Feeds and Speeds in the Machining Cost Model
For most machining operations, feed and speed are fundamental to the determination of cutting time.
Feed is the distance the tool travels along or through the part per rotation of the tool (or, for turning operations, per rotation of the workpiece). This is the distance the region of contact moves relative to the workpiece per rotation.
For milling and drilling operations, speed is how fast the tool turns in unit distance per unit time; that is, the speed at which a point on the outer edge of the tool moves along the circular path around the tool’s axis of rotation. For turning operations, speed is how fast the workpiece turns in unit distance per unit time; that is, the speed at which a point on the outer edge of the workpiece (at the cut location) moves along the circular path around the turning axis.
This section contains the following subsections:
Interpolated and User-specified Feed and Speed
When aPriori selects a tool for a machining operation, it establishes default values for feed and speed. The default values are arrived at by interpolation from cost model data tables, based on the following:
• Tool diameter
• Tool series
• material cut code
• For rough material removal, setting for Rough Material Removal Approach (see User Inputs for Machining)
Following are some of the data tables used for this purpose:
• tblMilling
• tblDrilling
• tblGeneralTurning
Several other tables are specific to a particular process, such as tblChamfering and tblGunDrilling.
See Tool Selection for Machining for more information.
Users can override these defaults and specify feed or speed explicitly by using one of a variety of process setup options (see User Inputs for Machining):
o Specify General Milling Speed
o Specify General Turning Speed
o Specify Cutting Speed for Contouring
o Specify Cutting Speed for Facing
o Specify Cutting Speed for Side Milling
o Specify Drilling Speed
o Specify Plunging Speed
o Specify Rough Turning Speed
o Requested Feed per Tooth
o Number of Teeth
o Requested Tool Cutting Speed
Note that the PSOs for milling operations, instead of specifying feed directly, specify the feed per tooth and the number of teeth: Feed = Feed per Tooth * Number of Tool Teeth.
For rough milling and bulk milling, you can also override the use of speed and feed, and specify material removal rate directly.
o Requested feed per Rev
o Requested Tool Cutting Speed
o Requested Tool Cutting Speed
Adjusted Feed and Speed
aPriori adjusts the interpolated or user-specified feed and speed values based on the following considerations:
• Machine limitations: speed is bounded above by the value specified for the machine property Spindle Speed. This property specifies the maximum spindle speed achievable by the machine. You can remove this limit with the setup option Ignore Machine Spindle Speed Limit.
• Stock hardness (or post-heat-treatment material hardness, if applicable for finishing operations—see General Routing Strategy and Material Hardness Achieved Through Heat Treatment in Machining Node Process Setup Options). The adjustment uses data from the lookup table tblHardnessCompensation.
• Tool length
• Tolerance requirements (see the "Specifying Tolerance and Roughness" section of the aPriori User Guide )
• Cost model variable speedSafetyFactor
• Cost model variable powerSafetyFactor
• For rough milling speed, setting of Rough Milling Aggression Adjustment Dial (see User Inputs for Machining).
aPriori further adjusts feed by multiplying by one of the following cost model variables:
• boreFeedAdjustment
• drillFeedAdjustment
• endmillFeedAdjustment
• millFeedAdjustment
• turningFeedAdjustment
aPriori further adjusts speed by multiplying by one of the following cost model variables:
• boreSpeedAdjustment
• drillSpeedAdjustment
• endmillSpeedAdjustment
• millSpeedAdjustment
• turningSpeedAdjustment
The adjusted values are sometimes referred to (for example, in the Process Options Editor) as final feed and final speed.
Feed, Speed, and Cut Time
aPriori generally uses the adjusted (final) values for feed and speed as follows in order to determine operation cut time:
• RPM: aPriori uses speed to determine tool RPM. Recall that speed is the speed at which a point on the outer edge of the tool moves along the circular path around the center of the tool. So the distance traveled by the point during one revolution of the tool is:
Pi * Tool Diameter
So the time elapsed during one rotation is:
(Pi * Tool Diameter) / speed
RPM is the reciprocal of this:
RPM = Speed / (Pi * Tool Diameter)
Speed is calculated (by aPriori) or specified (by the user) using the units of meters per minute. To calculate RPMs, aPriori converts speed to millimeters per minute, since diameter is calculated or specified in millimeters.
• Tool axis speed: aPriori uses RPM and feed to determine the speed of the tool as it moves along the tool path. Recall that feed is the distance the tool travels along the tool path per tool rotation. So tool axis speed is given by:
Tool Axis Speed = RPM * Feed
See also Tool Axis Speed.
• Area removal rate: for some operations , aPriori uses tool axis speed and contact width to determine area removal rate:
Area Removal Rate = Tool Axis Speed * Contact Width
Contact width is determined using various heuristics, based on tool diameter (or workpiece diameter, for turning), tool reach, and operation type, among other factors.
• Volume removal rate: for some operations, aPriori uses tool axis speed and contact area to determine volume removal rate:
Volume Removal Rate = Tool Axis Speed * Contact Area
Contact area is determined using various heuristics, based on tool diameter (or workpiece diameter, for turning) and cut depth, among other factors.
• Chipmaking time: this is the portion of cutting time during which the tool is engaged and in contact with the workpiece. aPriori usually determines chipmaking time in one of three ways:
o Based on tool path length and tool axis speed:
Chipmaking Time = Tool Path Length / Tool Axis Speed
Most hole-making and hole-finishing operations use this formulation; the tool path length is generally the length of the hole plus the drill-tip length (for blind holes) or twice the drill-tip length (for through holes). In addition, some cases of surface facing use this formulation; aPriori chooses a facing tool path based on tool diameter and surface geometry, as well as on the surface’s surrounding geometry.
o Based on GCD area and area removal rate:
Chipmaking Time = GCD Area / Area Removal Rate
Many surface finishing operations use this formulation. Geometry extraction determines the GCD area from the model.
o Based on removed volume and volume removal rate:
Chipmaking Time = Removed Volume / Volume Removal Rate
Bulk milling, rough milling, and rough turning use this formulation. Geometry extraction and material allowance help determine the volume to be removed.
Note that the Process Options editor displays the most recent costing’s values for adjusted feed and speed (Final Feed and Final Speed), as well as tool axis speed (Linear Axis Feed Rate) and tool diameter.
Cut time is chipmaking time and non-chipmaking time (during which the tool is engaged but not in contact with the workpiece), together with rapid movement time (during which the tool is not engaged and is approaching or departing a GCD). See Cut Time for Machining Operations for more information.