Material Approach
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 - This check box tells the system whether a chamfer tool is added in the list of operations.
Hole Type
Through - When this option is selected the system treats the hole as a through hole and applies the Length Through Cut parameter.
Blind - When this option is selected the system treats the hole as a blind hole.
Machining Order
Optimized - If this option is selected, BobCAM reorganizes the selected points to try to reduce the tool movement in the resulting NC program.
Pick Order - If this option is selected, BobCAM outputs the points in the program in the order they were selected for the 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.
Operation Parameters
Override Depth - Selecting this check box allows you to override the default calculated depth.
Center Drill Depth - This depth is defined as the positive incremental value starting from the Top Of the Part.
Center Diameter - This is for the diameter of the center drilled hole on the face of the material being drilled.
Center Angle - This is for the inclusive angle of the center drill that is used in this machining operation.
To learn about creating tools for milling features, please view the Milling Tool Pages.
This page indicates the drill that has been automatically selected for the operation based on the selections made in the Feature Parameters page.
Operation Parameters
Effective Depth - This value defines the depth of the hole excluding the drill tip from the Top of Part.
Overall Depth - This is the total depth that the drill reaches including the drill point. This value is output in the posted NC program.
Cycle Type
Single Depth - When this option is selected, the system always outputs a G81.
Peck - When selected the system outputs a G83. Built into the system is a parameter, Drill Step Ratio (in the Cutting Conditions Global and Cutting Conditions Program dialog boxes), that allows the system to automatically apply a peck cycle based on material selected and the depth of the hole. For example, if the value of Drill Step Ratio is set to 300 percent (the default), the system automatically outputs a G81 until the depth of the hole is 3 times the diameter of the drill. When the Drill Step Ratio is met, the system automatically outputs the G83 cycle.
Fast Peck - When selected the system outputs a G73. Built into the system is a parameter, Drill Step Ratio (in the Cutting Conditions Global and Cutting Conditions Program dialog boxes), that allows the system to automatically apply a peck cycle based on material selected and the depth of the hole. For example, if the value of Drill Step Ratio is set to 300 percent (the default), the system automatically outputs a G81 until the depth of the hole is 3 times the diameter of the drill. When the Drill Step Ratio is met, the system automatically outputs the G73 cycle.
Override Auto Peck - Selecting this check box allows you to edit the automatically assigned peck amount.
First Peck Depth - This value defines the first peck depth in the peck cycle.
Peck Depth - This value defines the depth of the peck.
Number of Pecks - This value displays the number of pecks that occur.
To learn about creating tools for milling features, please view the Milling Tool Pages.
This page indicates the chamfer tool that has been automatically selected for the operation based on the selections made in the Feature Parameters page.
Operation Parameters
Chamfer Depth - This determines the depth of the chamfer. The value must be greater than 0 or the operation is not applied.
To learn about creating tools for milling features, please view the Milling Tool Pages.
This page indicates the tap that has been automatically selected for the operation based on the selections made in the Tap Parameters page.
Operation Parameters
Effective Depth - This value defines the depth of the hole excluding the ineffective threads from the Top of Part.
Overall Depth - This is the total depth that the
tap reaches including the ineffective threads from the
Top of Part. This value
is output in the posted NC program.
Cycle Type
Thread Direction
Right Hand - This button instructs BobCAM to use the canned cycle configured in the post processor for a right-hand tap.
Left Hand - This button instructs BobCAM to use the canned cycle configured in the post processor for a left-hand tap.
Thread Type - Select to display a dialog box which allows you to select the type of thread to tap.