QuickMilling Operation Types
Roughing	Finishing	High Speed Finishing
Offset 2D Rough Cut Lace Rough Cut Plunge Rough Cut Pre-Drill Rough Cut	Offset 3D Cut Lace Cut Drive Curve Cut Z Level Cut (Side) Pencil Cut Flow 3D Cut Engrave 2D Cut Bulge Cut	HS Offset 2D Cut HS Lace Cut HS Flowing Cut

 

 

The QM Offset 3D Operation Definition Form shown below is typical for the QuickMilling operations. Each operation form contains parameters according to the matrix of operations shown above.

 

 

QM Offset 3D Operation Definition Form - Cutting Parameters Tab	QM Offset 3D Operation Definition Form - More Cutting Parameters Tab
QM Offset 3D Operation Definition Form - Lead and Link Parameters Tab	QM Offset 3D Operation Definition Form - Limiting Parameters Tab
QM Offset 3D Operation Definition Form - Speed, Feed Parameters Tab	QM Offset 3D Operation Definition Form - Post Parameters Tab
QM Offset 3D Operation Definition Form - Appearance Parameters Tab

 

 

 

Frames

 

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

 

Cutting

 

# of Steps

This specifies the number of steps during the Drive Curve Cut operation.

 

% Bulge

Used by the Bulge Cut operation. With a value of 0 (zero), the number of bulges will be equal to the number of flowing curves along Directrix (drive curve).  With a value of 100, the number of bulges will be ruled by the cusp height. This is similar to generating the pattern using HS Offset 2D or Offset 3D Cut operation.

 

% Finish Distance

This is the distance used for the finishing step. It is measured as a percentage of the Step Size above (or derived step size).  Enter a value between 0 and 100%.

 

For Rough Offset 2d Cut and Rough Lace Cut, this parameter is automatically set to 50.0% when the Cleanup Pass parameter (see below) is enabled and 0.0% when it is disabled.

 

% First Step

This parameter is used to change the cusp height of the first step in the tool path.  It is measured as a percent of the Step Size.  For operations with Add Uniform Cuts enabled (e.g., Lace, HS Lace, Z Level, HS Offset 2D and HS Flowing) the value must be between 60-120% (Default = 80%).  For Pencil and Drive Curve50% and for Offset 3D the range should be 100-120% (Default - 100%).

 

% Max Distance

Used by the Engrave 2D Cut operation.  This refers to the maximum feature distance to be milled.  The remaining distances should be milled by an area clearance (rough) operation.

 

% Offset

Use this parameter to offset the containment. It is measured as a percentage of the active tool diameter.  Set this parameter to 0 (zero) for female parts and > 1 for male parts.

 

% Sensitivity

This tells QuickMilling how sensitive to be when detecting intricate details such as pockets and fillets.

 

% XY Smoothing

Smooth all tool paths based on a percentage of the Step Size.

 

Add Uniform Cuts

If enabled, this parameter will execute an Offset 3D Cut operation in addition to the primary operation. It is designed to remove any remaining material and provide an equal cusp finish. All walls must be tapered at least 3 degrees.

 

Cast Offset

This parameter allows you to enter stock thickness to be considered during tool path calculations.

 

Cleanup Pass

Enable or disable exporting for area clearance (Roughing and Flowing). Area clearance is the process of removing large quantities of material using Z-level cuts.  

 

For Rough Offset 2d Cut and Rough Lace Cut, the % Finish Distance parameter (see above) is automatically set to 50.0% when Cleanup Pass is enabled and 0.0% when disabled.

 

Curve Projection

If enabled, the drive curve will be projected. This is useful for pencil milling.

 

Cut Regions

Pick yes or no to cut the part (pockets/bosses) by regions.

 

Cut Direction

You can specify an angular value (e.g. "45.0", "-45.0") in degrees or pick the button to select edge geometry to define a vector. When a vector is picked, its I,j,k coordinate values (e.g., 1.0000, -1.0000, 0.0000) are displayed in the field next to the button. The right mouse button will bring up the standard direction input options menu.

 

Cut Pattern

Used during the Flowing 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 - flow in a spiral direction between the guide curves.

 

Cut Pattern Guide

Used during the Rough Offset 2D Cut operation, this parameter specifies how the tool path will determine its flow. Select Part, Stock, Both or Longest Part Span.

 

Cutting Mode

This determines the flowing direction of the tool path. Select from the following:

 

• ZigZag - use a ZigZag cutting direction.

• Climb - utilize the tool objects direction property.

• Conventional - same as climb.

• Top to Bottom - flow from the top to the bottom of the part.

• Bottom to Top - flow from the bottom to the top of the part.

 

Cutting Progress

This forces the tool path to flow from the Inside Out or the Outside In.

 

Depth of Bulge

Used by the Bulge Cut operation. It refers to the depth of cut (Step Z value).

 

Directrix Step

Used by the Bulge Cut operation. It refers to the step size along the direction of Directrix (the drive curve).

 

Enable Spiral

This parameter enables continuous spiralization of the toolpath.

 

Enhance Corners

Pick Yes to enhance corners by adding a cut that looks like a chamfer.  The default is No.  Refer to the Tips & Techniques section on this page for cautionary information.

 

Frame

Alternate coordinate system defined within the setup for this operation.  First use the CAM Frame Manager to define alternate frames for the setup.  Then use this parameter to select an alternate frame from the list.

 

Generatrix Step

Used by the Bulge Cut operation. It refers to the step size along the direction of Generatrix (the generator curve).

 

Noise X, Y, Z

Used by the Bulge Cut operation.  It refers to the shift in bulge position in the X,Y and Z directions.  These are separate parameter values.

 

Path Prelink

Pick Yes or No to prelink high speed finishing operations.

 

Path Tolerance

This sets the tolerance for internally converting the part geometry to tessilation (triangulated) geometry.

 

Plunge Pockets

Pick Yes or No to allow the tool to plunge into pockets.

 

Preview Mode

If yes is selected, the pencil trace operation will not be enhanced and thus becomes very fast. The resulting tool path will not be subjected to the Tolerance value.

 

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.

 

Ramp Extent

This refers to the minimum length of a plunge move.

 

Tool Home Point

For Z level cut, this defines the start point for the operation.  Right-click for the standard input options.

 

Spiral Progress

Pick this button to toggle between Inside Out and Outside In to specify how the tool path should flow.

 

Surface Thickness (XY)

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

 

Surface Tolerance

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

 

Synchro Z Level

Use this value to generate the cutting loop at the specified Z level. The cutting at Z level is synchronized to meet this level.  Enter the Z value or pick a point from the graphics window.  You can set sets multiple Z levels to synchronize by selecting multiple points or x,y,z values.  The standard set of point input options are available.

 

Wave Propagation

If this is enabled, the tool path will start collapsing from stock otherwise it will follow the default flowing rules.  This is used in conjunction with Enable Spiral.

 

XY Min Step Size

This specifies the minimum step size.

 

XY or Z Corner Radius

Fillet the cut with this radius using Offset2D.

 

XY or Z Step Type

This sets the type of XY or Z step to use. Select from the following and then enter the value in the Step Size, Cusp Height or % Tool Diameter field below.

 

• Step Size - Linear XY or Z step size value.

• Cusp Height - Step value defined by the cusp height.

• Tool Diameter Percent - Step value defined as a percentage of the tool diameter.

• % Flute Length - Linear Z step size defined as a percentage of the flute length.

 

XY or Z Step Size

XY or Z Cusp Height

% Tool Diameter

Defines the XY or Z step size, cusp height, % tool diameter or % flute length. The name on this button will change depending on the XY or Z Step Type selected above.

 

Z Progress

Pick this button to toggle between Bottom to Top or Top to Bottom to define the Z progress of the tool path.

 

Z Surface Thickness

This provides control over the floor stock to be left on the workpiece.  If it is not defined, it will be the same as the XY Surface Thickness parameter.  This Z Surface Thickness parameter can be a negative value.

 

 

Analysis Accuracy

 

This is the grid step setting used to perform auxiliary, analytical computation inside QuickMilling. Nearly All aspects of tool path calculation (containment, rest milling, AFC, stock processing) are affected by this parameter except the tool path quality (under tolerance behavior).This parameter can dramatically impact running time. Cutting the value in half can easily triple the overall running time without a significant improvement in quality.

Set this value according to part size, quantity of features and the desired accuracy. It is recommended that you do not use a value larger than the Tool Diameter / 10.

 

Refer to the Tips & Techniques section on this page for more information.

 

User Value

Use this field to enter an Analysis Accuracy value directly.  

 

 

 

Path Control

 

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.

 

% Ramp Extent

This refers to the minimum length of a plunge move.  It is measured as a percentage of the Tool Diameter.  Range = is 50 % to 100% of tool diameter. Default value = 80 % of tool diameter.

 

 

Safe Ramp

(Yes or No) This will check Ramp moves to avoid any tool collision (and breakage) with the workpiece.

 

Cutting Mode

This determines the flowing direction of the tool path. Select from the following:

 

• ZigZag - use a ZigZag cutting direction.

• Climb - utilize the tool objects direction property.

• Conventional - same as climb.

• Top to Bottom - flow from the top to the bottom of the part.

• Bottom to Top - flow from the bottom to the top of the part.

 

Cleanup Pass

Enable or disable exporting for area clearance (Roughing and Flowing). Area clearance is the process of removing large quantities of material using Z-level cuts.  

 

For Rough Offset 2d Cut and Rough Lace Cut, the % Finish Distance parameter (see above) is automatically set to 50.0% when Cleanup Pass is enabled and 0.0% when disabled.

 

% Finish Distance

This is the distance used for the finishing step. It is measured as a percentage of the Step Size above (or derived step size).  Enter a value between 0 and 100%.

 

For Rough Offset 2d Cut and Rough Lace Cut, this parameter is automatically set to 50.0% when the Cleanup Pass parameter (see below) is enabled and 0.0% when it is disabled.

 

Cut Regions

Pick yes or no to cut the part (pockets/bosses) by regions.

 

Synchro Z Level

Use this value to generate the cutting loop at the specified Z level. The cutting at Z level is synchronized to meet this level.  Enter the Z value or pick a point from the graphics window.  You can set sets multiple Z levels to synchronize by selecting multiple points or x,y,z values.  The standard set of point input options are available.

 

% XY Smoothing

Smooth all tool paths based on a percentage of the Step Size.

 

 

Uniform Cut Parameters

 

Add Uniform Cuts

If enabled, this parameter will execute an Offset 3D Cut operation in addition to the primary operation. It is designed to remove any remaining material and provide an equal cusp finish. All walls must be tapered at least 3 degrees.  Selecting Yes for this parameter will enable the following parameters as well.

 

XY Step Size

This sets the XY step size for the additional Offset 3D Cut operation.

 

Z Step Size

This sets the Z step size for the additional Offset 3D Cut operation.

 

% First Step

This parameter is used to change the cusp height of the first step in the tool path.  It is measured as a percent of the Step Size (see above).  Refer to the Tips & Techniques section on this page for more information.

 

% Smoothing

Smooth the additional Offset 3D Cut tool path. Enter a value between 0 and 1.  0 = None; 1 = Maxim. This factor is multiplied by the step values above.

 

Cutting Progress

This Forces the tool path to flow from the Inside Out or the Outside In.

 

Advanced Cutting Mode

Use this parameter only when the # of Steps is greater than zero.  Otherwise, the Cutting Mode settings from the Cutting Parameter tab are used.

 

Enhance Corners

Pick Yes to enhance corners by adding a cut that looks like a chamfer.  The default is No. Refer to the Tips & Techniques section on this page for cautionary information.

 

 

Spiralize

 

• Enable Spiral - Select Yes or No to enable spiralization of the tool path.

• Min Curve Count - The minimum number of curves for spiral generation.

• % Aggressivity - This is a factor that determines how aggressive curves are fitted.  A higher value means that curve fitting is more accurate at the cost of increased calculation time.

• Over Mill - Add an extra path at the start and end of the spiral. Select None, Half or All.

• Island Topping- Select Yes or No to enable island topping.  If yes, see % Area below.

• % Area- Minimum island size to be cleaned/topped as a percentage of XY surface area.  Minimum value = 0.5

 

 

Pillow Optics

 

• Enabled - Enable or Disable bulge behavior. All QuickMilling finishing operations can have bulge behavior except for the Bulge Cut operation.

• # of Steps - If this value is 0, the number of steps is determined by the main Step Size parameter (see Cutting Tab above).

• Step Size - The step size along the tool path to perform bulging. This can override the main Step Size parameter (see Cutting Tab above) if set otherwise.

• % Elasticity - If this is set to 1, optimized links will be performed.  Otherwise, splines will be fit with various elasticities to smooth the bulge edge.

• Plunge Distance - This sets the plunge distance.

• Normal Bulging - This enables or disables bulging in the normal direction.

• Noise X, Y and Z - This refers to the shift in bulge position in the X, Y and Z directions. These are separate parameter values.

 

 

 

Link

 

Short Link Type

Straight - The shortest path from the end of one cut to the beginning of the next will track along the part (where its convex) or pass through air where the part is concave.
Step - This lifts the tool the minimum distance to avoid gouging and takes the shortest path through air toward the next cut.
Spline - This creates a spline (smooth) transition (geometrically continuous) from the end of a cut into the next. This can be optimal in terms of time, not distance, because it allows the tool to keep moving at a faster speed.

 

Long Link Type

Straight, Optimized - This is similar to Step above.
Curved, Optimized- This option will add curve optimized long links.
Clearance - This is similar to optimized, but the tool is always lifted to the Clearance Z.
Straight, Elastic Band- This option will add straight elastic band/convex hull links.  This is similar to Straight above.
Curved, Elastic Band- This option will add curved elastic band/convex hull links.
Spline - This move is a moderated spline in 3D, degouged and converted in a convex hull.
Rapid Clearance - This simulates a rapid move while linking with other moves at the clearance plane (Clearance Z). This is similar to a G0 clearance move.
Rapid Optimized -This simulates a rapid move while linking with other moves at optimal Z level.

 

% Short Link Limit - This factor decides if a future link will be short or long. If the distance in XY is larger than this factor multiplied by the XY Step Size, a link is considered to be long.  A smaller distance will be considered a short link.

 

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).

 

Safe 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.

 

Remove Air Cuts (Rough Operations Only) - Pick Yes to relink tool paths after lead in/out motions.

 

% Spline Elasticity- This sets the percent of spline elasticity used for spline link moves only.

 

 

Lead In

 

• Type - This parameter sets the type of lead in. Select from the following:
  
  Horizontal - Lead in horizontally (for Z Level Cuts).
  Vertical - Lead in vertically.
  Normal - Lead in 3-dimensionally.

 

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

• End Angle Type - This allows you to set the lead in end angle to be relative to the tool motion.

• 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.

• After Short Link - If this is set to No (the default), lead motions will only be inserted when there is a long link between the adjacent cuts.

• Open/Closed Spans - Use these parameters to force/apply lead in for "Opened" or "Closed" to cut spans (i.e., a set of cut data at "cut" feed rate after lead in and before lead out) you can force a Lead In.  The Ramp-in Angle and Ramp Height parameters (see below) are used to calculate the Lead In moves.

• Ramp-in Angle/Ramp Height - These define Lead In moves for each cut span in the tool path.  See Open/Closed Spans above for more.

 

 

Lead Out

 

 

• Type - This parameter sets the type of lead out. Select from the following:
  
  Horizontal - Lead out horizontally (for Z Level Cuts).
  Vertical - Lead out vertically.
  Normal - Lead out 3-dimensionally.

 

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

• End Angle Type - This allows you to set the lead out end angle to be relative to the tool motion.

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

• Radius - This sets the lead out radius.

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

• Before Short Link - If this is set to No (the default), lead motions will only be inserted when there is a long link between the adjacent cuts.

 

 

 

XY Limiting

 

XY limiting produces a closed containment that is used before expensive projection is performed.  This can dramatically reduce processing time.  Different kinds of limiting can be mixed and matched to achieve the desired results.

 

• Type - Select the type of XY limiting from the list below.
  
  Simple Box - This tells QuickMilling to use the bounding box of the input "Part" to clip the tool path.  You can apply an offset to this bounding box.
  Silhouettes - This tells QuickMilling to use the silhouette of the input "Part" to clip the tool path.  You can apply an offset to this boundary.
  Containment - You need to select the containment geometry (CAM features of type "contain").  This can be any class of CAM features. However, CAM features of class "profile" (preferably closed) are recommended.
  Silhouettes and Containment - See both above.
  Simple Box and Containment - See both above.

 

• Containment - Displays the Containment Definition Form.  Use it to define containment features and attributes.

• % Offset - Use this parameter to offset the containment measured as a percentage of the active tool diameter.  Set this parameter to 0 (zero) for female parts and > 1 for male parts.

• 3D Offset - Set this parameter to yes if you want the offset to occur in 3D.  Otherwise a 2D offset will occur.

• Limit Lead Moves- Pick Yes or No to limit leading moves to the inside of the XY limiting region.

 

 

Z Limiting

 

Z limiting is applied after the tool path is calculated and does not affect running time. Different kinds of limiting can be mixed and matched to achieve the desired results.

 

• Top, Bottom - This sets the top and bottom z clipping planes. Select a point for each parameter to define the planes. The top and bottom are detected automatically by default (with no value entered).

• Max Cut Depth - Milling will be performed between the Top and the Bottom cutting with this depth value.

• Rough Behavior - Enable this parameter to simulate a roughing behavior (linking at bottom). Otherwise a finishing behavior will be used.

• Ref Shoulder - When set to "Ignore", tool shoulder information will not be exported/considered for tool path calculation.

• Gouge Check -When enabled, VX CAM will try to determine the minimum tool hanging location (from the tip of the tool) to achieve a gouge free tool path. If this height is less than the tool height, a warning Message is issued.  This information along with the tool information is saved with the tool path.  This parameter is only available when the Tool Shoulder parameter is set to Consider.  Otherwise this parameter is disabled.

 

 

3D Limiting

 

3D limiting is applied after the tool path is calculated and does not affect running time. Different kinds of limiting can be mixed and matched to achieve the desired results.  Refer to the Tips & Techniques section on this page for more information.

 

• Reference Tool - A reference tool used to determine which regions could not be cut (using that tool). It is used to determine regions where further machining would be required.

• Ref Shoulder - If set to "Consider", the tool shoulder will be considered during gouge checking.  An accurate stock representation is required.

• Min Rest Height - This parameter sets the minimum height of detected rest material. The default value is 0.1. Refer to the Notes section below for more information.

• Anti Witness - This is a coefficient for fine tuning the rest finishing operations.

• Convert 3D -> 2D - If this parameter is enabled, the projective cycles will be better chained (topological linking can be applied). The drawbacks are potential skating near steep walls.

• Rest Rough - Use this parameter enable (Yes) or disable (No) rest rough analysis.  It only applies when Ref Op (Reference Operation) is defined for any of the QuickMilling finishing operations. Ref Op is located below Parameters in the finishing operations section of the CAM Plan Manager tree.
  
  If enabled, the reference operation is used to simulate the tool paths affect on the stock.  The results of the simulation define the work piece and then a rest finishing operation of the selected type is calculated.  If disabled, a finishing operation of the selected type is calculated.  See also Reference Tools and Operations.
  
  For AFC (Advanced Feed Control), the work piece has rest rough analysis applied to it regardless of Rest Rough being Yes or No as long as a RefOp is defined.
   

• % Anti Fragment- Often times when a tool path is limited (by boundary), the tool path may have jagged ends (i.e., tiny segments with links/leads motions).  This parameter helps to smooth out such cases.  With this option, VX CAM will not discard segments shorter than this distance improving tool path continuity.  This parameter is a % factor of the tool diameter.
   

 

Angular Limiting

 

Refer to the Tips & Techniques section on this page for more information.

 

• Min Angle - This sets the minimum clipping angle (default = 0).

• Max Angle - This sets the maximum clipping angle (default = 90).

• Prev Cut Dir - Mill only regions that tilt between the Min Angle and Max Angle values (see above) but also perform additional analysis to determine and cut any uncut material left over from a previous lace cut operation. The value in this field should equal the Cut Dir value of the previous lace cut operation. If a previous lace cut operation is not present or is not required, this field should be left blank.

• % Antiskate Offset - This value is used to offset limiting curves with a safe distance. This avoids potential skating near steep walls due grid inaccuracies.

 

 

Checks

 

Use these parameters for additional gouge checking.

 

• Tables - Set Consider to Yes to enable table checking and then enter a safe distance.

• Clamps - Set Consider to Yes to enable clamp checking and then enter a safe distance.  You can also specify the mill region to Inside or Outside of the clamps.

• Shank Collision - Set Check to Yes to enable Shank Collision checking.  Then specify the % Step and % Smooth values.

• Shoulder Collision - Set Check to Yes to enable Shoulder Collision checking.

 

 

Filtering

 

Use these parameters to filter out very short tool path segments.

 

• % Area - Remove regions smaller than XY Tool Area times %value [0%-100%]

• % Extents - Remove regions smaller than XY Extents times %value [0%-100%]

 

 

 

Speeds, Feeds

 

Speeds, Feeds

This refers to 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 theCAM Speed Feed Manager Formto create a new speed/feed object.

 

 

Advanced Feed Control (AFC)

 

• Enable AFC - Enable or disable Advanced Feed Control (AFC) for the active QuickMilling operation during output.  Set this parameter to Yes to enable the following AFC parameters.

• Short Span Distance - The value used to remove small spans with higher feed between long spans. A larger value will make milling process smoother and slower.

• Frontal Factor - A more rigid tool, with more flutes, has this coefficient higher.

• Radial Factor - A more rigid tool, with more flutes, has this coefficient lower.

• Min Feed Rate - Minimum feed rate per minute.

• Max Feed Rate - Maximum feed rate as a % of minimum feed rate.

• % Tool Height Load - Tool loading as a % of tool height.
  
   

 

Enable Arcs

 

Use these to enable arcs during post processing.

 

Enable Arcs

 

• XY - Enable arc interpolation in XY plane.

• YZ - Enable arc interpolation in YZ plane.

• XZ - Enable arc interpolation in XZ plane.

• Link - Enable arc interpolation for rapid moves.

• Minimum, Maximum Radius- Use this parameter to specify the minimum and maximum radius permitted for tool path arc fitting.

 

 

Path Filters

 

Use these to filter out very short tool path segments.

 

• %Area - Remove regions smaller than XY Tool Area times %value [0%-100%]

• % Extents - Remove regions smaller than XY Extents times %value [0%-100%]

 

 

Pause/Break

 

Use these to pause or break the tool path.

 

• Break Type
  None - Do not break the tool paths
  Time - Break tool paths after the Time Value in seconds has elapsed.
  Length - Break tool paths after the Length Value in millimeters has elapsed.

 

• Retract Type - Set the retract type to Relative or Absolute.

• Retract Distance - The Relative or Absolute distance used to retract.

• Motion Type - Should the tool retract as a Rapid Move or a Feed Move.

• Plunge Distance - The length in Z used to plunge with feed motion.

• Wait Time - The number of seconds to wait retracted.

 

 

Other

 

• Min Tool Length - Analyze the minimum tool length of the active tool to avoid gouging the part.

 

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.