances for the nominal diameter.

Cycle run

  1. The control positions the tool in the spindle axis at rapid traverse FMAX to the entered set-up clearance Q200 above the workpiece surface
  2. The control moves on a semicircle for the first helical path while considering the path overlap Q370. The semicircle begins at the center of the hole.
  3. The tool mills in a helix to the entered drilling depth at the programmed feed rate F.
  4. When the drilling depth is reached, the control once again traverses a full circle to remove the material remaining after the initial plunge.
  5. The control then centers the tool in the hole again and retracts it to set-up clearance Q200.
  6. This procedure is repeated until the nominal diameter is reached (the control calculates the stepover by itself)
  7. Finally, the tool is retracted to the set-up clearance or to the 2nd set-up clearance Q204 at rapid traverse FMAX. The 2nd set-up clearance Q204 will only come into effect if its value is greater than the set-up clearance Q200
 
Tip

If you program Q370=0 for the path overlap, the control uses the greatest path overlap possible for the first helical path. The control does this to prevent the tool from contacting the workpiece surface. All other paths are distributed uniformly.

Tolerances

The control allows you to store tolerances in the parameter Q335 NOMINAL 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.

Notes

 
Notice
Danger of collision!
If you enter the depth in a cycle as a positive value, the control reverses the calculation of the pre-positioning. The tool moves at rapid traverse in the tool axis to set-up the clearance below the workpiece surface! There is a danger of collision!
  1. Enter depth as negative
  2. 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
 
Notice
Caution: Danger to the workpiece and tool!
If the selected infeed is too large, there is a danger of tool breakage and damage to the workpiece.
  1. Specify the maximum possible plunge angle and the corner radius DR2 in the ANGLE column of the TOOL.T tool table.
  2. The control automatically calculates the max. permissible infeed and changes your entered value accordingly, if necessary.
  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • If you have entered the bore hole diameter to be the same as the tool diameter, the control will bore directly to the entered depth without any helical interpolation.
  • An active mirror function does not influence the type of milling defined in the cycle.
  • When calculating the overlap factor, the control takes the corner radius DR2 of the current tool into account so that the bottom of the hole will be as level as possible. The overlap factor is reduced to a minimum.
  • 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.
  • The control uses the RCUTS value in the cycle to monitor non-center-cut tools and to prevent the tool from front-face touching. If necessary, the control interrupts machining and issues an error message.

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.

Cycle parameters

Help graphic

Parameter

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

Q201 Depth?

Distance between workpiece surface and bottom of hole. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q206 Feed rate for plunging?

Traversing speed of the tool in mm/min during helical drilling

Input: 0...99999.999 or FAUTO, FU, FZ

Q334 Feed per revolution of helix

Depth of the tool plunge with each helix (=360°). This value has an incremental effect.

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

Q335 Nominal diameter?

Hole diameter. If you entered the nominal diameter to be the same as the tool diameter, the control will bore directly to the entered depth without any helical interpolation. This value has an absolute effect. You can program a tolerance if needed.

Tolerances

Input: 0...99999.9999

Q342 Roughing diameter? (optional)

Enter the dimension of the pre-drilled diameter. This value has an absolute effect.

Input: 0...99999.9999

Q351 Direction? Climb=+1, Up-cut=-1 (optional)

Type of milling operation. The direction of spindle rotation is taken into account.

+1 = climb milling

–1 = up-cut milling

(if you enter 0, climb milling is performed)

Input: -1, 0, +1 or PREDEF

Q370 Path overlap factor? (optional)

The control uses the path overlap factor to determine the stepover factor k.

0: The control uses the greatest path overlap possible for the first helical path. The control does this to prevent the tool from contacting the workpiece surface. All other paths are distributed uniformly.

>0: The control multiplies the factor by the active tool radius. The result is the stepover factor k.

Input: 0.1...1999 or PREDEF

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.

 
Tip

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.

Example

11 CYCL DEF 208 BORE MILLING ~

Q200=+2

;SET-UP CLEARANCE ~

Q201=-20

;DEPTH ~

Q206=+150

;FEED RATE FOR PLNGNG ~

Q334=+0.25

;PLUNGING DEPTH ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+50

;2ND SET-UP CLEARANCE ~

Q335=+5

;NOMINAL DIAMETER ~

Q342=+0

;ROUGHING DIAMETER ~

Q351=+1

;CLIMB OR UP-CUT ~

Q370=+0

;TOOL PATH OVERLAP

12 CYCL CALL