The 5 Axis Plane Cut Operation Definition Form shown below is typical for the 5 axis milling operations.  Each operation form contains parameters according to the matrix of operations shown above.

 

 

5 Axis Plane Cut Operation Definition Form - Cutting Parameters Tab	5 Axis Plane Cut Operation Definition Form - More Cutting Parameters Tab
QM Offset 3D Operation Definition Form - Lead and Link Parameters Tab	QM Offset 3D Operation Definition Form - 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.

 

Containment

Displays the Containment Definition Form.  The value selected in the "Type" input field of the Containment Definition Form is also shown here.

 

 

Cutting

 

Axis Control

Provides controls over the tool axis. Select from the following:

 

• Fixed Axis - The tool axis will be determined by lead and roll angles along the cutting direction and relative to the z axis of the frame.

• Tip Control - The local contact data determines the cutter orientation while the cutter tip point is kept within the cutting plane.

• Contact Control - The local contact data determines both the cutter orientation and tip point.

• 4-Axis tip Control - This is four axis machining combined with the Tip Control option above.

• 4-Axis Contact Control - This is four axis machining combined with the 4-Axis Tip Control option above.

• Contact Sidecut - The cutter side is tangent with the part tangent plane.

• User Defined - When this option is selected, the tool orientation including its axis and tip will be determined solely by the driving curves and the selected axis directions. All other options of axis control accept users' axis directions but the tool tip points will be calculated based on local part geometry along the driving curves.

 

Axis Option

Use these options to control the tool axis. Select from the following:

 

• Ruled Lines - the tool axis always follows the ruling direction of a drive surface for ruled surfaces.

• Vertical - the tool axis is both tangent to the drive surface and vertically tilted.

• Automatic - the tool axis follows "ruled lines" for curved ruled drive surfaces and will be vertical for other types of drive surfaces including flat ones.

 

Axis Directions

This parameter allows you to specify the tool axis along each driving curve.  To Input axis directions, right click the mouse. Four options will then pop up as On curve, On face, Curve normal, and Face normal. For On curve or On face, an axis direction can only be selected with its origin is exactly on a curve or on a face.

 

Base Thickness

This is a thickness value to be applied to the part surfaces.

 

Collision Check

If set to Yes, VX CAM will automatically check to see if the tool and its holder collide with any part of the setup.  If set to No, only local gouging with the part is checked.  If a collision is detected, the tool will be retracted and a warning message will be displayed suggesting a correction in tool length.

 

Control Point

This parameter is used to machine pockets. If defined, the control point overwrites the Axis Control parameter so that the tool axis passes through the control point.

 

Corner Radius

Fillet the cut with this radius.

 

Cut Depth

(Optional) Limits the depth the tool will overlap the drive surfaces.  If no value is specified, the tool path will make one pass and the base of the tool will contact the part surfaces.  If there is a value less that this depth of overlap, multiple passes will be made as the tool cuts closer to the part surfaces.  Each pass should not be more than this depth closer to the part (base) surfaces than the previous pass.

 

Cut Dir

Select the cut direction.  The right mouse button (RMB) will bring up the standard direction input options menu.

 

Cut Overlap

This is a re-cut distance to obtain smooth part surface when cutting closed loops.  This distance is added at the end of the cut (retracting the beginning of the cut) at the "cut" feed rate.

 

Cutting Mode

This determines the direction of cut. Select from the following:

 

• Climb - utilize the tool object's "Cut Dir" property.

• Conventional - same as "Climb"

 

Cutting Regions

This parameter determines what regions are to be machined.  Select from Pockets Only, Outside Only or All Regions.  If Outside Only is selected, then the Control Point parameter (see above) is disabled.

 

Cutting Order

This is used to compute tool path motions. Select from the following:

 

• Automatic - let vx determine the cutting order.

• Pick Order - compute the tool paths along the pick order of the elements.

• Distance - try to minimize the length of the cutting motion.

 

Cutting/Flow Pattern

This determines if the resulting tool path will proceed in only one direction (along the Cut Plane Angle) or if every other cut will have its direction reversed.  In the first case, there will necessarily be a tool lift between adjacent cuts, in the second case the tool is cutting as it moves in both directions across the part.

 

• Zigzag - every other cut will have its direction reversed.

• One Way - the resulting tool path will proceed in only one direction (along the Cut Plane Angle).

 

Fan In

A distance from a corner seam (edge) at which the tool will begin to lessen the influence of the drive surfaces on the tool axis so that it can assume the optimal orientation on the corner.

 

Fan Out

A distance the tool may traverse while transitioning from the optimal orientation in a corner to having the tool axis controlled by a drive surface.

 

Four Axis Plane

This option allows you to specify the tool axis plane normal for corresponding four-axis machining.  Right-click options are available for specifying the plane normal direction.

 

Flow Type

Used during the Flow Cut operation, this parameter specifies the tool path cut pattern. Select from the following:

 

• Along - flow in a direction along the guide curves.

• Across - flow in a direction across the guide curves.

• Spiral In - flow in an inward spiral direction between the guide curves.

• Spiral Out - flow in an outward spiral direction between the guide curves.

 

Iso Direction

For 5 Axis Guide Surface Iso Cut operations, use this parameter to specify the U or V iso direction.  Select either U-isolines or V-isolines.

 

Lead Angle

The angle the tool will be tilted in the forward motion direction.

 

Max Rotate Angle

This determines the maximum axis change for each tool motion.

 

Max Tilt Angle

This parameter limits tool axis tilting from the positive z-axis of the setup, or the selected frame. If it is empty, there is no limit of tilting.  For swarfcut, if Axis Option (see below) is set to "Automatic" and the tool axis reaches the tilt limits, the tool axis will be forced vertical.  For the remaining Axis Options, the tool axis will be tilted to this Max Tilt Angle.

 

Number of Cuts

This sets the number of cuts at each cutting layer.

 

Project Dir

This direction is used to calculate the driving curves on part surfaces.  Pick reference geometry from the graphics window to define the direction (e.g., edge or curve).  You can right-click to select from the standard directional input options. If this parameter is not defined, the shortest distance to the part surfaces will be used.

 

Roll Angle

The angle the tool will be tilted perpendicular to the forward motion direction.  A positive value will tilt the tool to the right, negative to the left.

 

Side Thickness

This is a thickness value to be applied for this operation on the drive and check surfaces.

 

Skew Angle

This specifies the angle between the side of the tool and the drive surfaces.

 

Start Axis

This is the starting orientation for the tool axis. If not specified, 0., 0. 1. (the current Frame's Z axis) is assumed.

 

Start Point

Used to specify a starting point off of the part from which the tool tip will proceed on first entry into the material. (Otherwise 0., 0., Clear Z is assumed.)

 

Step Over

This parameter is only active when Cutting Pattern (see above) is set to zigzag.  It specifies the connection type between adjacent cuts.  Select from the following options:

 

• Direct - a linear connection is added between adjacent cuts.

• Round - a tangent arc-linear connection is added between adjacent cuts.

 

Step Type

This is the spacing of adjacent cuts when more than one cut is indicated by "no. of cuts."  Select from the following:

 

• Diam Percent - compute spacing from this percentage and the tool diameter.

• Center Dist - distance between tool center point along adjacent cuts.

• Contact Dist - distance between tool contact points on the part surface. In the case of Rough tool paths, this is equivalent to "Center Dist".

• Scallop Height - the spacing between adjacent cuts is computed from the tool shape and this scallop height value.  In the case of 2- ½ axis tool motion, this is computed in the X Y cutting plane and the cut spacing is constant.

 

Step Value

Use this value in conjunction with step type to control adjacent cuts.

 

Surface Thickness

Offset added to all surface geometry, may be positive (offset away from part surfaces, or negative (offset toward part surfaces).  If negative, the magnitude may not exceed the positive thick (optionally) specified for a given surface in a CAM feature plus the tool's corner radius.

 

Tolerance

Chord height tolerance applied to curves and surface/solid geometry to control the density of tool path points.

 

Tool Home Point

This defines the start and end point for this tool path operation.  Right-click the mouse for the standard point input options menu.

 

Tool Side (Drive Curve Cut)

For this parameter, select include on, left and right from the driving curves.

 

• On - The curve offset defined in any profile feature will be ignored.

• Left, Right - The cutting tool follows the corresponding left (or right) side of each driving curve when looking down from the z-axis. The left or right offset equals the sum of the curve offset of the profile feature and the tool radius.

 

Trim Holes

This specifies whether or not holes trimmed in a surface are to be ignored.  This parameter is similar to the same parameter used in Surface Feature Sets.  However, this setting takes precedence, it does not require Features to be defined and it can be applied to all components being machined.

 

• Respect - holes trimmed in surfaces will not be ignored.

• Ignore - will treat round holes in the part as if they are not there and the adjacent surfaces are not trimmed at those locations.

 

Under Cut

If is set to "Yes", VX CAM will automatically orient the cutter axis so that the cutter can reach any "Under" area.

 

 

 

Base Depths

 

Depth Direction

This field specifies the direction in which cutting levels are defined. Select a direction.  It can be a datum axis, plane axis, curve tangent, curve normal, face normal or a centerline.  Right-click to select the input option or your choice.  The depth regions are managed by the Cut Depth, Top and Bottom parameters (see below).  

 

Cut Depth Type

 

• Z-level - cut depth is measure in z-axis direction.

• Along tool axis - cut depth is measure in tool axis direction.

 

Cut Depth

This is the maximum depth of each cutting layer.

 

Top

If this value is higher than the highest tool path point computed from the part geometry, it has no effect. If it is lower than that highest point, the tool motions above that depth are discarded and each cut will be lengthened to the part boundary. The points added will be at the depth of the lowest tool path point computed.

 

• Enter a z value, an absolute coordinate value (x,y,z) or select a point from the graphics window. Point input options are available by right-clicking the mouse.

 

Bottom

If this value is less than the lowest tool path point, each cut will be lengthened to the part boundary. The points added will be at this "Bottom" depth.

 

• Enter a z value, an absolute coordinate value (x,y,z) or select a point from the graphics window. Point input options are available by right-clicking the mouse.

 

Side Thickness (Swarf Cut Only)

This is the remaining material from previous operations or from the original stock. This parameter is used for interference checking. This value can be determined from a roughing or semi-finishing operation.

 

Spiral Down (Side Cut)

Use this parameter to enable spiral progress for the current Side Cut operation.

 

End Over Mill (Side Cut)

If Spiral Down (see above) is set to "Yes" then this parameter allows you to enable or disable end over-milling.

 

 

Side Depths

 

Use these parameters to cut the base (part) surfaces with 5x finish and roughing options.  The parameters allow you to machine drive surfaces in side depths and part surfaces in base depths with either side cut first on each level or base cut first for each side cut.

 

• Side Cast Offset - Defines the material offset to be machined on side or drive surfaces.

• Side Cut Depth - Defines the cut depth for each side cut.

• Side Cut Pattern - Define the cutting pattern of all side cuts on each cutting level.
  
  One Way - All side cuts will follow the cutting mode of either climb or conventional.
  Zigzag - Only the last side cut on each level follows the specified cutting mode. The rest of the sidecut will cut material in the zigzag pattern.
   

• Depth Cut Order - This determines the depth cut order.
  
  Base First - Cut down to base (part) surfaces first for each side cut.
  Side First - Cut sides first on each level.

   

 

 

Link

 

• Short/Long Link Type
  
  Tool path links can be classified as long or short using the % Short Link Limit parameter whose value is a percentage of the tool end diameter. Each path link has the following options.
  
  Automatic - The system calculates the path link in motions of the linear-arc-linear style.
  Z Lift Up - The tool lifts up along the Z-axis so that it traverses above the top of the part by at least the Safe Distance parameter.
  Straight - The tool moves directly from the end of the current cut path to the start of the next cut path while in cutting mode.
  Clearance - The tool lifts up a distance defined by Clear Z (see CAM Frame Manager before traversing to the next cut.
   

• % Short Link Limit-Tool path links can be classified as long or short using this parameter whose value is a percentage of the tool end diameter.

 

• Max Rotate Angle - This angle limits the axis rotational angle of each traversal movement.

 

• Smooth Distance - This parameter, if set greater than 0 (zero) will set the global joining and smoothing distance. This value cannot be larger than 2 * tool corner radius. The default value is 0 (zero).

 

• Save Distance - This value is added to the clearance that is automatically detected to avoid hitting stock. This distance is applied after cutting and before linking/re-linking moves. You can specify a minimum safe distance to avoid any collisions.  Based on part geometry, it will determine the length of moves before linking the tool path for next cut.

 

• Max Plunge Length - This is a maximum distance for a plunge before the start of the actual cut.  It is a plunge move added before each lead In for safer tool engagement.  If this is left blank, it will default to the Safe Distance value above.   

 

 

Lead In

 

• Type - This parameter sets the type of lead in. Select from the following:
  
  None - Lead in  is simply punching down and lead out is simply retracting in the direction of tool axis.
  Arc-Linear Ramp - Lead-in or out motion is in the form of an arc, linear or arc-linear. If Ramp Angle (see below) is set to zero, the motion lies in the xy-plane. The ramp angle is measured from xy-plane.
  Normal - Lead-in or out motion is in the form of an arc, linear or arc-linear, which lies in the plane normal to the tangent plane of the machining surfaces.
  Tool Axis Plane - Lead-in or out motion is in the form of an arc, linear or arc-linear, which lies in the plane of the tool axis direction and tool path tangent direction.

•  

• Start Angle - This sets the lead in start angle in degrees.

• End Angle - This sets the lead in end angle in degrees.

• Radius - This sets the lead in radius.

• Linear Length - This specifies the length of a line which will form part of the Lead motion. For Lead In the order is first Line then Arc.

• Ramp Angle - This is only used when the lead in or out type (see above) is set to Arc-Linear Ramp.  It is measured from xy-plane.

 

 

Lead Out

 

 

These parameters are the same as the Lead In parameters above but are applied to lead out motions.

 

 

 

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.