Cycle 276 THREE-D CONT. TRAIN

ISO programming

G276

Application

In conjunction with Cycle 14 CONTOUR and Cycle 270 CONTOUR TRAIN DATA, this cycle enables you to machine open and closed contours. You can also work with automatic residual material detection. This way you can subsequently complete for example inside corners with a smaller tool.

In contrast to Cycle 25 CONTOUR TRAIN, Cycle 276 THREE-D CONT. TRAIN also processes tool axis coordinates defined in the contour subprogram. This cycle can thus machine three-dimensional contours.

We recommend that you program Cycle 270 CONTOUR TRAIN DATA before Cycle 276 THREE-D CONT. TRAIN.

Cycle run

Machining a contour without infeed: Milling depth Q1 = 0

  1. The tool traverses to the starting point of machining. This starting point results from the first contour point, the selected milling mode (climb or up-cut) and the parameters from the previously defined Cycle 270 CONTOUR TRAIN DATA (e.g., the Type of approach). The control then moves the tool to the first plunging depth
  2. According to the previously defined Cycle 270 CONTOUR TRAIN DATA, the tool approaches the contour and then machines it completely to the end
  3. At the end of the contour, the tool will be retracted as defined in Cycle 270 CONTOUR TRAIN DATA
  4. Finally, the control retracts the tool to the clearance height.

Machining a contour with infeed: Milling depth Q1 not equal to 0 and plunging depth Q10 are defined

  1. The tool traverses to the starting point of machining. This starting point results from the first contour point, the selected milling mode (climb or up-cut) and the parameters from the previously defined Cycle 270 CONTOUR TRAIN DATA (e.g., the Type of approach). The control then moves the tool to the first plunging depth
  2. According to the previously defined Cycle 270 CONTOUR TRAIN DATA, the tool approaches the contour and then machines it completely to the end
  3. If you selected machining with climb milling and up-cut milling (Q15 = 0), the control will perform a reciprocation movement. The infeed movement (plunging) will be performed at the end and at the starting point of the contour. If Q15 is not equal to 0, the tool is moved to clearance height and is returned to the starting point of machining. From there, the control moves the tool to the next plunging depth
  4. The departure will be performed as defined in Cycle 270 CONTOUR TRAIN DATA
  5. This process is repeated until the programmed depth is reached.
  6. Finally, the control retracts the tool to the clearance height

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
 
Notice
Danger of collision!
A collision may occur if you position the tool behind an obstacle before the cycle is called.
  1. Before the cycle call, position the tool in such a way that the tool can approach the starting point of the contour without collision
  2. If the position of the tool is below the clearance height when the cycle is called, the control will issue an error message
  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • If you program APPR and DEP blocks for contour approach and departure, the control monitors whether the execution of any of these blocks would damage the contour.
  • If using Cycle 25 CONTOUR TRAIN, you can define only one subprogram in Cycle 14 CONTOUR.
  • We recommend that you use Cycle 270 CONTOUR TRAIN DATA in conjunction with Cycle 276. Cycle 20 CONTOUR DATA, however, is not required.
  • The memory capacity for programming an SL cycle is limited. You can program up to 16384 contour elements in one SL cycle.
  • If M110 is activated during operation, the feed rate for arcs compensated on the inside will be reduced accordingly.
  • 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

Notes on programming

  • The first NC block in the contour subprogram must contain values in all of the three axes X, Y and Z.
  • The algebraic sign for the depth parameter determines the working direction. If you program DEPTH = 0, the control will use the tool axis coordinates that have been specified in the contour subprogram.
  • If you use local QL Q parameters in a contour subprogram, you must also assign or calculate these in the contour subprogram.

Cycle parameters

Help graphic

Parameter

Q1 Milling depth?

Distance between workpiece surface and contour floor. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q3 Finishing allowance for side?

Finishing allowance in the working plane. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q7 Clearance height?

Height at which the tool cannot collide with the workpiece (for intermediate positioning and retraction at the end of the cycle). This value has an absolute effect.

Input: –99999.9999...+99999.9999

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

Q15 Climb or up-cut? up-cut = -1

+1: Climb milling

-1: Up-cut milling

0: Climb milling and up-cut milling alternately in several infeeds

Input: -1, 0, +1

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

Q446 Accepted residual material? (optional)

Specify the maximum value in mm up to which you accept residual material on the contour. For example, if you enter 0.01 mm, the control will stop machining residual material when it has reached a thickness of 0.01 mm.

Input: 0.001...9.999

Q447 Maximum connection distance? (optional)

Maximum distance between two areas to be fine-roughed. Within this distance, the tool will move along the contour without lift-off movement, remaining at machining depth.

Input: 0...999.999

Q448 Path extension? (optional)

Length by which the tool path is extended at the beginning and end of a contour area. The control always extends the tool path in parallel to the contour.

Input: 0...99.999

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 276 THREE-D CONT. TRAIN ~

Q1=-20

;MILLING DEPTH ~

Q3=+0

;ALLOWANCE FOR SIDE ~

Q7=+50

;CLEARANCE HEIGHT ~

Q10=-5

;PLUNGING DEPTH ~

Q11=+150

;FEED RATE FOR PLNGNG ~

Q12=+500

;FEED RATE F. ROUGHNG ~

Q15=+1

;CLIMB OR UP-CUT ~

Q18=+0

;COARSE ROUGHING TOOL ~

Q446=+0.01

;RESIDUAL MATERIAL ~

Q447=+10

;CONNECTION DISTANCE ~

Q448=+2

;PATH EXTENSION