1. In the CAM Plan Manager, right-click on Operations, select Insert and then select the 5 axis milling operation from the form provided.  The operation will be added to the manager tree.
    

2. Select Parameters under the operation you just added and set the parameters using the definition form provided.  Pick Accept when you are done.  Each 5 axis operation uses a unique definition form.  They are shown on this page under each operation type.  See 5 Axis Milling Operation Form Parameters for a definition of each parameter.
   
   Notice that (undefined) is shown next to Features under the 5 axis operation you just added.  This means that no features are yet defined for the operation.

 

3. Your CAM features (once you define them) are listed under the Geometry section of the manager tree.  Under Geometry, find the CAM component (i.e., part : name) and expand it (i.e., select to the left of the part) to list the CAM features currently defined for that component and select one.  It will now be listed under Features for the 5 axis operation you just created. The (undefined) flag will be removed.  
   
   To create a new CAM feature: Again, under Geometry right-click on the CAM component, select Add Feature and follow the forms and prompts.  You will be prompted to select geometry from the graphics window.

 

 

 

Control surfaces are CAM surface features whose Class property is set to Control Surface (CS) and the CS Type attribute is set to Drive Surface, Part Surface, Start Check Surface or Stop Check Surface.  These attributes are automatically recognized by VX CAM when the CAM surface features are applied to operations.  

 

For example, the swarf cut operation can use control surfaces to drive the tool axis while the interactive cut operation can use groups of part, check and drive surfaces to create a sequence of tool motions.  Refer to each operation type below to find out how to apply control surfaces.

 

1. In the CAM Plan Manager, expand the Geometry section of the tree and locate the CAM component (i.e., part : name) that contains the surfaces you want to define.
    

2. From the manager tree, right-click on the component, select Add Feature and then select Surface from the list.
    

3. The component will be displayed in the graphics window.  Select the surfaces and then middle-click to display the Surface Feature Form.
    

4. Pick Class and then select Control Surface (CS) from the pop-up list.
    

5. In the attributes section of the Surface Feature Form, pick CS Type and then select from the list of Control Surface attributes.  Drive Surface, Part Surface, Start Check Surface and Stop Check Surface are supported.  See CAM Surface Features for more about Control Surfaces.
    

6. Pick Position and then select a tool position option from the list.
    

7. Complete the reminder of the form as desired to create the CAM surface feature.  The Control Surface attributes are defined within the CAM feature.
    

8. Refer to each operation type below to find out how to apply the Control Surfaces to individual tool path operations.

 

 Notes

 

• If a Control Surface feature contains drive and part surfaces, the part surfaces within the feature belong only to the local drive surfaces.  If a Control Surface feature contains only part surfaces, the part surfaces are shared by all drive surfaces in different cam features.

 

 

 

The swarf cut operation will automatically recognize any Control Surfaces that are present within the CAM surface features.  See How to define 5 axis milling operations above to find out how CAM surface features are used with all 5 axis operations.

 

The Cam Feature list in the operation can contain any number of CAM control surface features. Within each CAM feature, there are four types of control surfaces including drive surfaces, part surface, start check surface and stop check surfaces. All drive surfaces in a single CAM feature must consist of only one path. See How to Define Control Surfaces above for more information.

 

For example, to machine a 3D pocket, the CAM feature can be created by selecting all the surfaces of the pocket wall as drive surfaces and the surfaces of the pocket bottom as part surfaces.

 

• If the original part from which the Control Surfaces are selected resides in the CAM assembly, it will be used for gouge-checking during swarf cut operations. Tables and clamps are automatically considered.

 

1. Follow the steps above in How to Define Control Surfaces.  

2. Follow the steps above in How to Define 5 Axis Milling Operations and select the CAM surface feature that contains the Control Surfaces you defined.

 

 

 

 

Control Surfaces are applied on-the-fly using two additional forms when the interactive cut operation is calculated.  These forms are the Interactive Path Calculation Form and the Swarf Cut Surface Selection Form.  Both are documented below.  Using these forms, multiple swarf cut tool motions can be defined, each with differing Control Surfaces.

 

 

 

The 5 axis plane cut creates a cutting pattern based on parallel cuts at a user specified angle with respect to the frame's X axis. This cutting pattern can be used to control the tool tip or the contact location of the tool on the part. It is possible to constrain the tool axis to a plane (for 4 axis milling) or to a specific orientation (for 3 axis milling).

 

This operation supports z-level roughing, round or direct zigzag linking, trimmed hole considerations (ignore/respect) and CAM containments. Control surfaces (see above) are not supported in this operation.  The Class attribute of any CAM surface features for this operation should be set to "General surface."

 

 

 

The 5 axis Swarf Cut operation uses Control surfaces (see above) to calculate the tool path.  The tool axis is controlled by drive surfaces with which the side of the tool maintains contact. The bottom of the tool (contact point) is controlled by part surfaces.  Drive and Partsurfaces are class attributes applied to CAM surface features.

 

Swarf Cut requires that part surfaces be selected in the same surface feature as the drive surfaces.  A CAM feature that only contains part surfaces will be ignored and a warning message is displayed.  You can use this cut as a reference operation for the 5 axis Flow Cut operation.

 

 

 

 

The 5 axis Drive Curve Cut uses 3D driving curves to calculate the tool path. The cutter is driven along these curves and respects the surface geometry to be cut. This operation shares the same Axis Control capability as the 5 Axis Plane Cut operation. The remaining parameters are also similar.

 

 

Notes

 

• The 5 axis Drive Curve Cut accepts a reference operation that can be used as driving curves in addition to the CAM profiles.
   

• If Ref Op is selected, field "Project Dir" should be specified for drive cut to follow exactly the existing path of the referenced operation.  If the field is left as blank, the shortest distance rule is used to find the driving path on the part.
   

• Unique to the Drive Curve Cut is the Project Dir parameter. It is used to calculate the driving curves on part surfaces. If this parameter is not defined, the shortest distance will be used. Features for this operation will include a CAM Profile feature for the driving curves and surface or solid features for the part surfaces.  You can use this cut as a reference operation for the 5 axis Flow Cut operation.
   

• If there are only profiles selected in its feature list, a 5x drive curve operation will cut the 3d curves defining the profiles directly. The tool axis will be determined by the lead and roll angle relative to the reverse of the projecting direction along the driving curve tangent direction.

 

 

 

The interactive cut operation provides additional flexibility by allowing you to create a sequence of 5 axis swarf cut tool motions by specifying groups of part, check and drive surfaces.  You will notice that the definition form shown below is similar to that of the swarf cut shown above.

 

 

Sample Interactive Cut Operation Containing Multiple Tool Motions using Control Surfaces

 

 

 

The 5 axis Flow Cut operation requires either a 5 axis Swarfcut or a 5 axis Drive Curve Cut as a reference operation that contains two separated cuts.  These two cuts will be used as flowing curves. The Swarfcut or Drive Curve Cut can also have multiple depths. VX CAM will select the two bottom cuts as flowing curves.

 

It also enables the Start Point of the Flow Cut operation. The Flow Cut path is generated by interpolation between these two flowing curves.  This operation is very useful for machining areas between two tilted walls (turbine blades for example).

 

Four flowing types are available and include Along, Across, Spiral In and Spiral Out.  The path pattern can be either Zigzag or One Way.  Supported CAM features include the part or surfaces to be machined. Currently, CAM profiles features cannot be used as flowing curves.

 

 

 

Each 5 axis Guide Surface Iso Cut operation must have drive surface(s) selected in its feature list with general surfaces input as the cutting target. The guide surface defined by a drive surface forces tool axis to follow its normals along the isolines. If the field "Cut Drive Surface" is toggled as "Yes", the drive surfaces will serve as the cutting target in addition to other general surfaces in the feature list. If "No", the drive surfaces will be ignored. The cutting pattern consists of two options: "one way" and "zigzag". The iso direction will be either U-isolines or V-isolines. Conventional or climbing.

 

 

 

The 5 axis Side Cut operation accepts parts or general surface features as geometric inputs. Based upon different axis control options, it allows you to position the cutter in various orientations including normal or side tangent to the part with lead, roll and skew angles.  This operation is a good choice for turbine top machining or complex pocket finishing with point control.

 

 

 

When the interactive cut is calculated, this form is displayed first.  It allows you to define multiple tool paths within the operation.  Continuing cuts will be connected automatically.  The Browse icons are used to cycle through the tool motions you create.

 

 

• Class -Currently only 5-axis is available.

• Type - Currently only swarf cut available.

• New - This creates a new tool path within the interactive cut operation and displays the Swarf Cut Surface Selection Form (see below).  This form is used to apply Control Surfaces and other swarf cut parameters to the tool path.

• Edit - This recalculates only the active tool path.  When you change any of the interactive cut parameters, use the Browse icons to locate a tool path and then press this button to recalculate it.

• Regen - This recalculates all tool paths you have currently defined for the interactive cut operation.

• Delete - This deletes the active tool path.  Use the Browse icons to locate a tool path and then press this button to delete it.

 

 

 

This form is displayed when the New button of the Interactive Path Calculation Form (see above) is picked.  It is used to apply Control Surfaces and other swarf cut parameters to a new tool motion within the interactive cut operation.  See also How to define Control surfaces and How to apply Control surfaces to swarf cut operations above.

 

 

 

Drive Loop

The drive surfaces list (see below) must be connected. If the whole list you selected forms a closed wall (for example), set this option to closed. The resulting tool path will also be closed. Otherwise, leave this option as open.

 

Cut Overlap

This is the recut distance to obtain smooth finishing when cutting closed loops. This distance is added at the end of the cut (retracing the beginning of the cut) at the "cut" feed rate.  This parameter also appears on the swarf cut operation definition form.

 

Axis Option

Used to control the tool axis. This parameter also appears on the swarf cut operation definition form.  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.

 

Control Surfaces

These are properties used to classify surfaces for use with the swarf cut tool motion within the interactive cut operation.  Collectively they are referred to as Control Surfaces.

 

Select a button and then select the part surfaces to apply the attributes to.  Middle-click to complete the selection and a system generated name will appear in the field to the right.

 

If you select the button again, a form similar to the CAM Surface Feature Form will be displayed allowing you to modify other attributes and add additional surface sets.  Select from the following buttons:

 

• Drive Surfaces - These control the tool axis.

• Part Surfaces - These control the tool height.

• Start Check Surfaces - These determine the starting position of the tool path.

• Stop Check Surfaces - These determine the ending position of the tool path.

 

Start Point

Used to specify a starting point off of the part from which the tool tip will proceed to on first entry into the material. (Otherwise 0,0, Clear Z is assumed.).  This option is only used if Drive Loop (see above) is set to close.  You can pick the point from the part or input x,y,z coordinates directly.

 

Start Axis

In most cases, the drive surface will determine the tool axis clearly so there would be no need to define the starting axis. But, for example, when you want to select a XY plane as drive surface, the starting axis must then be selected. The starting axis is optional to help the system calculate the tool axis correctly.

 

You can pick the direction from the part or input x,y,z coordinates directly.  If not specified, 0, 0,1 (the current Frame's Z axis) is assumed.

 

 

 

An alternative to 5 Axis indexing through rotation about table axes is the use of head attachments. Head attachments can allow the machining of tool paths wherein the tool axis is not along the machine Z axis. Instructions for the automatic loading of heads are written in CL output as appropriate.

 

In order to support the management of Head attachments in output, the following Output Variables have been added:

 

TAB_AXIS1_NAME

TAB_AXIS1_ANGLE

TAB_AXIS2_NAME

TAB_AXIS2_ANGLE

HEAD_NAME

HEAD_NUM

HEAD_IAXIS

HEAD_JAXIS

HEAD_KAXIS

FIXTURE_OFFSET_REGISTER(not yet in use)

 

Output variables are located in the file "OutputVariables" located in the "/cam_config" subdirectory of your VX install directory. If you copy this file to your User Directory and then modify the copy, the modified version will be used. VX CAM will first look in your User Directory to locate the file. If it is found there, it will be used.

 

• Head attachment information is currently not exported to or imported from CAM libraries.

 

When a Tooling List is requested from the NC Program Output Form, the names and locations of the required Head Attachments are written out as part of the machine definition. Also, the "Toolpath space" field will only allow "machine" as the selection. The "local" option will not be allowed.

 

In this initial implementation of head attachments, there is no CAM Object Class to manage them. Therefore there is no geometric representation support for head attachments.

 

In order to use head attachments, the following steps should be taken:

 

1. The file "HeadAttachments" located in the "/output_def" subdirectory of your VX install directory should be modified or a copy can be made into your User Directory and then modified.

2. The format of the file is the same for each line:
   station_id_for_head_attachment:Name_of_head_attachment

 

As many head attachments as necessary may be loaded in this file.

 

3. Select Machine Manager > Programming and set the "MULTITAX" field of the Machine Programming Details Form to "yes."

4. Select Setup Manager > Frame Manager and use the "Head" field to select a head attachment defined in step 2 above. Press "Accept" and it will be used during output for all operations created in the frame.

5. (Optional) Select Process Manager > Operations >Sort and set the "Object Type" field to "frame." All operations which share a common head attachment will be output consecutively.

 

When output is created, each tool path using a given frame will have its coordinates transformed to the correct machine space and the appropriate head for that tool path will be used.

 

If it is necessary to write out 5 axis motion and there are no table axes or head attachments defined, then the data will be transformed to machine space. In this case it is recommended that you still perform step 3 above.

 

In the unlikely event that both head attachments and rotational axes are both present, the head attachment will take precedence.