|
|
|
|
|||
|
|
|
|
|
This version of Spiral Pocketing (in both the In-Out and Out-In cycles) uses a different algorithm and contains many options to control the creation of the tool path than the other Spiral Pocketing cycles. This method allows for more complex geometry to be handed to the tool path generator.
Spiral Pocket Out-In will start at a point at the outside edge of the pocket and create offset tool paths, moving toward the inside of the pocket. There are parameters to allow a plunge start or a ramp start, and also options for keeping the tool down while in the pocket or allowing the tool to pick up and move to another area of the pocket to continue the shape.
Note: This cycle is only available on 32-bit Operating Systems. If you are running a 64-bit Operating System, you will be able to use the Advanced Pocketing cutting cycles including Advanced Rest Pocketing. |
Spiral Pocket Out2In tool path.
Spiral Out2In parameters.
The following parameters effect the toolpath creation:
The value of 'Y' defines that the cycle will start on the outside portion of the geometry and work its way to the inside of the geometry. To have it work from the inside of the geometry to the outside, select the cutting cycle 'Spiral In2Out'.
The value of 'N' defines that it will NOT work from the inside of the geometry to the outside of the geometry. To have it work from the inside of the geometry to the outside, select the cutting cycle 'Spiral In2Out'.
The value is not applicable to a Spiral Pocket function.
The value is not applicable to a Spiral Pocket function.
The value is not applicable to a Spiral Pocket function.
The value is not applicable to a Spiral Pocket function.
The value entered here will be added to Finish Pass above to provide material left for a clean up pass on the pocket with a separate tool.
This value is the percentage of the tool diameter between each pass of the tool in the pocket. This needs to be a real number such as 25.0 or 50.0.
The value represents if the cutting cycle will be doing Climb (CCW) milling <Y> or if you want the cutting cycle to do Conventional (CW) milling <N>
A CleanUp Pass is described as an additional tool path that travels around geometry allowing you to use Cutter Compensation for the boundary of the geometry.
A Ramp-In set to <Y> will allow you to have the cutting cycle enter the cut with a ramp instead of a plunge. If this parameter is changed from the default of <N>, then the parameter of Ramp Angle will need to be defined in degrees.
If Ramp-IN is set to <Y>, then this parameter would need to be defined. The parameter will need a numeric value defining the degrees of the ramp such as 30 or 45.
The safety plane is the index plane Z location. If a ' * ' is used as the first character, that position is absolute in world Z coordinates, otherwise it is considered to be the distance above the shape.
This controls the depth per pass in Z. It is also the initial Peck Increment.
This parameter controls the total depth of the cut. If a ' * ' is used as the first character, that position is absolute in world Z coordinates. If it does not, then that distance is considered to be the distance below the initial shape.
Initial feedrate to start the drilling operation.
The RPM value to use for the spindle for this tool path.
Values placed here will be output in the cut cycle before the tool enters the material, typically at the height of the Safety Plane once the tool length compensation is set.
Values placed here will be output in the cut cycle after the tool has retracted from the cut, typically at the height of the Safety Plane after the cut is finished.
A numeric value to use for the tool path created to allow the Sequence to place cuts in a specific order when the code is created.
**Changing values in the cycle parameters may yield unexpected results with some settings or on some geometry. Examine the toolpath and NC Code carefully before running your machine tool if you change these default settings.
