Cycle 22 ROUGH-OUT

ISO programming

G122

Application

Use Cycle 22 ROUGH-OUT to define the technology data for roughing.

Before programming the call of Cycle 22, you need to program further cycles:

  • Cycle 14 CONTOUR or SEL CONTOUR
  • Cycle 20 CONTOUR DATA
  • Cycle 21 PILOT DRILLING, if applicable

Cycle run

  1. The control positions the tool above the cutter infeed point, taking the finishing allowance for side into account
  2. After reaching the first plunging depth, the tool mills the contour in an outward direction at the programmed milling feed rate Q12
  3. The island contours (here: C/D) are cleared out with an approach toward the pocket contour (here: A/B)
  4. In the next step, the control moves the tool to the next plunging depth and repeats the roughing procedure until the program depth is reached
  5. Finally, the tool retracts in the tool axis to the clearance height or to the position last programmed before the cycle. This behavior depends on the machine parameter posAfterContPocket (no. 201007).

Notes

 
Notice
Danger of collision!
If you have set the posAfterContPocket parameter (no. 201007) to ToolAxClearanceHeight, the control will position the tool at clearance height only in the direction of the tool axis when the cycle has finished. The control will not position the tool in the working plane. There is a danger of collision!
  1. After the end of the cycle, position the tool with all coordinates of the working plane (e.g., L X+80 Y+0 R0 FMAX)
  2. Make sure to program an absolute position after the cycle; do not program an incremental traversing movement
  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • During fine roughing, the control does not take a defined wear value DR of the coarse roughing tool into account.
  • If M110 is activated during operation, the feed rate for arcs compensated on the inside will be reduced accordingly.
  • This cycle monitors the defined usable length LU of the tool. If the LU value is less than the DEPTH Q1, the control will display an error message.
  • The cycle considers the miscellaneous functions M109 and M110. During the inside and outside machining of circular arcs the control keeps the feed rate constant at the cutting edge for inside and outside radii.
  • Adapting the feed rate for circular paths with M109

 
Tip

This cycle might require a center-cut end mill (ISO 1641) or pilot drilling with Cycle 21.

Notes on programming

  • If you clear out an acute inside corner and use an overlap factor greater than 1, some material might be left over. Check especially the innermost path in the test run graphic and, if necessary, change the overlap factor slightly. This allows another distribution of cuts, which often provides the desired results.
  • Define the plunging behavior of Cycle 22 with parameter Q19 and in the ANGLE and LCUTS columns of the tool table:
    • If Q19=0 is defined, the tool will always plunge perpendicularly, even if a plunge angle (ANGLE) has been defined for the active tool.
    • If you define ANGLE = 90°, the control will plunge perpendicularly. The reciprocation feed rate Q19 is used as plunging feed rate.
    • If the reciprocation feed rate Q19 is defined in Cycle 22 and ANGLE is between 0.1 and 89.999 in the tool table, the control plunges helically using the defined ANGLE.
    • If the reciprocation feed is defined in Cycle 22 and no ANGLE can be found in the tool table, the control displays an error message.
    • If the geometry conditions do not allow helical plunging (slot geometry), the control tries a reciprocating plunge (the reciprocation length is calculated from LCUTS and ANGLE (reciprocation length = LCUTS / tan ANGLE))

Note regarding machine parameters

  • Use the machine parameter posAfterContPocket (no. 201007) to define how to move the tool after machining the contour pocket.
    • PosBeforeMachining: Return to starting position
    • ToolAxClearanceHeight: Position the tool axis to clearance height.

Cycle parameters

Help graphic

Parameter

Q10 Plunging depth?

Tool infeed per cut. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q11 Feed rate for plunging?

Traversing feed rate in the spindle axis

Input: 0...99999.9999 or FAUTO, FU, FZ

Q12 Feed rate for roughing?

Traversing feed rate in the working plane

Input: 0...99999.9999 or FAUTO, FU, FZ

Q18 or QS18 Coarse roughing tool? (optional)

Number or name of the tool with which the control has already coarse-roughed the contour. You can use the action bar selection to apply the coarse roughing tool directly from the tool table. In addition, you can enter the tool name yourself by selecting Name in the action bar. The control automatically inserts the closing quotation mark when you exit the input field. If there was no coarse roughing, enter "0"; if you enter a number or a name, the control will only rough-out the portion that could not be machined with the coarse roughing tool. If the portion to be roughed cannot be approached from the side, the control will mill in a reciprocating plunge-cut; for this purpose you must enter the tool length LCUTS in the TOOL.T tool table and define the maximum plunging angle of the tool with ANGLE.

Input: 0...99999.9 or max. 255 characters

Q19 Feed rate for reciprocation? (optional)

Reciprocation feed rate in mm/min

Input: 0...99999.9999 or FAUTO, FU, FZ

Q208 Feed rate for retraction? (optional)

Tool traversing speed in mm/min when retracting after the machining operation. If you enter Q208 = 0, the control retracts the tool at the feed rate specified in Q12.

Input: 0...99999.9999 or FMAX, FAUTO, PREDEF

Q401 Feed rate factor in %? (optional)

Percentage value to which the control reduces the machining feed rate (Q12) as soon as the tool moves with its entire circumference within the material during roughing. If you use the feed rate reduction, then you can define the feed rate for roughing so large that there are optimum cutting conditions with the path overlap (Q2) specified in Cycle 20. The control then reduces the feed rate as per your definition at transitions and narrow places, reducing the total machining time.

Input: 0.0001...100

Q404 Fine roughing strategy (0/1)? (optional)

Define how the control moves the tool during fine roughing:

0: Between areas that need to be fine-roughed, the control moves the tool along the contour at the current depth. The entry is effective only when the diameter of the fine-roughing tool is larger than or equal to the coarse roughing tool radius.

1: Between the areas that need to be fine-roughed, the control retracts the tool to the set-up clearance and then moves it to the starting point of the next area to be roughed out.

Input: 0, 1

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 22 ROUGH-OUT ~

Q10=-5

;PLUNGING DEPTH ~

Q11=+150

;FEED RATE FOR PLNGNG ~

Q12=+500

;FEED RATE F. ROUGHNG ~

Q18=+0

;COARSE ROUGHING TOOL ~

Q19=+0

;FEED RATE FOR RECIP. ~

Q208=+99999

;RETRACTION FEED RATE ~

Q401=+100

;FEED RATE FACTOR ~

Q404=+0

;FINE ROUGH STRATEGY