 |
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.
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.
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:
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 selected, the feeds and speeds values of the operation will be updated when the feeds and speeds values of the tool are modified.
These two check boxes work separately: if feedrate Automatic Compute is checked and not the spindle Automatic Compute then the only the feedrate values are computed. If they are not selected, the 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:
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.
When a tool is selected for the machining operation, the operation is updated with the new tool's feeds and speeds data.
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:
In these cases, the toolpath should be recomputed.
Transition
FeedratesYou can locally set the feedrate for a transition path to a machining operation B from a machining operation A or from a tool change activity. This is done by selecting the Transition check box in the Machining Operation dialog box for operation B.
The transition feedrate type (machining, approach, retract, finishing, and so on) can then be selected from the combo box. If a local transition feedrate is required, you must enter the desired feedrate value.
The locally defined feedrate value will be displayed in the Tool Path Replay dialog box and in the APT output. The corresponding color will be used for the transition path.
The color of the operation transition path during replay will depend on the selected feedrate type (as defined in the Tools > Options > Machining > General).
If the Transition check box in the Machining Operation dialog box for operation B is not selected, the transition feedrate is determined as follows: