Cycle 32 TOLERANCE
ISO programming
G62
Application
Refer to your machine manual.
Machine and control must be specially prepared by the machine manufacturer for use of this cycle.
With the entries in Cycle 32 you can influence the result of HSC machining with respect to accuracy, surface definition and speed, in as much as the control has been adapted to the machine’s characteristics.
The control automatically smooths the contour between any two contour elements (whether corrected or not). This means that the tool has constant contact with the workpiece surface and therefore reduces wear on the machine tool. The tolerance defined in the cycle also affects the traverse paths on circular arcs.
If necessary, the control automatically reduces the programmed feed rate so that the program can be executed at the fastest possible speed without jerking. Even if the control does not move the axes with reduced speed, it will always comply with the tolerance that you have defined. The larger you define the tolerance, the faster the control can move the axes.
Smoothing the contour results in a certain amount of deviation from the contour. The size of this contour error (tolerance value) is set in a machine parameter by the machine manufacturer. With Cycle 32 you can change the pre-set tolerance value and select different filter settings, provided that your machine manufacturer has implemented these features.
With very small tolerance values the machine cannot cut the contour without jerking. These jerking movements are not caused by poor processing power in the control, but by the fact that, in order to machine the contour transitions very exactly, the control might have to drastically reduce the speed.
Reset
The control resets Cycle 32 if you do one of the following:
- Redefine Cycle 32 and confirm the dialog prompt for the tolerance value with NO ENT
- Select a new NC program
After you have reset Cycle 32, the control reactivates the tolerance that was predefined by the machine parameters.
Influences of the geometry definition in the CAM system
The most important factor of influence in offline NC program creation is the chord error S defined in the CAM system. The chord error defines the maximum point spacing of NC programs generated in a postprocessor (PP). If the chord error is less than or equal to the tolerance value T defined in Cycle 32, then the control can smooth the contour points unless any special machine settings limit the programmed feed rate.
You will achieve optimal smoothing of the contour if you choose a tolerance value in Cycle 32 between 110% and 200% L of the CAM chord error.
Related topics
- Working with CAM-generated NC programs
Notes
- Watch out for possible collisions!
- Define the T-FMAX parameter in accordance with the machining operation
- Use only a single tuning or optimization cycle
- Deactivate active cycles, if necessary, in order to avoid overlaps
- You can execute this cycle in the following operating modes: FUNCTION MODE MILL.
- Cycle 32 is DEF-active which means that it takes effect as soon as it is defined in the NC program.
- In a program with millimeters set as unit of measure, the control interprets the tolerance values entered in T and T-FMAX as millimeters. In an inch program, it interprets them as inches.
- As the tolerance value increases, the diameter of circular movements usually decreases, unless HSC filters are active on your machine (set by the machine manufacturer).
- If Cycle 32 is active, the control shows the defined cycle parameters on the CYC tab of the additional status display.
Keep the following in mind for 5-axis simultaneous machining!
- NC programs for 5-axis simultaneous machining with spherical cutters should preferably be output for the center of the sphere. The NC data are then generally more uniform. In Cycle 32, you can additionally set a higher rotary axis tolerance TA (e.g., between 1° and 3°) for an even more constant feed-rate curve at the tool center point (TCP).
- For NC programs for 5-axis simultaneous machining with toroid cutters or spherical cutters, where the NC output is for the south pole of the sphere, choose a lower rotary axis tolerance. 0.1° is a typical value. However, the maximum permissible contour damage is the decisive factor for the rotary axis tolerance. This contour damage depends on the possible tool tilting, tool radius and engagement depth of the tool.
With 5-axis hobbing with an end mill, you can calculate the maximum possible contour damage T directly from the cutter engagement length L and permissible contour tolerance TA:
T ~ K x L x TA K = 0.0175 [1/°]
Example: L = 10 mm, TA = 0.1°: T = 0.0175 mm
Sample formula for a toroid cutter:
When machining with a toroid cutter, the angle tolerance is very important.
Tw: Angle tolerance in degrees
π: Circular constant (pi)
R: Major radius of the torus in mm
T32: Machining tolerance in mm
Cycle parameters
Help graphic | Parameter |
---|---|
T Tolerance of contour deviation Permitted contour deviation in mm or inch >0: The control uses the maximum permitted deviation you have specified. 0: The control uses a value configured by the machine manufacturer. When skipping this parameter with NO ENT, the control uses a value configured by the machine manufacturer. Input: 0...10 | |
HSC-MODE: Finishing=0, Roughing=1 Activate filter: 0: Milling with increased contour accuracy. The control uses internally defined finishing filter settings. 1: Milling with increased feed rate. The control uses internally defined roughing filter settings. Input: 0, 1 | |
TA Tolerance for rotary axes Permissible position error of rotary axes in degrees with active M128 (FUNCTION TCPM). The control always reduces the feed rate in such a way that—if more than one axis is traversed—the slowest axis moves at its maximum feed rate. Rotary axes are usually much slower than linear axes. You can significantly reduce the machining time for NC programs for more than one axis by entering a large tolerance value (e.g., 10°), because the control does not always have to position the rotary axis at the given nominal position. The tool orientation (position of the rotary axis with respect to the workpiece surface) will be adjusted. The position at the Tool Center Point (TCP) will be corrected automatically. For example, with a spherical cutter measured in its center and programmed based on the center path, there will be no adverse effects on the contour. >0: The control uses the maximum permitted deviation you have programmed. 0: The control uses a value configured by the machine manufacturer. When skipping this parameter with NO ENT, the control uses a value configured by the machine manufacturer. Input: 0...10 | |
T-FMAX Tolerance of path deviation at rapid traverse Permitted path deviation in rapid traverse FMAX in mm or inches >0: In positioning blocks with FMAX, the control uses the maximum permitted deviation you have specified. 0: In positioning blocks with FMAX, the control uses the same tolerance as in the T parameter. When removing this parameter with NO ENT, the control uses the same tolerance as in the T parameter. Input: 0...10 |
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 32.0 TOLERANCE |
12 CYCL DEF 32.1 T0.02 |
13 CYCL DEF 32.2 HSC-MODE:1 TA5 |
13 CYCL DEF 32.3 T-FMAX2 |