Cycle 39 CYL. SURFACE CONTOUR (#8 / #1-01-1)
ISO programming
G139
Application
Refer to your machine manual.
This function must be enabled and adapted by the machine manufacturer.
This cycle enables you to machine a contour on a cylindrical surface. The contour to be machined is programmed on the unrolled surface of the cylinder. With this cycle, the control adjusts the tool in such a way that, with radius compensation active, the walls of the milled contour are always parallel to the cylinder axis.
Describe the contour in a subprogram that you program with Cycle 14 CONTOUR.
In the subprogram you always describe the contour with the coordinates X and Y, regardless of which rotary axes exist on your machine. This means that the contour description is independent of your machine configuration. The path functions L, CHF, CR, RND and CT are available.
Unlike in Cycles 28 and 29, in the contour subprogram, you define the contour actually to be machined.
Cycle sequence
- The control positions the tool above the starting point of machining. The control locates the starting point next to the first point defined in the contour subprogram offset by the tool diameter
- The control then moves the tool vertically to the first plunging depth. The tool approaches the workpiece on a tangential path or on a straight line at the milling feed rate Q12. A finishing allowance programmed for the side is taken into account. The approach behavior depends on the machine parameter apprDepCylWall (no. 201004)
- At the first plunging depth, the tool mills along the programmed contour at the milling feed rate Q12 until the contour train is complete.
- The tool then departs the ridge wall on a tangential path and returns to the starting point of machining.
- Steps 2 to 4 are repeated until the programmed milling depth Q1 is reached.
- Finally, the tool retracts in the tool axis to the clearance height.
The cylinder must be set up centered on the rotary table. Set the preset to the center of the rotary table.
Notes
This cycle performs an inclined machining operation. To run this cycle, the first machine axis below the machine table must be a rotary axis. In addition, it must be possible to position the tool perpendicular to the cylinder surface.
- By setting the displaySpindleErr machine parameter (no. 201002) to on/off, you can define whether the control displays an error message or not in case the spindle is not switched on.
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- The spindle axis must be perpendicular to the rotary table axis when the cycle is called.
- Ensure that the tool has enough space laterally for contour approach and departure.
- The machining time can increase if the contour consists of many non-tangential contour elements.
Notes on programming
- In the first NC block of the contour program, always program both cylinder surface coordinates.
- The algebraic sign for the DEPTH cycle parameter determines the working direction. If you program DEPTH=0, the cycle will not be executed.
- The set-up clearance must be greater than the tool radius.
- If you use local QL Q parameters in a contour subprogram, you must also assign or calculate these in the contour subprogram.
Note regarding machine parameters
- Use machine parameter apprDepCylWall (no. 201004) to define the approach behavior:
- CircleTangential: Tangential approach and departure
- LineNormal: The tool approaches the contour starting point on a straight line
Cycle parameters
Help graphic | Parameter |
---|---|
Q1 Milling depth? Distance between cylindrical surface and contour floor. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q3 Finishing allowance for side? Finishing allowance in the plane of the unrolled cylindrical surface. This allowance is effective in the direction of the radius compensation. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q6 Set-up clearance? Distance between the tool face and the cylindrical surface. This value has an incremental effect. Input: –99999.9999...+99999.9999 or PREDEF | |
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 | |
Q16 Cylinder radius? Radius of the cylinder on which the contour will be machined. Input: 0...99999.9999 | |
Q17 Dimension type? deg=0 MM/INCH=1 Program the rotary axis coordinates in degrees or mm (inches) in the subprogram. 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.
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.
11 CYCL DEF 39 CYL. SURFACE CONTOUR ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|