Rapid Movements
Clearance Plane - The height at which the tool can rapid safely from operation to operation.
Rapid Plane - The height at which the tool can rapid safely within the current machining feature.
Top of Part -
The top of the material for the feature. This value is incremental
from the Machine Setup or machining origin.
Parameters
Use Chamfer - Selecting this check box adds a chamfer operation to the machining feature.
Posting Parameters
Work Offset # - This box allows you to choose which work offset code to use for this feature in the posted NC program. The post processor must be configured to support the work offset selected.
Output Rotary Angle - When selected, the angle entered into the Rotation Angle box is output in the posted NC program.
Rotation Angle - When performing 4th axis indexing, the rotary angle is entered here. This box is unavailable until the Output Rotary Angle check box is selected.
To learn about creating tools for milling features, please view the Milling Tool Pages.
Patterns
Zig Zag - This pattern of parallel cuts causes the tool to feed in both directions of the pattern.
No Profile - When the Zig Zag option is selected, a finish pass with the rough tool is not calculated.
Profile After - When the Zig Zag option is selected, a finish pass with the rough tool is added after the pattern is applied to remove the material from the pocket.
Profile Before - When the Zig Zag option is selected, a finish pass is added before the pattern is applied to remove the material from the pocket.
Offset Pocket In - When this option is selected, the pocket pattern continually offsets the outer shape of the pocket and process the toolpath from the outside in.
Offset
Pocket Out - When this option is selected, the pocket pattern
continually offsets the inner shape of the pocket and process
the toolpath from the inside out.
Cut Direction - These options are only available when Offset Pocket In or Offset Pocket Out is selected.
Climb Mill - When this option is selected the tool travels in a counter clockwise direction along the inside shapes of the model and travels in a clockwise direction along the outside edges of the model.
Conventional
Mill -
When this option is selected the tool travels in a clockwise direction
along the outside edges of the model.
Parameters
Lace Angle - The angular direction that the Zig Zag passes are generated for clearing the pocket.
Cut Width % - This box allows you to specify how much of the tool is used for the distance between passes.
Finish
Side Allowance - This sets the amount of material that remains for finishing on the walls. The material is removed when the finish pass is applied.
Bottom Allowance - This sets the amount of material
that remains for finishing on the floor. The material is removed
when the finish pass is applied.
Depth
Single Step - The depth entered in the Total Depth box is processed in one pass.
Multiple Steps - When this option is selected, the values in the Total Depth and Depth of Cut are used to generate the number of equal cuts used to process the pocketing operation.
Even Depths - When this option is selected the distance that the tool plunges for each step, at any given point, is equal.
Defined Depths - When this option is selected the distance that the tool plunges for each step, at any given point, is less than or equal to the Depth of Cut value.
Total Depth - The depth of the material removed by the pocketing operation.
Depth of Cut - When the Multiple Steps option is selected, this box becomes active. The Depth of Cut is the depth at which each equal pass is processed. This value may be different than entered because the value of the Number of Cuts must be a whole number and the depth of each pass is the Total Depth divided by the Number of Cuts.
Number of Cuts - When the Even Depth option is selected this value is automatically calculated by the system when the Depth of Cut is entered.
Material Entry
Plunge - When this option is selected for the material entry type, the system generates a plunge move at the starting point of the pocket.
Ramp - When this is selected, the Number of Steps box appears to the right of the option buttons. This box allows you to specify how many ramp moves the system generates between each pass. The movement created begins at the material top in the case of the first pass and single pass, or from the depth of the previous pass.
Spiral - This option is available if a start point is specified before editing the pocketing operation. The movement created by this option always begins at the designated material top when using a single depth, or on the first pass when using multiple depths. When the Spiral option is selected, the following option buttons and entry boxes become available.
CW - With this option selected the spiral approach is generated in a clockwise rotation.
CCW - With this option selected, the spiral approach is generated in a counter-clockwise rotation.
Number of Steps - This value indicates the number of loops the system generates for each pass.
Spiral Tolerance - This value sets an interpolation accuracy for the system, which indicates the minimum length of the segments produced in the code generated for the approach.
NOTE: The Ramp and Spiral approach types do not support collision detection or island avoidance. It is suggested that these options be used with caution.
Please see the Milling Tool Pages
Pattern Group
Standard - This option is used to generate a toolpath for cutting the perimeter of one or more contours.
Compensation
System Compensation - With this option On, the system offsets the geometry by the tool radius. With this option Off, it is suggested that you turn on Machine Compensation.
Off - When this option is selected the toolpath is calculated from center line.
Left - The toolpath generated is calculated to the left of the selected contour.
Right - The toolpath generated is calculated to the right of the selected contour.
Machine Compensation - These options only effect the output in the posted code.
Off - When this option is selected, no cutter compensation codes are output in the posted program.
Comp Left (G41) - When this option is selected, the toolpath of the feature represents the center of the cutter. The post processed code includes the command for cutter compensation to the left of the contour.
Comp Right (G42) - When this option is selected, the toolpath of the feature represents the center of the cutter. The post processed code includes the command for cutter compensation to the right of the contour.
Entry
Plunge - The plunge entry style is always used for this feature.
Lead In
Vertical - With this option selected the system generates a plunge feed move into the profile.
Parallel - With this option selected the system generates a linear feed move into the profile.
Right Angle - With this option selected the system generates a linear feed at a right angle to the profile.
Circular - With this option selected the system generates a radial move into the profile and the Radius box appears for input.
Length - Used with the Parallel and Right Angle lead options, this box indicates the distance of travel the system generates before the cutter reaches the defined edge.
Radius
- Used with the Circular
lead option, this box indicates the radius of the approach
into the profile.
Lead Out
Same As Lead In - When this check box is selected, the Lead Out matches the Lead-In settings.
Vertical - With this option selected the system generates a plunge feed move into the profile.
Parallel - With this option selected the system generates a linear feed move into the profile.
Right Angle - With this option selected the system generates a linear feed at a right angle to the profile.
Circular - With this option selected the system generates a radial move into the profile and the Radius box appears for input.
Length - Used with the Parallel and Right Angle Lead options, this box indicates the distance of travel the system generates before the cutter reaches the defined edge.
Radius - Used with the Circular Lead option, this box indicates the radius of the approach into the profile.
Please see the Milling Tool Pages.
Patterns
Standard - This option is used to generate a toolpath for cutting the perimeter of one or more contours.
Compensation
System Compensation - With this option On, the system offsets the geometry by the tool radius. With this option Off, it is recommended that you turn on Machine Compensation.
Off - With this option selected the toolpath is calculated from center line.
Left - The toolpath generated is calculated to the left of the selected contour.
Right - The toolpath generated is calculated to the right of the selected contour.
Machine Compensation - These options only effect the output in the posted code.
Off - When this option is selected, no cutter compensation codes are output in the posted program.
Comp Left (G41) - When this option is selected, the toolpath of the feature represents the center of the cutter. The post processed code will include the command for cutter compensation to the left of the contour.
Comp Right (G42) - When this option is selected, the toolpath of the feature represents the center of the cutter. The post processed code includes the command for cutter compensation to the right of the contour.
Tool Position
Cutter Position - This box specifies a distance away from the center of the toolpath to begin the cut, in order to use a chamfer tool that does not have flutes that extend all the way to the tip.
Depth
Chamfer Depth - With this option selected, the Depth box is available to the right and you are able to specify the chamfer size by its depth.
Chamfer Length - With this option selected, the Length box is available to the right and you are able to specify the chamfer size by its length.
Chamfer Width
- With this option selected, the Width
box is available to the right and you are able to specify the
chamfer size by its width.
Sharp Tool - If the chamfer tool has a sharp point, select this option.
Flat Bottom Tool
- If the chamfer tool has a bottom, select this option and the
Small Diameter box becomes
available.
Depth - Enter the depth of the chamfer here if the Chamfer Depth button is selected.
Length - Enter the length of the chamfer here if the Chamfer Length button is selected.
Width
- Enter the width of the chamfer here if the Chamfer
Width button is selected.
Small Diameter - If Flat Bottom Tool is selected, this box becomes available and you can specify the width of the bottom of the chamfer tool.
Chamfer Angle - Enter the angle of the chamfer here.