Creating a Generic Machine and Managing Its Parameters

You can create a generic (virtual) NC machine and define its parameters. The NC machine is created under a Manufacturing Cell.

This task shows you how to:

See Also
NC Machine Resources

Create a Generic Machine

You can choose from several types of NC machine.

  1. Optional: If more than one manufacturing cells are created, select a manufacturing cell under which to create the machine:
    1. From the Tools section of the action bar, click App Options .
    2. In the App Options panel, select the ASO check box.
      The ASO panel appears at the left edge of the work area.
    3. In the App Options panel, click Change Active Simulation Object to a Newly Selected One and select a manufacturing cell in the tree.
      The selected manufacturing cell appears in the ASO panel. For more information, see Selecting the Active Simulation Object.
  2. From the Setup section of the action bar, click Generic Machine .
  3. In the Generic Machine dialog box that appears, select the type of machine to create:
    • 3-axis Machine
    • 3-axis with Rotary table Machine
    • 5-axis Machine
    • Mill-Turn Machine
    • Wire EDM Machine
  4. Optional: Enter a name and a comment for the machine.
  5. See below how to specify its parameters.
  6. Click OK.
    The reference machine is created under the selected manufacturing cell.

Choose Between Reference Parameters and Local Modifications

You can choose to propagate the reference parameters (defined at the creation of the reference machine) or allow modifications of the parameters in instantiations of the NC machine (local modifications).

Most reference parameters that are available when creating the reference NC machine are also available for local modifications. However, for Mill Turn machines, the turret and spindle parameters are only editable in the reference machine.

Important:
  • When a new machine instance is created, the initial values of its parameters are the same as the parameters of the reference machine.
  • NC programming is always done with reference parameters of NC machine, except those that are modified locally.
  • Local modifications are available only in the current Manufacturing Cell.

  1. In the Resource Configuration View, right-click the reference machine and select Edit NC Resources.
    1. In the dialog box that appears:
    2. To forbid local modifications, click in front of a parameter. Local modifications are no longer allowed if changes to .
    3. Click to allow the local modification again.
    4. Click OK.
  2. In the Resource Configuration View, right-click the instance machine and select Edit Local Parameters.
    A dialog box appears. All the parameters appear with the value defined in the reference machine. By default, they are not editable. The parameters you have locked in the reference machine are marked with a lock. The parameters available for local modification are marked with .

    1. When possible, click in front of the parameter.
    2. It changes to , and the parameter becomes editable.
    3. Modify the value as required.
    4. Optional: Click again to reset the parameter.
    5. Click Reset Local Modifications to reset all local modification parameters.
    6. Click OK.

    The modifications apply only to the instance of the machine. The values in the reference machines have remained the same.

Edit the Spindle Parameters

You can edit spindle parameters for all machines.

Note: When an Machining Operation is edited, its associated spindle and corresponding spindle axis system is highlighted in the work area.

  1. Select the Spindle tab.
  2. For a Mill-Turn Machine:
    1. Click Add Spindle to add one.
    2. Click Remove Spindle to remove one.
    3. Edit the spindle name.
    4. Define its number with a spinner.
    5. Activate the local definition of the part axis system.
    6. Define or modify the part axis system.
    7. Define the spindle axis.
    8. Define the radial axis.
    9. Define the maximum spindle speed.
  3. For other machines, you can define the following parameters.
    1. Edit the X, Y, and Z coordinates of the home point.
    2. Edit the I, J, and K axis of the orientation of the spindle.

Edit the Turret Parameters

You can edit the Turret parameters for Mill-Turn machines.

Note: When a Manufacturing Program is edited, its associated turret and corresponding turret axis system are highlighted in the work area.

Select the Turret tab.
  1. Click Add Turret to add one.
  2. Click Remove Turret to remove one.
  3. Edit the turret name.
  4. Define its number with a spinner.
  5. Define the type of the turret from the list (Rotary or Mill).
  6. Activate the local definition of the turning tool axis system.
  7. Define or modify the system from turning to axis.
  8. Select the axial axis.
  9. Select the radial axis.
  10. Define the X, Y, and Z coordinates of the tool change point or use the origin of the turning tool axis system.

Edit the Rotary Table Parameters

You can edit Rotary table parameters for 3-axis machines with rotary table.

  1. Select the Rotary table tab.
  2. Select the rotary axis from the list (A, B, C).
  3. Select the rotary direction from the list (Clockwise, Counter-clockwise, Shortest).
  4. Select the rotary type from the list (Absolute is the only possible value).
  5. Optional: Select the Rotable output in multi-axis mode check box to enable its output.
  6. Edit the other values as required.

Edit the Technology Parameters

You can edit the Technology parameters for wire EDM machines. Technology parameters are managed by the controller and help you choose the correct output code. You can then save these predefined parameter values into a Technology Set. A Technology Set can be associated with wire EDM operations and output in APT files.

  1. Select the Machine Type (manual or automatic).
  2. Optional: Click Select an Excel or Text Document to import a Parameters Table.
  3. Under Technology Parameters, click to add a new technology parameter.
    1. In the Technology Parameters dialog box that appears, enter a name such as TechnoParameter.1
    2. Select the Parameter Type.
    3. Click Default Value to define this as the default setting.
    4. Click OK.
  4. Optional: Select to remove an existing technology parameter.
  5. Under Technology Set, select to add a new technology set.
    1. In the Technology Set dialog box that appears, enter a name such as TechnologySet.1
    2. Optional: Edit the previously defined technology parameters, if required.
    3. Click OK.
  6. Optional: Select to remove an existing technology set.
  7. Optional: Select an existing technology set to display its parameters.

Edit the Tooling Parameters

You can edit the Tooling parameters for all machines.

  1. Select the Tooling tab.
  2. Select the tools library list.

    Note: By default, the Not Specified option appears when nothing is saved from CATPreference and Machine.

    1. Click to select a library or a library class from the database.
      Notes:
      • Selected libraries are saved in CATPrefence.
      • Last selected repository is set in machine. Resources are searched in the library browser in the repository set in machine instance or in machine reference.
  3. Optional: Activate the Radius compensation check box to enable the support of the radius compensation.
  4. Define the X, Y, and Z coordinates of the tool change point.

Edit the Compensation Parameters

You can edit the Compensation parameters for all machines.

  1. Select the Compensation tab.
  2. Select the 3D Contact Compensation Mode from the list (No, Contact, Tip & Contact).
  3. Select the check box Set 3D Contact compensation to all operations supporting this mode.

    • This check box can only be selected when 3D Contact Compensation Mode is defined as No.
    • Some Machining Operations propose cutter compensation modes other than 3D contact (2D radial profile, for example). See About 3D Feature for Spindles and Turrets for more information.

    If Set 3D Contact compensation to all operations supporting this mode is not selected and 3D Contact Compensation Mode is defined as Contact or Tip & Contact, a Compensation tab appears in the Strategy tab of the Machining Operation. In this case, 3D contact compensation is managed at the Machining Operation level.

Edit the Numerical Control Parameters

You can edit Numerical Control parameters for all machines.

Before you begin: The path for controller emulator and post processors are defined in Me > Preferences > App Preferences > Simulation > Machining NC Machining Apps Common Services > Output. Post processor words tables are defined in Me > Preferences > App Preferences > Simulation > Machining NC Machining Apps Common Services > Resources > .
  1. Select the Numerical Control tab.
  2. Select a Post Processor Provider to display the different PPs in the Post Processor field. Then select a Post Processor from the list.
    Note:

    If you do not specify the Post Processor Provider, then your selection in preferences determines the provider.

    For IMS and ICAM Foundation, the command to the right of the Post Processor field allows you to customize the post-processor.

  3. Select a post processor words table by doing either of the following:
    • Select a post processor words table from the list of pptables available in the preference path as mentioned above.
    • Select a post processor words table from the database by clicking the command to the right of the Post Processor words table field. Then select a pre-existing pptable document in the database or create one if an existing one is not already present.
  4. For machines with kinematics only, select a Controller Emulator Provider to list the different CEs in the Controller Emulator field below, then select a Controller Emulator from the list.
    Note: If you do not specify the Controller Emulator Provider, then your selection in preferences determines the provider.
  5. Select the preferred NC data type.
    • APT: Specifies APT source output.
    • CLF-3000 or CLF-15000: Specifies Clfile output. For circular interpolation, either 3000 and 5000 record type CLFiles or 15000 record type CLFiles are generated.
    • ISO: Specifies NC code output.
  6. For NC data type ISO, under NC Code Extensions, specify a single or multiple suppported NCCode file extensions (separated by a comma). For example: CATNCCode,tap,iso.
  7. Select the preferred NC data format.
    • Point (tool point coordinates (x,y,z))
    • Axis (tool axis components (x,y,z,i,j,k))
  8. Select the home point strategy from the list. It defines whether no instruction or a GOTO or FROM instruction is generated for the home point in the output.
  9. Optional: Define the Max Taper Angle to specify the maximum angle that the wire can reach.

    Note: For wire EDM machines only.

  10. Define the minimum and maximum interpolation radius used in the tool path computation and output file generation when generating circular interpolation.
    1. If an interpolation value is modified after the creation of the Machining Operation and the generation of the tool path, recompute the tool paths before generating the output file.
  11. Define the minimum discretization step and angle.
  12. Select the required check boxes to enable:
    • A 3D linear interpolation between 2 points.
    • A 2D circular interpolation between 2 points.
    • A 3D circular interpolation between 2 points.
    • A Helical Interpolation between two consecutive points
  13. Select the required check box to generate 3D NURBS interpolation data in an APT output file.

    See NURBS Formats in APT Output for more information.

    • When this check box is selected, an Output tab becomes available in the Machining Operation dialog box (provided they support NURBS).
    • If the Nurbs format check box in the Output tab is selected, NURBS output data is generated for the Machining Operation.
    • If it is not selected, there is no NURBS output data generated for the Machining Operation.
  14. Specify the maximum machining feedrate.
  15. Specify the rapid feedrate.

    This is used to compute an accurate machining time (in Display or Simulate, for example) and is used to replace the RAPID instruction in the output APT source.

  16. Select the required check box to use an axial or radial movement between the end of one Machining Operation and the start of the next one.
    A RAPID GOTO statement is added for the axial-radial movement if the option is selected.



  17. Activate RTCP mode by selecting the following check boxes: RTCP Support and RTCP ON (Default Mode). For more information, see About Polar and RTCP Modes.

    Note: Use RTCP mode with both generic and imported machines with at least one rotary axis.

  18. Select the Duplicate tools on heads check box for virtual machine simulation with multiple spindle heads (gantry machines, for example).

    Note: Multiple machines must be created.

    There is no primary/secondary relationship in the machine head definition. Tools are instantiated on all tool mount points on the command joint. The programmed tool mount point (and its corresponding head) is considered the primary. All the other tool mount points (and their corresponding heads) are implicitly considered secondary.

    It is not possible to modify the programming scenario in the same program. To machine three identical parts and define one part with a finishing operation, create two separate part operations: one part operation to machine the three parts, and one part operation to perform the finishing operation.

  19. Click User Variables.
    The Define User Variables dialog box appears.
    • Click New to add a user variable.
    • Select a user variable and click Delete to remove it.
    • Double-click any existing variable to edit its name.

Edit NC Output Parameters

You can define NC Output parameters for all machines.

  1. Select the NC Output tab.
  2. Specify the required options for:
    • Feedrates.
    • Tool motions:

      When generating APT, select Remove coincidental point between operators to remove the replicating points between Machining Operations if the end point of a machining operation and start point of the subsequent Machining Operation are exactly same.

    • Statements:

      For example, general information statements to be presented with the PPRINT syntax.

    • Format for point coordinates (X,Y,Z) and Format for axial components (I,J,K).