Interfacing with the CAM Feature Manager is performed using standard Object Editing techniques.  Right-click on a CAM feature in the CAM Plan Manager tree and select an option from the popup menu.  Each option is discussed on this page.  Additional forms are provided for each feature type.

 

 

 

CAM features are the fundamental geometry used in a CAM plan (e.g., curve, hole, pocket, surface, etc.). A single CAM feature can contain a single feature or a list of homogenous features. The individual features in the list may be different dimensionally.  However, all features in the list must be from the same parent CAM component.  Each CAM Feature Form (see below) provides the tools needed to assemble and manage CAM features of a similar type.

 

CAM features can be added at the Operations Manager level (see Referencing CAM Features in the Operations Manager section).  These features can be shared with multiple operations.  You can also add CAM features (including profiles for containment) at the Feature Manager level in each operation.  Right-click on Features within the Operation and select Add.  These CAM Features only apply to that operation.  See also Edit, Remove and Preview CAM Features in this section.

 

 

 

The creation of CAM features is initiated from the CAM Component Manager.  Right-click on a component in the CAM Plan Manager and select Add Feature from the popup menu.  A list of CAM features will be provided.  Select the feature to create and refer to that feature type on this page.

 

 

 

Use these commands to highlight and unhighlight individual CAM features in the graphics window.  This makes it easy to identify individual features when many features are defined.

 

 

 

After a CAM feature is added to a component (see Add a CAM Feature above), you can use this command to make changes to the feature.  The CAM Feature Form (see below) for that feature will be displayed with the feature list defined.

 

 

 

Use this command to remove a CAM feature from a component.  Only the definition of the CAM feature is removed and not the original part feature.  The feature will be removed from the CAM Plan Manager tree.

 

 

 

 

This function differs from the Highlight function because it's for Features referenced in an operation.  Highlight shows actual geometry as defined/picked for the CAM feature.  Preview shows the sampled profiles/containment geometry in the frame of reference used for an operation.

 

 

 

The following properties and functions are common to each CAM Feature Form. Refer to each form below for additional functions unique to each feature type.

 

Sample CAM Feature Form (Surface)

 

 

CAM Feature Properties

 

Name

The name of the CAM feature defaults to the feature type followed by a numeric sequence (e.g., profile 1, profile 2, profile 3, etc.).  You can use this field to change the name of the feature.

 

Class

This property defines the class of the CAM feature.  For some feature types such as profiles, the default class is set to "General."  For others such as surfaces, the class takes on more significance.  The word "Class" becomes a button that when selected, will display an additional option called "Control Surface (CS)."  This class further identifies the surface feature for special handling when defining certain tool paths.  Refer to each CAM Feature Form below to see if additional classes are available for that feature type.

 

Type

This property defines the CAM feature as being either a part feature or a containment feature.  Part features are used to derive tool paths while containment features are used to contain or limit tool path movement.

 

Component

Identifies the CAM component from which the feature is derived.

 

File

Identifies the VX file from which the CAM component is derived.  These fields cannot be edited.

 

 

CAM Feature Attributes

 

Feature List

The feature list is shown on the left. Select a feature to display its attributes shown on the right.

 

Lift-click selects and highlights a feature from the list.

 

    

Select or highlight a feature from the list and middle or right-click to display a list of functions.  These are the same functions listed under Other Functions below. The function will apply to the selected feature.

 

Attribute List

The attributes for the feature selected from the list on the right are listed on the left.  Refer to each CAM Feature Form below for information about each feature attribute.

 

 

Other Functions

 

Modify Attributes

Use this function to modify the attributes for individual elements of a feature. Here are some examples:

 

• Set attributes of a curve (or a surface) in a pocket different from the entire pocket.

• A face within a solid.

• A curve within profile.

 

1. Select the element of an existing feature (from the graphics window) to modify.

2. Set the attributes for the individual element using the form provided.  The attributes are similar to those of the entire feature. Refer to each CAM Feature Form below for information about each attribute.

3. Pick Accept to set the attributes for the element or Cancel to close the form.

 

Apply Attributes

If you make changes to the attribute values, select this button to apply the new values to the selected feature.

 

Add (feature)

Add a selection of geometry defining a feature to the list of features defining the active feature.

1. You can select the Pick Filter icon to select from the element types supported by the feature.

2. Select the entities from the screen to define the feature and middle-click to continue. All part elements selected will be considered one CAM feature.
   
   The CAM feature identifier (e.g., p#) will be added to the list of features on the left.

 

3. Select the CAM feature identifier from the list on the left to display its attributes on the right (optional).

 

Remove (feature)

Select the feature identifier from the list on the left and then pick the Remove button to delete it.  Only the definition of the CAM feature is deleted and not the original part feature.

 

 

 

Other Options

 

• OK - Create CAM feature set with the specified information.

• Reset - Pick Reset to ensure that the form's contents show the current values for that CAM feature.

• Cancel - Close the form without creating a CAM feature.

 

 

 

Use the form shown below to add CAM surface features to the active CAM component.  Faces, part features or shapes may be selected to define the feature.  Of special note is the Class, CS Type and Position attributes. These further classify the CAM surface feature.  See below for more information.

 

1. Right-click on a component in the CAM Plan Manager tree and select Add Feature.

2. Select Surface from the popup list of CAM features.

3. Select the part entities to define the feature.  The CAM feature identifier (e.g., s#) will be added to the list of features on the left.

4. Select a feature identifier from the list and edit its attributes on the right if desired.

5. Pick OK to add the CAM feature to the manager tree under the selected component.

 

See also CAM Feature Form Commonalities for additional information.

 

 

CAM Surface Feature Properties

 

Class

This property is used to further classify the surface feature set and is recognized by tool path operations.  Most operation definitions except for the 5 axis swarf cut will use the "General Surface" class.  The 5 axis swarf cut and interactive cut operations will use the "Control Surface (CS)" class.

 

• General Surfaces - Use this class for all operation definitions except for the 5 axis swarf cut.  This is a general surface classification.

• Control Surface (CS) - If this class is selected, the CS Type and Position attributes are activated (see below).  These further define the CAM surface class.  For example, you can use a CAM surface feature to represent a pocket that is to be machined.  The feature can have all the wall surfaces of the pocket as drive surfaces and the bottom surfaces of the pocket as part surfaces.  The CS Type needs to be set for each surface set in the feature.

 

 

CAM Surface Feature Attributes

 

Tolerance

This represents a design tolerance that is saved as an attribute of the surface feature.

 

Offset Normal

This represents an offset value normal to the surface for material which is intended to remain on the part after the CAM Operations are completed. This offset is applied to all operations that reference the surface feature. Most operation types provide an additional offset to be applied to the individual operation type.

 

The offset may be dictated by the shape of the part, or used to facilitate the manufacturing of tooling for a part, without copying or modifying the actual part geometry.

 

CS Type

This is used to further classify the CAM surface feature and is recognized by tool path operations.  This option is not available if Class above is set to GeneralSurface. The CS Type needs to be set for each surface set in the feature.  Choose from the following options:

 

• Drive Surface - controls the tool axis.

• Part Surface - controls the tool height.

• Start Check Surface - determines the starting position of the tool path.

• Stop Check Surface - determines the ending position of the tool path.

 

Position

This is used for tool position options relative to the selected surfaces. This option is not available if Class is set to GeneralSurface. Choose from the following options:

 

• To - the tool path moves to the check surfaces.

• Past - tool path moves past the check surfaces.

• On - currently not supported.

• Tangto - the tool path is tangent to the check surfaces.

 

Trim Holes

This specifies whether or not holes trimmed in a surface are to be ignored. Select Ignore or Respect by clicking on the Trim Holes button.

 

Surface Side

This specifies which side of the surface is defined as the part material side. For 3-Axis Milling, all parts are machined on the positive Z side. In most cases the result is obvious. However, when surfaces are vertical or near vertical, it may not be obvious. In this situation, the surface side option allows you to clearly specify your intent.

 

Select Auto, Reverse, or Natural by clicking on the Surface Side label button.

 

• Auto - In cases where there are many surfaces of mixed orientation, the system will determine the part material side.

• Natural - Use the surface or surface set normal vector to determine the part side.

• Reverse - Reverses the natural direction.

 

 

 

Use the form shown below to add CAM solid features to the active CAM component.  Only solids may be selected.  Use this form to select an entire component as a CAM feature.  See below for more information.

 

1. Right-click on a component in the CAM Plan Manager tree and select Add Feature.

2. Select Solid from the popup list of CAM features.

3. Select the part solids to define the feature.  The CAM feature identifier (e.g., s#) will be added to the list of features on the left.

4. Select a feature identifier from the list and edit its attributes on the right if desired.

5. Pick OK to add the CAM feature to the manager tree under the selected component.

 

See also CAM Feature Form Commonalities for additional information.

 

 

CAM Solid Feature Attributes

 

Tolerance

Represents a design tolerance that is saved as an attribute of the solid feature.

 

Offset Normal

Represents an offset value normal to the surface for material which is intended to remain on the part after the CAM Operations are completed. This offset is applied to all operations that reference the surface feature. Most operation types provide an additional offset to be applied to the individual operation type.

 

The offset may be dictated by the shape of the part, or used to facilitate the manufacturing of tooling for a part, without copying or modifying the actual part geometry.

 

Finish

Represents a design finish that is saved as an attribute of the solid feature.

 

Trim Holes

Specifies whether or not holes trimmed in a solid are to be ignored. Select ignore or respect by clicking on the Trim Holes button.

 

 

 

Use the form shown below to add CAM profile features to the active CAM component.  Curves in a CAM profile are projected onto the XY plane of the active frame. An Offset can then be applied and gaps closed using the specified Join Method. If the Close option is specified, a closed region is generated.

 

If necessary, separate regions will be created. A tool path referencing the feature will utilize all regions. It is important to note that tool paths are created from the implicit profile geometry. If the part geometry is modified the CAM profiles must be regenerated to reflect the changes.

Here are some additional considerations:

 

• Curves defined within a single CAM profile are machined together if possible. The attributes assigned to a CAM profile are applicable only for that profile.

• A feature can include any number of CAM profiles. If multiple CAM profiles are defined in the feature they do not need to touch and may or may not be machined as a continuous curve.

• Two CAM profile features can have profiles referencing the same curves but having different attributes. The original curves are not modified in any way by the definition of CAM profiles.

• Each CAM profile added is defined as an open or closed entity.

 

 

 

 

1. Right-click on a component in the CAM Plan Manager tree and select Add Feature.

2. Select Profile from the popup list of CAM features.

3. Select the part entities to define the feature.  Curves and profiles (i.e., a part sketch) are supported.  The CAM feature identifier (e.g., p#) will be added to the list of features on the left.

4. Select a feature identifier from the list and edit its attributes on the right if desired.

5. Pick OK to add the CAM feature to the manager tree under the selected component.
    

See also CAM Feature CAM Feature Form Commonalities for additional information.

 

CAM Profile Feature Attributes

 

Tolerance

Specifies the tolerance used to determine if the profile is closed. This is also used for sampling points along the profile.

 

Offset

Represents the value normal to curves for material which is intended to remain on the part after the CAM operations are completed. This offset is applied for all operations referencing the profile feature. Most operation types provide for an additional offset to apply on an individual operation basis. Offset is applied in the direction opposite the part side. A CAM profile groups curves and adds information to them. The original geometry is not affected nor is new geometry created.
 

Offset may be dictated by the shape of the part, or used to facilitate the manufacturing of tooling for a part, without copying or modifying the actual part geometry.

 

Open / Close

Specifies whether the CAM profile will form an open or closed boundary. Select Open or Close by clicking on the Open / Close button.

 

• Close -Specifies that the CAM profile consists of a closed set of curves or edges ( if the curve set is open, the specified Join Method is used to connect curves and close the profile).

• Open - Specifies that the CAM profile consists of an open set of curves or edges. No attempt is made to resolve gaps between selected entities.

 

Join Method

Specifies how gaps in a CAM profile are to be closed. Select Linear, Circular or Intersect by clicking on the Join Method button.

 

When the curves or edges defining the CAM profile are selected, gaps may exist between the curves. Also, when an offset is applied to the geometry, some of the geometry may separate. The join method determines how these gaps are connected to form a continuous curve.

 

• Circular - Attempts to fit an arc, equal to the radius of the cutting tool, tangentially, to fill the gap. If this fails, then the intersect method is used.

• Intersect - Extends one or both curves if necessary until they intersect. If this method fails, then the linear method is used.

• Linear - Connect the gap with a straight line.

 

Reverse Direction

This option reverses the direction of the profile feature - in effect, it changes the part side from right to left or vice versa.

 

Part Side

This specifies which side of the CAM profile is the part side. Select from the list of options (i,e., Left, Right, Left and on, or Right and on). Left and on and Right and on are used for containment class profiles only.

 

The part side is the side where part material should remain after machining. To determine the part side of a containment profile, highlight the profile in the profile list.  Now face in the direction of the arrow shown on the screen.  Select from the list of options based upon your left or right side.

 

The CAM system uses a counter-clockwise rule to determine the part side for part class profiles. CAM profiles are oriented in a counter-clockwise direction for a closed pocket profile, in a clockwise direction for an island profile, or along the direction of creation for an open profile. Left specifies that the part side of the profile is on the left hand side. Right specifies that the part side is on the right.

 

• A pocket would be defined as part side right.

• An island would be part side left.

 

The system does not require that the geometry be created using a counter-clockwise orientation, nor does it re-orient the geometry.  However, the pick sequence when selecting the curves that define a profile is important.  The rules above should be taken into account.

 

 

 

Use the form shown below to add CAM pocket features to the active CAM component.  Pocket features may be a set of curves, profiles (i.e., a sketch), surfaces or features. Use the Modify Attributes (see CAM Feature Form Commonalities above) to modify the boundary condition for individual elements within the pocket.  See below for more information.

 

 

 

 

1. Right-click on a component in the CAM Plan Manager tree and select Add Feature.

2. Select Pocket from the popup list of CAM features.

3. Select the part entities to define the feature.  The CAM feature identifier (e.g., p#) will be added to the list of features on the left.

4. Select a feature identifier from the list and edit its attributes on the right if desired.

5. Pick OK to add the CAM feature to the manager tree under the selected component.

 

See also CAM Feature Form Commonalities for additional information.

 

 

CAM Pocket Feature Attributes

 

Tolerance

The machining tolerance for the active pocket feature.

 

Offset

Represents the value normal to curves for material which is intended to remain on the part after the CAM operations are completed. This offset is applied for all operations referencing the pocket feature. Most operation types provide for an additional offset to apply on an individual operation basis.

 

Offset is applied in the direction opposite the part side. A CAM pocket groups curves and adds information to them. The original geometry is not affected nor is new geometry created.

 

Offset may be dictated by the shape of the part, or used to facilitate the manufacturing of tooling for a part, without copying or modifying the actual part geometry.

 

Draft

The draft angle per side to be applied to the active pocket feature. If a draft feature is already incorporated into the pocket feature geometry, this field is left blank and the parameter is calculated automatically when tool paths are generated.

 

Depth

The depth to be applied to the active pocket feature. Use this attribute to machine a pocket from a profile of curves. If depth is already incorporated into the pocket feature geometry, this field is left blank and the parameter is calculated automatically when tool paths are generated.

 

 

 

Use the form shown below to add CAM hole features to the active CAM component.  Since CAM hole positions are defined by reference points, circles, cylinders or part hole features, make sure the center points exist in your CAD data. If not, they should be created before defining your hole features. See below for more information.

 

 

 

 

1. Right-click on a component in the CAM Plan Manager tree and select Add Feature.

2. Select Hole from the popup list of CAM features.

3. Complete the Required Inputs (see below).

4. Complete the Optional Inputs if desired (see below)

5. Pick OK and the CAM Hole Feature Form is displayed (see below).

 

Required Inputs

 

• Input Type - Defines the method of input you will use to select the holes.  Point, Circle, Cylinder or Hole are supported.  You can also set the input method using the Pick Filter. Refer to the Optional Inputs section below for options specific to each type.

• Holes - Select the holes to include in the CAM feature.

• Diameter - Specifies the hole diameter when the Input Type above is set to Point.

• Depth - Specifies the hole depth.  Leave this blank for through holes.  This input is removed when the Input Type above is set to Holes or Cylinder (i.e., the feature geometry contains depth definition).

 

Optional Inputs

 

• Hole Axis - If an axis is specified, only those holes with the same axis will be selected. If left blank, all picked holes will be accepted.

• Hole List - This option defines how the selected holes will be grouped.
  
  Individual - List all holes individually.
  Groups - List all holes in groups of the same attributes.  See the Tip box above about grouping similar holes.
  Misc Group - List all holes in a single group (i.e., The Input Type above is set to Holes).
   

• Min Dia/Max Dia - Use these to set the minimum and maximum diameter values for the holes.

• Min Dep/ Max Dep - These two fields will tell VX CAM to only select holes whose depth fall between these depth values. These holes will be shown on the CAM Hole Feature Form (see below).

• Cylinder Type -When Input Type (see above) is set to Cylinder, use this option to detect Closed Cylinders, Open Cylinders or All Cylinders.

• Min Angle/Max Angle -When Input Type (see above) is set to Circle, use this option to detect holes from those arcs with arc angles between the specified minimum and maximum values.

• Tolerance - Hole diameter tolerance.  If the tool diameter differs from the hole diameter by an amount greater than this tolerance, you will get a warning message.

• Finish - Hole surface finish. This is for reference only and is not used when calculating a tool path.

 

See also CAM Feature Form Commonalities for additional information.

 

CAM Hole Feature Form

 

These attributes apply to the holes in the active feature set select from the Holes list on the left.

 

• Diameter - Hole diameter.

• Depth - Hole depth. This field is blank when it is a through-hole. Depth is computed on the fly during tool path computation for through holes.

• Tolerance - Hole diameter tolerance.  If the tool diameter differs from the hole diameter by an amount greater than this tolerance, you will get a warning message.

• Finish - Hole surface finish. This is for reference only and is not used when calculating a tool path.

• Csink Diameter - Countersink diameter.

• Csink Angle - Countersink included angle.

• Cbore Diameter - Counterbore diameter.

• Cbore Depth - Counterbore depth.

• Thread Diameter - Thread diameter for tapped holes.

• Thread Depth - Thread depth for tapped holes.

• Thread Pitch - Thread pitch for tapped holes.

• Hole Axis - This allows you to specify an alternate hole axis.  Otherwise VX CAM will calculate it for you.

 

 

 

Use the form shown below to add CAM slot features to the active CAM component.  Slot features may be a set of curves, profiles (i.e., a sketch), surfaces or part features. Use the Modify Attributes (see CAM Feature Form Commonalities above) to modify the boundary condition for individual elements within the slot feature.  See below for more information.

 

1. Right-click on a component in the CAM Plan Manager tree and select Add Feature.

2. Select Slot from the popup list of CAM features.

3. Select the part entities to define the feature.  The CAM feature identifier (e.g., s#) will be added to the list of features on the left.

4. Select a feature identifier from the list and edit its attributes on the right if desired.

5. Pick OK to add the CAM feature to the manager tree under the selected component.
    

See also CAM Feature Form Commonalities for additional information.

 

 

CAM Slot Feature Attributes

 

Tolerance

The machining tolerance for the active slot feature.

 

Offset

Represents the value normal to curves for material which is intended to remain on the part after the CAM operations are completed. This offset is applied for all operations referencing the slot feature. Most operation types provide for an additional offset to apply on an individual operation basis.

 

Offset is applied in the direction opposite the part side. A CAM slot groups curves and adds information to them. The original geometry is not affected nor is new geometry created.

 

Offset may be dictated by the shape of the part, or used to facilitate the manufacturing of tooling for a part, without copying or modifying the actual part geometry.

 

Draft

The draft angle per side to be applied to the active pocket feature. If a draft feature is already incorporated into the pocket feature geometry, this field is left blank and the parameter is calculated automatically when tool paths are generated.

 

Depth

The depth to be applied to the active pocket feature. Use this attribute to machine a pocket from a profile of curves. If depth is already incorporated into the pocket feature geometry, this field is left blank and the parameter is calculated automatically when tool paths are generated.

 

 

 

Use the form shown below to add CAM step features to the active CAM component.  Step features may be either a set of curves, profiles, surfaces or features.  Use the Modify Attributes (see CAM Feature Form Commonalities above) to modify the boundary condition for individual elements within the step feature.  See below for more information.

 

1. Right-click on a component in the CAM Plan Manager tree and select Add Feature.

2. Select Step from the popup list of CAM features.

3. Select the part entities to define the feature.  The CAM feature identifier (e.g., s#) will be added to the list of features on the left.

4. Select a feature identifier from the list and edit its attributes on the right if desired.

5. Pick OK to add the CAM feature to the manager tree under the selected component.

 

See also CAM Feature Form Commonalities for additional information.

 

 

CAM Step Feature Attributes

 

Tolerance

The machining tolerance for the active step feature.

 

Offset

Represents the value normal to curves for material which is intended to remain on the part after the CAM operations are completed. This offset is applied for all operations referencing the step feature. Most operation types provide for an additional offset to apply on an individual operation basis.

 

Offset is applied in the direction opposite the part side. A CAM step groups curves and adds information to them. The original geometry is not affected nor is new geometry created.

 

Offset may be dictated by the shape of the part, or used to facilitate the manufacturing of tooling for a part, without copying or modifying the actual part geometry.

 

Draft

The draft angle per side to be applied to the active pocket feature. If a draft feature is already incorporated into the pocket feature geometry, this field is left blank and the parameter is calculated automatically when tool paths are generated.

 

Depth

The depth to be applied to the active pocket feature. Use this attribute to machine a pocket from a profile of curves. If depth is already incorporated into the pocket feature geometry, this field is left blank and the parameter is calculated automatically when tool paths are generated.

 

 

 

Use the form shown below to add CAM chamfer features to the active CAM component.  Chamfer features may be either a set of curves, profiles, surfaces or features.  Use the Modify Attributes (see CAM Feature Form Commonalities above) to modify the boundary condition for individual elements within the chamfer feature.  See below for more information.

 

1. Right-click on a component in the CAM Plan Manager tree and select Add Feature.

2. Select Chamfer from the popup list of CAM features.

3. Select the part entities to define the chamfer feature.  Use the Pick Filter to isolate entities as desired.  Curves, profiles, surfaces and features are allowed.  

4. The CAM Chamfer Feature Attributes Form is displayed.  The CAM feature identifier (e.g., s#) will be added to the list of features on the left.  Select a feature identifier from the list and edit its attributes on the right if desired.

5. Pick OK to add the CAM feature to the manager tree under the selected component.

 

See also CAM Feature Form Commonalities for additional information.

 

 

CAM Chamfer Feature Attributes

 

Tolerance

The machining tolerance for the active step feature.

 

Offset Normal

Represents the value normal to curves for material which is intended to remain on the part after the CAM operations are completed. This offset is applied for all operations referencing the step feature. Most operation types provide for an additional offset to apply on an individual operation basis.

 

Offset is applied in the direction opposite the part side. A CAM step groups curves and adds information to them. The original geometry is not affected nor is new geometry created.

 

Offset may be dictated by the shape of the part, or used to facilitate the manufacturing of tooling for a part, without copying or modifying the actual part geometry.

 

Trim Holes

This specifies whether or not holes trimmed in a surface are to be ignored. Select Ignore or Respect by clicking on the Trim Holes button.

 

Surface Side

This specifies which side of the surface is defined as the part material side. For 3-Axis Milling, all parts are machined on the positive Z side. In most cases the result is obvious. However, when surfaces are vertical or near vertical, it may not be obvious. In this situation, the surface side option allows you to clearly specify your intent.

 

Select Auto, Reverse, or Natural by clicking on the Surface Side label button.

 

• Auto - In cases where there are many surfaces of mixed orientation, the system will determine the part material side.

• Natural - Use the surface or surface set normal vector to determine the part side.

• Reverse - Reverses the natural direction.