Cylinder surface machining with CYLINDER SURFACE (#8 / #1-01-1)
Application
The CYLINDER SURFACE NC function allows you to machine the cylinder surface with various NC functions, for example OCM cycles (#167 / #1-02-1), pocket milling cycles or path functions.
Related topics
- Cycles for cylinder surface machining
- OCM cycles
- Pocket milling cycles
- Path functions
Requirements
- Machine with at least one rotary table axis
Rotary table axis as modulo axis
- Software option Adv. Function Set 1 (#8 / #1-01-1)
- The cylinder is set up centered and perpendicular on the rotary table
Workpiece preset in the center and on the surface of the cylinder
- Milling operation FUNCTION MODE MILL
- PARAX COMP DISPLAY NC function programmed with at least the main axes X, Y and Z
HEIDENHAIN recommends defining all of the available axes within the PARAX COMP DISPLAY function.
- Tool call with tool axis Z
- No active coordinate transformation such as TRANS ROTATION
- Working plane for cylinder surface machining:
- Cylinder axis parallel to a machine axis
- Tool axis parallel to a machine axis and perpendicular above the cylinder axis
- Tip
Machines with axes installed at a right angle or at 45 degrees meet these conditions after tilting the working plane, if required.
Different kinematics possibly do not allow you to meet these conditions.
Description of function
Use the NC function CYLINDER SURFACE ON to activate cylinder surface machining. When the NC function CYLINDER SURFACE is active, the control displays an icon in the Positions workspace. This icon covers the icon for the PARAX COMP DISPLAY NC function.
The control deactivates cylinder surface machining in the following cases:
- CYLINDER SURFACE OFF
- M2 or M30
- End of program END PGM
- Cancellation of an NC program
You program the contour or machining cycles on the unrolled surface of the cylinder. The control transfers the programmed values to the cylinder surface. The control automatically calculates the feed rate of the rotary table axis based on the programmed feed rate and the cylinder diameter.
Use the X and Y coordinates to program the contour or machining cycles, independent of which rotary axes exist on your machine. The X coordinate describes the circumference of the cylinder and defines the position of the rotary table axis. The Y coordinate is on the cylinder axis. The Z axis serves as infeed axis.
The following table shows a possible sequence for cylinder surface machining:
Description | Help graphic |
---|---|
The workpiece preset is in the center and on the surface of the cylinder. | |
You tilt the working plane to the spatial angle SPB-90 and position the tool in the Y axis on the value 0. The working plane is tilted to the spatial angle SPB-90. The tool is thus oriented perpendicularly above the cylinder axis. Due to the tilted working plane, the cylinder axis and the tool axis are each parallel to a machine axis. | |
You activate the NC function CYLINDER SURFACE. The control automatically shifts the workpiece datum in the direction of the tool axis on the cylinder surface:
| |
You shift the workpiece datum in the direction Y-. | |
You program the contour on the unrolled surface of the cylinder. | |
The completed contour is transferred to the cylinder surface. |
If the CYLINDER SURFACE NC function is active, the tool is positioned perpendicularly to the cylinder surface and as a result, the tool center is aligned with the cylinder center. If the X coordinate changes, the control moves the rotary table axis and not the tool.
This results in the following effects:
- When using a contour definition with Y coordinates, the walls are not parallel to each other.
- The bottom of a pocket, for example, can be uneven.
- When you produce threads using thread milling cycles, the threads will be conical.
Only use tapping cycles for cylinder surface machining.
If cylinder surface machining is active, do not use the following NC functions:
- M91/M92
- TOOL CALL
- M140
- M144 (#9 / #4-01-1)
- POLARKIN
- Tool radius compensation
- 3D tool compensation (#9 / #4-01-1)
- FUNCTION TCPM or M128 (#9 / #4-01-1)
- Rotary axis movements
- Tilting the working plane with PLANE functions
- Switching the machining mode with FUNCTION MODE
- Handwheel superimpositioning with M118 (#21 / #4-02-1)
Input
CYLINDER SURFACE ON
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 CYLINDER SURFACE ON D99 X AS LIN | ; Activate cylinder surface machining and define the cylinder size |
To navigate to this function:
Insert NC function All functions Special functions Functions Cylinder kinematics CYLINDER SURFACE ON
The NC function includes the following syntax elements:
Syntax element | Meaning |
---|---|
CYLINDER SURFACE ON | Syntax initiator for activating cylinder surface machining |
R or D | Radius or diameter of the cylinder Number or numerical parameter |
X AS | Axis of the unrolled surface of the cylinder |
LIN or DEG | Indication of coordinates defining the unrolled surface of the cylinder as length or angle DEG currently has no function If DEG is selected, the control will display the error message Block format incorrect. |
CYLINDER SURFACE OFF
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 CYLINDER SURFACE OFF | ; Deactivate cylinder surface machining |
To navigate to this function:
Insert NC function All functions Special functions Functions Cylinder kinematics CYLINDER SURFACE OFF
The NC function includes the following syntax elements:
Syntax element | Meaning |
---|---|
CYLINDER SURFACE OFF | Syntax initiator for deactivating cylinder surface machining |
Note
If a basic rotation around the cylinder axis is active, you always must tilt the working plane using, for example, PLANE SPATIAL SPA+0 SPB+0 SPC+0 before machining the cylinder surface.
Basic rotation and 3D basic rotation
Program structure for cylinder surface machining
Here you see a possible program structure for cylinder surface machining.
BLK FORM... | ||
TOOL CALL... | ||
If required, tilt the working plane | PLANE SPATIAL... | |
Pre-position above the cylinder axis | L X... Y+0 Z... | |
Activate cylinder surface machining | CYLINDER SURFACE ON... | |
Shift datum, if required | TRANS DATUM... | |
Machine cylinder surface | CYCL DEF 251 RECTANGULAR POCKET | ; E.g., pocket milling cycle |
CYCL CALL... | ||
Reset datum shift | TRANS RESET | |
Deactivate cylinder surface machining | CYLINDER SURFACE OFF | |
If required, reset tilt angle and deactivate tilting of the working plane | PLANE RESET... | |
... |
Example: Rectangular pocket with CYLINDER SURFACE
The following machining operations were already executed on the workpiece blank BLANK.STL:
- Outside diameter as circular stud
- Inside diameter as circular pocket
- Chamfering at circular pocket and circular stud
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.
0 BEGIN PGM 1442806 MM | |||
1 BLK FORM FILE "Blank.stl" | |||
2 CALL LBL "RESET" | |||
3 ; | |||
4 * - | ; Main program | ||
5 FUNCTION PARAX COMP DISPLAY X Y Z | ; Activate FUNCTION PARAX COMP DISPLAY | ||
6 TOOL CALL "MILL_D10" Z S15000 | |||
7 PLANE SPATIAL SPA+0 SPB+90 SPC+0 TURN MB MAX FMAX | ; Tilt the working plane | ||
8 L X+0 Y+0 R0 FMAX M3 | ; Pre-position above the cylinder axis | ||
9 ; | |||
10 CYLINDER SURFACE ON D99 X AS LIN | ; Activate cylinder surface machining | ||
11 ; | |||
12 TRANS DATUM AXIS Y-36 | ; Shift workpiece datum in direction Y- | ||
13 CONTOUR DEF P1 = LBL "Pocket" | |||
14 CYCL DEF 271 OCM CONTOUR DATA ~ | |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
15 CYCL DEF 272 OCM ROUGHING ~ | |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
16 CYCL CALL | |||
17 CYCL DEF 274 OCM FINISHING SIDE ~ | |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
18 CYCL CALL | |||
19 TRANS RESET | ; Reset datum shift | ||
20 ; | |||
21 CYLINDER SURFACE OFF | ; Deactivate cylinder surface machining | ||
22 ; | |||
23 CALL LBL "RESET" | |||
24 TOOL CALL "CHAMFERING_D10" Z S15000 | |||
25 PLANE SPATIAL SPA+0 SPB+90 SPC+0 TURN MB MAX FMAX | ; Tilt the working plane | ||
26 L X+0 Y+0 R0 FMAX M3 | ; Pre-position above the cylinder axis | ||
27 ; | |||
28 CYLINDER SURFACE ON D99 X AS LIN | ; Activate cylinder surface machining | ||
29 ; | |||
30 TRANS DATUM AXIS Y-36 | ; Shift workpiece datum in direction Y- | ||
31 CONTOUR DEF P1 = LBL "Pocket" | |||
32 CYCL DEF 271 OCM CONTOUR DATA ~ | |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
33 CYCL DEF 277 OCM CHAMFERING ~ | |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
34 CYCL CALL | |||
35 TRANS RESET | ; Reset datum shift | ||
36 ; | |||
37 CYLINDER SURFACE OFF | ; Deactivate cylinder surface machining | ||
38 FUNCTION PARAX COMP OFF X Y Z | ; Deactivate FUNCTION PARAX COMP | ||
39 ; | |||
40 CALL LBL "RESET" | |||
41 M30 | |||
42 ; | |||
43 * - | ; Subprograms | ||
44 LBL "Pocket" | |||
45 L X+25 Y+31 | |||
46 L X+25 Y+5 | |||
47 L X-25 Y+5 | |||
48 L X-25 Y+31 | |||
49 L X+25 Y+31 | |||
50 LBL 0 | |||
51 ; | |||
52 LBL "SAFE" | |||
53 M140 MB+50 | |||
54 L Z+300 R0 FMAX M91 | |||
55 L X+400 Y-300 R0 FMAX M91 | |||
56 LBL 0 | |||
57 ; | |||
58 LBL "RESET" | |||
59 FUNCTION RESET TCPM | |||
60 M140 MB+50 | |||
61 CALL LBL "SAFE" | |||
62 TRANS DATUM RESET | |||
63 PLANE RESET TURN FMAX | |||
64 LBL 0 | |||
65 END PGM 1442806 MM |
Definition
Modulo axis
Modulo axes are axes whose encoder only returns values between 0° and 359.9999°. If an axis is used as a spindle, then the machine manufacturer must configure this axis as a modulo axis.