The Center Operation Definition Form shown below is typical for the hole making operations. Each operation form contains parameters according to the matrix of operations shown above.

 

Center Operation Definition Form - Cutting Parameters Tab

3-Axis Spiral Cut Operation - Appearance Parameters Tab

 

 

 

Frames, Speeds and Containments

 

• Frame - Alternate coordinate system defined within the setup for this operation.

• Speeds Feeds - The speed/feed values to use for this operation's tool motions. Select from the list of speed/feed objects you have previously defined. You can also pick Create to display the CAM Speed Feed Manager Form to create a new speed/feed object.

 

 

Operation

 

Axial Thickness

Offset added to bottom of hole, this thick will remain after this operation.

 

Axis Type

Sets the number of axes needed for the hole operation. Select 3 Axis to generate 3 or 5 Axis fixed face tool paths.  Select 5 Axis for simultaneous tool paths. The traverse motions between different holes will consist of linear or arc movements.

 

VX automatically calculates hole orientations in spite of their definitions from point, arc, cylinder or hole feature data based on the geometry. Global collision avoidance is automatic.  

 

Boring Diameter

(Boring Operations) The effective diameter of the tool.

 

Collision Check

Analyze all motion between holes for collisions with objects in the current setup. Lift the tool where necessary to avoid collisions (the tool will lift to the height of the interfering geometry plus the approach distance). Select Yes or No.

 

If Yes is selected, gouging and collision checking with the table and clamps as well as local gouging of the hole depths with all geometry will be performed. If No is selected, none of above gouging and collision checking will be performed.  However, collision with geometry in the feature list is always checked and avoided regardless of this parameter value.

 

Cut Order

Order in which holes will be machined. Select from the following:

 

• Pick Order - the order in which the hole features groups are selected in this Tactic and within that list, the order in which they are defined within those feature groups.

• Distance - the shortest path between holes that can be found in reasonable time.

• X Zigzag - sort with priority on the X axis.

• X Oneway - sort with priority on the X axis, choosing holes with lower value of Y first.

• Y Zigzag - sort with priority on the Y axis.

• Y Oneway - sort with priority on the Y axis, choosing holes with lower value of X first.

 

Depth of Cut

The length of the hole measured from the top of the hole. By default, this depth will reference the tool shoulder (not the tip) to ensure the correct diameter down to this depth.

 

Dwell Time

Duration of time to hold the tool at the bottom of the hole in order to complete machining.

 

Max Depth

The maximum depth the tool will advance into the hole before it should be retracted to facilitate chip removal.

 

Min Depth

The minimum depth the tool will advance (plunge) into the hole (see Reduction Factor).

 

Off-Center Distance

(Fine Bore Operation) Distance the tool can be moved off-center to avoid collision between the tool insert and the hole sides. This distance should be less than the effective width of the boring insert. This motion away from the hole axis is 180 degrees away from the "Orient Angle".

 

Orient Angle

(Fine Bore Operation) Orientation angle for the insert on the tool. 0-360 degrees, where 360 is along the X axis. This is used with "Off-Center Dist" to advance the tool into the hole without it interfering with the hole sides.

 

Radial Thickness

Offset added to the sides of the hole. The machined diameter will be the hole diameter minus 2 times this radial thick.

 

Reduction Factor

The factor by which the cutting depth is reduced (see reduction start) new_depth_of_cut = Max_Depth * (1. - Reduction_Factor).

 

Reduction Start

This is a cut number at which to begin using the reduced depth of cut ("new_depth_of_cut" above) if "reduction start" is 5, the first 4 plunges of the tool will be at "Max_Depth" all plunges after that will be at the reduced depth. (assuming the hole is deep enough to require 5 or more plunges to complete).

 

Retract Offset

Cutting will being at this distance above the bottom of the previous cutting motion.

 

Return Level

A drill operation involves several steps. The tool first moves from the initial point to the clear point. It then moves to the control point with a given feed rate and starts the drilling process. The distance from the initial point to the drill control point is defined by the Clear Z parameter in the Setup Manager. Use this parameter to set the return level of the tool to either the Initial Level (G98) or the clear point (G99) (i.e., "R"-Level).

 

R-Level Clear

Distance above the top of the hole from which the cutting motion into the hole will begin.

 

Tap Type

Use this parameter during Tap Drill operations to specify the tap type and use the Dwell Time parameter to set dwell time for cam output.  For Tap Type, select from General, Reverse, Rigid or Reverse Rigid.  If a Tap Type other than General is selected, it will be output to the CL file before the tap cycle statement.  Nothing will be output to the CL file if the Tap Type is set to General.  Dwell time will be output to tap cycle statement.

 

Tool Home Start, Tool Home End

Use these parameters to control the tool's home position. The current home orientation is the Cam Frame's z-axis for 3-axis or 5-axis index. For 5-axis, it is the machine's axis.

 

Tool Depth Reference

This parameter determines which location on the tool should reach the cut depth.  Choose from the following:

 

• Tip - Ensures the tool tip does not go below the cut depth shoulder.

• Shoulder - Ensures that the full diameter is maintained down to the cut depth.

• Spot-Drill - The drill depth is determined by the smaller diameter between the hole and the tool as well as the tool tip angle.

 

 

 

 

This figure illustrates how the Tool Depth Reference is used to achieve spot-drilling.  If the tool diameter is greater than or equal to the hole diameter (A and B), drilling will stop when the hole diameter is achieved.  If the tool diameter is less than the hole diameter (C), drilling will stop when the tool diameter is achieved.

 

 

 

 

 

See Tool Path Analysis and Appearance Options.

 

 

 

• OK - Update the operation definition with the new parameters and automatically updates the last modified date for this operation.

• Reset - Reset the form to the parameters already stored for this operation in the CAM plan. If this is a new operation, the contents of the form will default to values defined in your CAM Configuration files.

• Cancel - Close the form without saving any changes to the operation.

• Calculate -Calculate the tool path using on the current parameters.  You can also right-click on the operation in the CAM Plan Manager and select Calculate.  If a parameter is invalid, the Opdef form stays up and warning is given.  If no tool or feature is defined or if the tool path already exists and it is “Locked,” the parameters are saved, the Opdef form goes down and a warning is given.