Feeds and Speeds

Cutting conditions (feed/tooth and cutting speed) can be included in a tools catalog. This data is converted into machining feedrate and spindle speed parameters to be used in machining operations by means of formula.

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 & Speeds tab of the Tool Definition dialog box.

In the Feeds and Speeds tab of milling operations, the Rough or Finish quality of the operation and the tool data are taken into account for computing the feeds and speeds.

Cutting Conditions

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.

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

N (in rev/mn)  = Vc / (D * PI)
where:
D = tool diameter for milling/drilling in mm
Vc = cutting speed of the tool or insert.

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

Vf (in 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 operation is finishing type (for example, Lathe Profile Finishing) or if it includes a finishing feedrate.

If the tool data is set to 0 (that is, if there are no specified values in the catalog), then spindle speed N and machining feedrate Vf are not computed on the operation.
In such cases, if Automatic Compute from Tooling Feeds and Speeds is set, the last values set on this operation are retained. If a new operation is created, a default value is used.

Update of Feeds and Speeds on Machining Operation

Operation with a Tool

When you modify a feeds and speeds attribute on the tool, the feeds and speeds values of the operation are not automatically updated.

Feeds & speeds of the operation will be updated according to tooling feeds and speeds:

• when you select a new tool
• by selecting the Automatic Compute check boxes in the Feeds and Speeds tab of the operation
• by clicking the Compute button located in the Feeds and Speeds tab of the operation.

Two check boxes allow operation feeds and speeds values to be updated automatically when feeds and speeds values of the tool are modified.

If they are checked then the feeds and speeds values of the operation will be updated when the feeds and speeds values of the tool are modified.
These two buttons will work separately: if feedrate Automatic Compute is checked and not the spindle Automatic Compute then the only the feedrate values will be computed.
If they are not selected then automatic update will not be done.

When you modify the feeds and speeds values on a tool, all existing operations with these check boxes selected that use this tool (or an assembly using this tool) will be recomputed.

The Compute button allows you to force the update of the operation values if one or both check boxes are not selected.

The feed and speed values are computed according to the Quality setting on the operation.

Possible Quality setting are:

• Rough: rough values of the tool are taken into account
• Finish: finish values of the tool are taken into account
• Either: no computation will be done for the operation's feeds and speeds.

In Tools > Options > Machining > Resources, settings are available to define how the Automatic Compute check boxes in the Feeds and Speeds tab are to be initialized for creating new operations.

Operation without Tool

When a tool is selected for the machining operation, the operation is updated with the new tool's feeds and speeds data.

Feeds and Speeds Change and Toolpath Computation

Depending on the type of operation and feedrate, when the user modifies a feedrate or spindle speed, the toolpath is not broken and is updated with the new value of feedrate or spindle speed. The user can therefore change feeds and speeds without needing to recompute the toolpath.

Please note, however, that the toolpath is broken when the user modifies:

• a local feedrate
• a plunge, approach or retract feedrate in an axial machining operation
• feedrate reduction in corners
• feedrates defined in turning operations.

In these cases, the toolpath should be recomputed.