The Spiral Rough Operation Definition Form shown below is typical for the rough milling operations.  Each operation form contains parameters according to the matrix of operations shown above.

 

 

Spiral Rough Operation Definition Form - Cutting Parameters Tab	Spiral Rough Operation Definition Form - More Cutting Parameters Tab
Spiral Rough Operation Definition Form - Lead and Link Parameters Tab	Spiral Rough Operation Definition Form - Appearance Parameters Tab

 

 

 

 

Frames, Speeds and Feeds

 

• 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.

 

 

 

Thicknesses

 

These parameters refer to stock allowances to remain on the part after this operation has been performed.

 

Curve Thickness

Offset added to all curve geometry, may be positive (offset away from part boundaries, or negative (offset toward part boundaries).

 

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.

 

Horizontal Thickness

Rather than applying the thick along the surface normal, this thick is applied in the XY plane only and away from the part surfaces.  It must be >= 0.  Performance note: tool path computation can be significantly faster for rough and sidecut tool paths if "Horiz Thick" and "Vert Thick" are used and "Surface Thick" and the tool's corner radius are zero.

 

Vertical Thickness

This thick is applied along the tool axis (+/- Z).  It has the same effect as translating the tool path up or down by this amount.

 

 

 

Air Access

If set to Yes, the roughing cutter will not touch the stock during the approach/engage motion.  This increases cutter life and improves machining results.

 

Auto Cut Dir

• Yes - set the cutting direction to be parallel to the longest linear boundary element.

• No - cutting direction will be determined by "Cut Dir."

 

Bottom

Z height representing the bottom of the stock.  If left blank, the Bottom will be computed from the geometry being cut.  Pressing the Bottom button brings up a prompt to "Select Point."  The right mouse button will bring up the standard point input menu.

 

Cast Offset

Offset applied normal to the part surfaces which defines the stock to be removed.

 

Corner Loop

Inserts circular moves to turn the tool way from part boundaries.  After the tool reaches the turning point, it reverses , then follows a circular move into the next cut, moves back to the turning point and then proceeds along that next cut.  Select "Yes" or "No."  This option is only available when the Spiral Progress option is set to either Step Inward or Step Outward.

 

Curve Tolerance

Chord height tolerance applied to curves to control the density of tool path points.

 

Cut Dir

Select a cut direction. The right mouse button will bring up the standard direction input options menu. This parameter is only available if Auto Cut Dir is set to "No."

 

Cut Direction (Contour and Contour Cast Rough operations)

• Radial - cuts are created perpendicular to the region's medial curve.

• Parallel - cuts are created parallel to the region's medial curve.

 

Cut Order

• Level First - remove all material at one level (Z depth) before proceeding to the next.

• Region First - remove all material from one boundary region (all depths) before proceeding to the next region.  This is relevant only if there is more than one z level being machined.

 

Cutting Mode

Determines the direction of cut.  Select from the following:

 

• Climb - utilize the tool object's "Cut Dirn" (direction) property.

• Conventional - same as "Climb"

 

Max Depth

Determines the maximum depth between cuts.

 

Ramp Angle

If this value is > 0, the tool will ramp from the current cut depth down to the next.  The path is computed over the cut at that next depth.  Use of ramping motion removes the need for access holes.

 

Plane Cleanup

Indicates plane cleanup.  If set to Yes, VX CAM will automatically clean up tops of all planes.  Various roughing cases, like roughing pockets, user-defined profiles, stocks as well as cam containments are taken into account.

 

Pre-drill Points

Indicates locations where drilling operations will create access holes prior to executing this tool path.  All tool motion at each depth will utilize these access holes as appropriate.  A "Drill" type operation, with subtype "Access Hole" should be defined which indicates this operation as its "Ref Oprn."  Then, after this tool path has been calculated, the locations for the access holes and their depths will be computed automatically.  Select from the following:

 

• None - don't use or compute access hole locations

• Auto - automatically calculate all access holes after calculating the tool path.

• Input Points - you can pre-select the locations where access holes will be created, and the tool path will create motions to begin within those access holes at each cut depth.  The depths of those holes will be calculated automatically. If more access holes are required, they will be calculated automatically.  You are prompted to "Select Points."  The right mouse button brings up the standard point input menu.

 

Side Cleanup

Indicates whether a final cleanup pass should be made on the part boundaries.  If this is "Yes" then there will be two passes along the boundaries.

 

Side Region

Controls the cutting region of the side cut tool paths without requiring you to create a stock or containment.  Select from the following:

 

• All Regions - Default, cuts all regions accessible to the cutter.

• Pockets Only - Limits tool path motion to those regions inside a pocket in the part (the complement of "outside only").

• Outside Only - Limits tool path motion to those regions which are not inside a pocket in the part.

 

Slow Down Angle

Controls the output of slowdown feed rate at the corners which angles are greater than the user specified slowdown angle.

 

Slow Down Distance

Refers to the slowdown motion distance around sharp corners.

 

Spiral Progress

• Step Inward - cuts begin by following the part boundaries, subsequent cuts are each offset by a greater amount determined by the stepover value.  Each offset is connected by a linear move where possible.

• Step Outward - the reverse of "Spiral Inward" with cuts progressing by smaller offsets toward the part boundaries.

• Spiral Inward - cuts begin by following the part boundaries, subsequent cuts are the result of a continuously increasing offset from the part boundaries.

• Spiral Outward - the reverse of "Spiral Inward" with cuts continuously progressing toward the part boundaries.

• Air Access Inward - the roughing cutter will not touch the stock during the approach/engage motion.  This increases cutter life and improves machining results.

 

Step Type

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

Value to use in conjunction with Step Type to control adjacent cuts.

 

Surface Tolerance

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

 

Tool Location

Determines if tool side should touch the part or island curves (tan = outer side of tool, past = inner side of tool) or if the tool center should touch the curves (on).  Note that the ON condition will cause several of the stock offsets to be ignored for those boundary elements.

 

Top

Z height representing the top of the stock.  If left blank, the Top will be computed from the geometry being cut.  Pressing the Top button brings up a prompt to "Select Point."  The right mouse button will bring up the standard point input options menu.

 

Under Cut

If set to "Yes" the entire tool is used for computing a gouge-free path on the part.  If set to "No" then only the bottom of the tool is used.  If the part has a positive (or zero) draft it should not be necessary to select "Yes"; if the part has regions with a negative draft, or a tapered tool is being used then "Yes" should be selected.  Performance note: there is a significant performance difference in most cases when "under cut" is set to "Yes."

 

 

 

Link Parameters

 

• 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.

 

• 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.

 

 

Lead In Lead Out Parameters

 

 

• 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.

• Ramp 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.

 

 

Macros

 

These parameters define engage and retract motions. If not supplied, Auto parameters will be used.

 

• Full Approach - Macro object for the first entry for cutting this operation.

• Partial Approach - Macro object for subsequent entries during this operation.

• Full Retract - Macro object for the final exit from cutting this operation.

• Partial Retract - Macro object for previous exits during this operation.

 

 

 

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.