Calculating Feeds and Speeds from a Material: Lathe
Mastercam will automatically take tool and stock material into consideration
when calculating speed and feed percentages needed for an operation.
The calculations and approaches are taken directly from the Machinist's Handbook (2000: Industrial Press)and
based on the formulas described in the following sections. If you need
to adjust these values (for example, to compensate for a hardened or softened
material), or need to create a material that is not in the library, you
can do so in the Material
Definition dialog box.
For most lathe operations, the spindle speed is usually programmed using
constant surface speed (CSS). This keeps the
cutting speed constant as the tool cuts toward or away from the Z axis.
Exceptions are drilling and threading operations, which are programmed
in revolutions per minute (RPM). Feed rates for threading operations are
not included in the material definition and must be defined with the threading
tool. For additional information, please see the Parameters
tab (Threading tools).
Calculating
spindle and cutting speed values
Spindle and cutting
speed (CS) values are calculated based on
the material’s base cutting speed value multiplied by the operation
type cutting speed percentage multiplied by the tool’s cutting speed
percentage. The formula looks like:
Spindle speed = (material
CS value x operation type CS %) x tool CS %
Most of these values are stored as part of the
material definition and accessed in the Material Definition dialog
box. The tool’s cutting speed % is specific to each tool and is read
from the tool definition. You set this on the
Parameters tab (turning and boring tools) for the tool definition
in the % of Material CS text box.
For example, aluminum
has a base cutting speed value of 1000 SFM. Assume ID roughing operations
use 80% of this base value. If the boring bar used for the operation
has its CS percentage at 80%, the spindle speed for this material
which will be output to the NC program is 640 SFM using the following
equation:
Spindle speed = (1000
x .80) x .80 = 640 SFM
For drilling operations,
the spindle speed in SFM is then multiplied by 3.82 / drill diameter
(for inch tools) or 318 / drill diameter (metric tools) to give the
spindle speed in RPM. For example, for a ½" diameter drill and
a constant surface speed of 1000 SFM:
Spindle speed = 1000
x (3.82 / .5) = 7640 RPM
Calculating
plunge rates from material
When From
material is chosen in the Tool
Settings tab of the Machine Group Properties dialog box and you
click Calc. Speed/Feed(shown
below) in the Finalize Properties page of the Create New wizard, default
plunge and retract rates are calculated at 50% of the feed rate. Please
see Creating Tools with the Tool wizard for more details.
Plunge rates are
only applied if your operation includes plunges, and your plunge cutting
method and parameters are set correctly in the Plunge
Cut Parameters dialog box.
Calculating feed
rate values
Feed per revolution
(FPR) works in much the same way. The FPR value is calculated based
on the material’s base FPR multiplied by the Tool Type FPR percentage
multiplied by the tool’s FPR percentage. The formula looks like:
FPR = (material base
FPR value x tool type FPR %) x tool FPR %
Set the tool FPR% on theParameterstab
(turning and boring tools)in the% of Material
Feed/Revtext box.
For example, aluminum
has a base feed per revolution value of .020". Assume that ID
roughing operations use 80% of this base value. If the boring bar
used for the operation has its FPR percentage at 90%, the FPR for
this material which will be output to the NC program is .0144 inches
per revolution using the following equation:
FPR = (.02 x .80)
x .90 = .0144 inches/rev