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.
Arc Fit - When this check box is cleared, the posted NC program for this feature is entirely line segments. If the check box is selected, the posted NC program includes arc segments within the entered tolerance of the toolpath entities. This option can greatly reduce the number of lines of the NC program.
Arc Fit Tolerance - The tolerance for the fitting of arcs to the toolpath entities is entered here.
To learn about creating tools for milling features, please view the Milling Tool Pages.
Cut Pattern
Zig - This pattern of cuts causes the tool to remain on the model in one direction, retract to the rapid plane, then rapid from the end of the last cut to the beginning of the next cut.
Zig
Zag - This pattern of cuts causes the tool to feed in both
directions of the pattern.
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 in X and Y.
Allowance XYZ - The distance that the toolpath is calculated above the model. This leaves material remaining for a finish pass without having to offset the model geometry.
Min. Width of Flatlands - Any flat areas with a width smaller than the given value are ignored.
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 treats the surface as
if it is continuous and unbroken.
Depth Options
Top of Job - This 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 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 - Creates a vertical plunge into the material at the start point of the toolpath.
Ramp - This option allows you to make linear ramp moves into the toolpath generated by the system. The ramps are automatically adjusted, based on 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
Vertical - 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.
Right Angle - When this option is selected the system generates the feed move at a right angle to the toolpath.
Circular - When this option is selected the system generates a radial move into the toolpath and the Radius box becomes available.
Length - Used with the Parallel and Right Angle lead options, 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
Same as Lead In - When selected this check box sets the Lead Out to match the Lead In style.
Vertical - 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.
Right Angle - When this option is selected the system generates the lead out at a right angle to 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 box becomes available.
Length - Used with the Parallel and Right Angle lead options, 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.
Point
Tool Tip - The 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 - These options are used to connect one toolpath chain to the next toolpath chain.
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 entity.
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.
Filter
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.