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.
Cut Pattern
Standard - When this option is selected machining starts from the outer most loop on the part and progresses inwards.
Center Away - When this option is selected machining starts from the inside and progresses outwards within each region.
Outside to Center - When this option is selected machining starts from the outside and progresses inwards within each region.
Top to Bottom - When this option is selected machining starts at the top slice for all regions.
Bottom
to Top - When this option is selected machining starts
at the floor for all regions.
Cut Direction
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 inside shapes of the model and travels in a counter clockwise direction along the outside edges of the model.
Finish
Stepover - The distance the system generates between each pass.
Allowance
XYZ - The distance that the toolpath is calculated above
the model. This leaves material remaining for a finish pass without
needing to offset the model geometry.
Cut Holes - Instructs BobCAM to extend the toolpath into any holes that exist in the surface.
Ignore Holes - If there are any holes in the selected surfaces, this option instructs BobCAM not to place the toolpath into those holes and treat the surface as if it is continuous and unbroken.
Depth Options
Top of Job - This box indicates the top most location for the toolpath on a model. All toolpaths that would normally be generated above this location in the Z-axis are removed.
Bottom of Job - This box indicates the lowest location for the toolpath on a model. All toolpaths that would normally be generated below this location in the Z-axis are removed.
NOTE: The Bottom of Job and Top of Job values are absolute values. It is important to know where the model is located in the graphics area before setting these values.
Entry
Plunge - This option forces the tool to plunge directly to the start point of the toolpath.
Ramp - This option allows you to make linear ramp moves into the stock. The ramps are automatically adjusted, based on the values entered, so that collision into the model is avoided. When this option is selected the following box becomes available.
Angle of Approach - This indicates the angle generated between the ramp motion and the top of the stock.
Spiral - This option allows you to make a helical entry into the toolpath created by the system. When this option is selected the following boxes become available.
Spiral Radius - This indicates the distance from the center of the spiral to the edge of the spiral, when viewing the ramp from the top.
Angle of Approach - This indicates the angle generated between the ramp motion and the top of the stock.
Lead In - These option are only available for the plunge entry type.
Plunge - When this option is selected the system generates a plunge feed move into the toolpath.
Parallel - When this option is selected the system generates a linear feed move into the toolpath.
Circular - When this option is selected the system generates a radial move into the toolpath and the Radius and Angle boxes become available.
Length - Used with the Parallel Lead option, this indicates the distance of travel the system generates before the cutter reaches the defined edge.
Radius - Used with the Circular Lead option, this indicates the radius of the approach into the toolpath.
Angle
- Used with the Circular
Lead option, this indicates the total sweep of the
arc generated for the circular lead.
Lead Out - These option are only available for the plunge entry type.
Same as Lead In - When this check box is selected, the Lead Out matches the Lead-In settings.
Plunge - When this option is selected the system generates a vertical retract out of the toolpath.
Parallel - When this option is selected the system generates a linear retract out of the toolpath.
Circular - When this option is selected the system generates a radial move away from the toolpath. When this option is selected the Radius and Angle boxes become available.
Length - Used with the Parallel Lead option, this indicates the distance of travel the system generates for moving away from the defined edge.
Radius - Used with the Circular Lead option, this indicates the radius of the departure from the toolpath.
Angle - Used with the Circular Lead option, this indicates the total sweep of the arc generated for the circular lead.
Toolpath Output
Extents - The outer boundary of the part is automatically calculated. The calculated toolpath is then contained inside the outer boundary using the tool tip as the calculation point.
Part Bottom - The outer boundary of the model is calculated from the lowest Z-axis value. The equidistant contours are calculated to include this area.
3D Extents - The outer boundary of the model includes
the bottom edge of the selected surfaces at the outermost extremities.
Point
Tool Tip - This instructs BobCAM to calculate the toolpath from the tool tip.
Tool Center - The instructs BobCAM to calculate the toolpath from the center of the bottom of the tool in the case of a straight cornered end mill, or from the center of the radius on the tool in the case of bull-nose or ball-end mills.
Links
Follow - This transition type follows the contour of the surface being machined.
Direct - This transition type directly connects one pass to the next with a line.
S-Link - This transition type creates a S shaped link between each path in the toolpath tangent to both paths that lie on the surface of the model.
Max Link Gap (% of Tool Diameter) -Tells the system the maximum gap between passes to which it may apply this link type before it must retract the tool. If the distance between the end of one pass and the start of next pass is the same as or smaller than the percentage of the tool entered, the toolpath entities use the selected link type. If the distance between the ends of the passes is greater, the system retracts the tool to clearance before moving to the next toolpath entity. The value entered is a percentage of the tool diameter.