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.
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
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.
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 entry.
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 entry.
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.