About Feeds and Speeds

This section describes how to manage the feedrates and spindle speeds of machining operations.

This page discusses:

See Also
Setting a Transition Feedrate

Cutting Conditions

Cutting conditions are included in a tools catalog. This content is converted into machining feedrate and spindle speed parameters that are used in machining operations by means of Formulas.

For an example of such a tools catalog, see FeedsAndSpeeds.xls file delivered in the .../startup/Manufacturing/Samples folder.

Cutting conditions are also available in the Feeds and Speeds tab of the Tool Definition dialog box.

In the Feeds and Speeds tab of the Machining Operation dialog box, the Quality (Rough or Finish) of the machining operation and the tool data are taken into account for computing feeds and speeds.

The units associated with each attribute are set using Me > Preferences > App Preferences > Simulation > Machining .

  • For cutting speed, you can choose the industry standard unit you are accustomed to: m/mn or ft/mn. Cutting speed is a linear value.
  • For spindle speed, the unit is turn/mn. Spindle speed is an angular value.
  • Cutting speed and spindle speed are related as follows (when tool diameter units are in mm): LG 
    spindle speed = cutting speed*1000/(Pi*tool diameter)
  • The feedrate attribute represents the global feedrate of the tool. If you modify the global feedrate, the feedrate per tooth is updated according to the Formula: 
    feedrate per tooth = global feedrate/number of teeth

    Note: The feedrate per tooth cannot be edited directly in the Feeds & Speeds tab.

The following cutting conditions data are supported: cutting speed (Vc), feedrate/tooth (Sz), and depth of cut.

Cutting conditions for drilling tools: 

 	MFG_VC: cutting speed in mm/mn
 	MFG_SZ: feedrate/tooth in mm/rev
 	MFG_PP: Depth of cut.

Roughing and Finishing cutting conditions for milling tools: 

 	MFG_VC_FINISH: finishing cutting speed in mm/mn
 	MFG_SZ_FINISH: finishing feedrate/tooth in mm/rev
 	MFG_VC_ROUGH: roughing cutting speed in mm/mn
 	MFG_SZ_ROUGH: roughing feedrate/tooth in mm/rev.

Roughing and Finishing cutting conditions for lathe inserts: 

 	MFG_VC_FINISH: finishing cutting speed in mm/mn
 	MFG_SZ_FINISH: finishing feedrate/tooth in mm/rev 
 	MFG_SZ_AA_FINISH: axial depth of cut for finishing
 	MFG_SZ_AR_FINISH: axial depth of cut for finishing
 	MFG_VC_ROUGH: roughing cutting speed in mm/mn
 	MFG_SZ_ROUGH: roughing feedrate/tooth in mm/rev
 	MFG_SZ_AA_ROUGH: axial depth of cut for roughing
 	MFG_SZ_AR_ROUGH: axial depth of cut for roughing.

Note: For a machining operation and its associated tools handling finish or rough parameters:
  • The finishing speed is either a Finishing Cutting Speed or a Finishing Spindle Speed.
  • The roughing speed is either a Roughing Cutting Speed or a Roughing Spindle Speed.

When a tool is selected for a machining operation, the spindle speed (N) and machining feedrate (Vf) are computed using the following Formula:

N (rev/mn) = Vc / (D * PI)

Where:

  • D = tool diameter for milling/drilling in mm
  • Vc = cutting speed of the tool.

For turning operations, N is automatically set in mm/min with the value of the insert cutting speed.

Vf (mm/rev) = Sz * N * Z

Where:

  • Sz = feedrate/tooth on the tool
  • N = spindle speed in rev/min
  • Z = number of teeth on the tool: (MFG_NB_OF_FLUTES) or 1 for a lathe insert.

Finishing data is used if the machining operation is a finishing type (for example, Turning Profile Finishing) or if it includes a finishing feedrate.

If the tool data is set to 0, then the spindle speed N and machining feedrate Vf are not computed on the machining operation. For new machining operations, default values are used.

Access to Feeds and Speeds Parameters

Feeds and Speeds parameters are accessible from several locations.

You can access Feeds and Speeds parameters by clicking More in:

  • The tool definition dialog box.
  • The Machining Operation dialog box.
  • The Tool Change dialog box.

The values defined in the Tool Definition dialog box apply to the machining operation or tool changes that use the tool.

If access to the speeds and feedrates values is allowed, those values are modified in the Machining Operation or Tool Changes. They are then applied to all the machining operations or tool changes using this tool.

Note: Access to the speeds and feedrates values is controlled by the administrator, from the Tool Definition dialog box, by switching the access icons from On to Off and vice versa:
  • If the tool definition dialog box has the Cutting speed and Feedrate per Tooth activated, access is allowed to the speeds, but not to the feedrates.
  • In the Machining Operations or Tool Changes dialog boxes:
    • If you select the first icon , it turns to and lets you access the speeds value (you have to select the one you need to modify).
    • The second icon is not clickable and prevents access to the feedrate value.

This feature is useful for all Turning, Milling, and Drilling tools.

Updating Feeds and Speeds in Machining Operations

You can update feeds and speeds values of the machining operation that have not been automatically updated.

Machining Operation Without Tool

As soon as a tool is assigned to a machining operation, the operation is updated with the tool feeds and speeds values.

Machining Operation with a Tool

When you modify a feedrate or spindle speed value in the Tool Definition dialog box, the feeds and speeds values of the machining operation must be updated.

Feeds and speeds of the machining operation are updated:

  • From the Feeds & Speeds dialog box.
  • From the Activities Process Tree, when you select Expanded View :
    1. In the Cutting Condition or Finishing Condition column, do one of the following:
      • Double-click the values of one or multiple machining operations with the same tool or tool assembly.
      • Right-click one or multiple machining operations, then select Edit from the context menu
    2. Select the new cutting or finishing condition.
    Note: The options Advanced Edit and From... can be used together to select the Cutting Condition or Finishing Condition to be the same as that of another machining operation.
  • From the Tool Definition feeds and speeds:
    • When you select a new tool
    • When you click Compute in the Feeds and Speeds tab of the Machining Operation dialog box.
      Note: The computation of the feeds and speeds of the machining operation depends on the Quality setting:
        • Rough: Rough values of the tool are taken into account.
        • Finish: Finish values of the tool are taken into account.
        • Either: No computation is done for the operation feeds and speeds.

Maximum Spindle Speed

You can set a maximum spindle speed value for all turning and axial machining operations, and modify it in the Machining Operation dialog box to suit the cutting conditions.

You can access this parameter from:

  • The Generic Machine dialog box, in the Mill-Turn Machine tab, Spindle tab:

    Max spindle speed is set to 6000turn_mn. The minimum value is 1.

  • The turning or axial Machining Operation dialog box Feedrate tab:

    The value of Max. Spindle Speed in the machining operation is editable, but cannot exceed that of the machine (a message error is displayed in this case).

    By default, the value of Max. Spindle Speed in the Machining Operation dialog box is that defined in the machine.

If the Spindle Output option is checked, the maximum spindle speed value can be automatically generated in the APT file at the beginning of the operation. This occurs by defining the NC Command NC_SPINDLE_MAXSPEED in the PP table.

The maximum spindle speed value serves as output in the APT file at the beginning of the machining operation with the command name NC_SPINDLE_MAXSPEED and syntax MAXSPNDL/%MFG_MAX_SPNDL_SPEED, & MFG_MAX_SPNDL_UNIT.

Example: 

*START_NC_COMMAND NC_SPINDLE_MAXSPEED
MAXSPNDL/%MFG_MAX_SPNDL_SPEED, & MFG_MAX_SPNDL_UNIT, & MFG_SPNDL_WAY*END

Note: If the option Spindle Output is not checked, syntax corresponding to NC_SPINDLE_MAXSPEED will not be generated. However, you still have the option to generate the maximum spindle speed value by using the parameter %MFG_MAX_SPNDL_SPEED in other operation-related instructions.

Feeds and Speeds Change and Tool Path Computation

Depending on the type of machining operation and feedrate, when you modify a feedrate or spindle speed, the tool path is updated with the new value of feedrate or spindle speed.

Note: However, the tool path is broken when you modify:
  • A local feedrate.
  • A plunge, approach, or retract feedrate in an axial machining operation.
  • Feedrate reduction in corners.
  • Feedrates defined in a turning machining operation.

In these cases, you need to recompute the tool path.

Multi-Configuration of Cutting Conditions for Tools

In the Tool tab of the Machining Operation dialog box, you can select the Machined material, Machining type, and Quality of surface - one for each configuration such as material, machining type, or quality.

To create a configuration, select any value from the list (generated from Resource Settings) or enter a new value. Click the plus icon . The configuration (set of three values) is assigned to the tool if the same configuration is not already present. The new configuration is added to the end of the list.

To delete a configuration, select one or multiple columns, and click the delete icon .

In the Feeds & Speeds tab of the Machining Operation dialog box, you can select any configuration that is applied to the machining operation. The configuration list displays the configuration of the tool selected in the Tool tab of the Machining Operation dialog box. Clicking ... opens the Imported parameterspanel which allows you to select which configuration attributes to import. These attributes vary depending on the tool but some examples are: machining feedrate, spindle speed, radial width of cut; axial depth of cut, and others.

Note: When migrating tools from previous versions:
  • Drilling tools: Create a configuration containing values from old attributes of Feedrate and Technology:
    • Material = Undefined
    • Type of Machining = Undefined
    • Quality = Undefined
  • Milling tools and Lathe inserts: Create two configurations containing values from old attributes of Feedrate and Technology:
    • Finishing values:
      • Material = Undefined
      • Type of Machining = Finishing
      • Quality = Undefined
    • Roughing values:
      • Material = Undefined
      • Type of Machining = Roughing
      • Quality = Undefined

For more information, see Parameters for Milling, Drilling Tools and Lathe Inserts.

Multi-Configuration of Cutting Conditions for Tool Assemblies

When a tool assembly is created, it inherits the same configuration as its related tool. However, a tool assembly configuration does not take into account the modifications made to the tool configuration. For example:

  • If you add a new configuration to the tool, it will not appear in the tool assembly configuration.
  • If you modify a parameter value in the tool configuration, it will not be modified in the tool assembly configuration.

In the Feeds and Speeds tab of the Tool Assembly Creation dialog box, an icon appears to indicate where the set of parameter values is created:



The parameter values are created at tool configuration level.


The parameter values are created at tool assembly configuration level.


The parameter values are created at tool configuration level and modified either at tool assembly or tool configuration level.

Tool Parameters

When you create a tool, you can specify parameters for removing chunks of material in the Feeds & Speeds and Technology tabs.

The following parameters do not apply to shanks.

Parameters Description
Max Chip Thickness Specifies a maximum thickness value for the chips to be removed during machining
Max Volume Rate Specifies a maximum volume value for the chips to be removed during machining
Max Power Specifies a maximum power value required for the material to be removed during machining