Machine Dynamics: General Machine Parameters
Use this tab to
enter feed rate and cornering information that is used by the
highfeed
machining function in the Toolpaths
Manager.
Highfeed machining
is a method of optimizing Mill or Router 2.5- and 3-axis toolpaths
to reduce machining time by controlling feed rates around corners
and calculating chip load. It also manages machine forces to prevent
axis over-travel.
NOTE
Highfeed machining cannot
be used with Multiaxis or Lathe toolpaths.
Feed Rate Smoothing
Mastercam uses these parameters to break up a toolpath into
small segments or blocks. When you optimize the toolpath with
highfeed machining, Mastercam analyzes the feed rate for each
block, then uses these parameters to combine blocks back together
into single moves that use the same feed rate. To refine the deceleration
into and acceleration out of corners, Mastercam applies the Accelerate to smooth feed rates parameter
to break the motion into even smaller blocks to create a gradual
slowing down or speeding up of the tool motion.
Cornering
Use these parameters to define a corner as a degree
of a change in direction and to limit feed rates when machining
a corner. Use Cornering acceleration to enter the acceleration
value in Gs that your machine tool is capable of. If the manufacturer
has not provided this information, you can perform a cornering
acceleration test to determine the best values.
Parameters
Recombine segments when feed rate changes less than
If the feed rate of a segment changes less than this percentage, compared to the
previous segment in the toolpath, the segments are combined into a single line or
arc. The suggested setting is 10%.
Look-ahead (% of tool diameter)
Breaks the toolpath into segments whose maximum length is the look-ahead distance.
This parameter slows the feed rate before reaching an area where the tool is buried.
Larger values increase the distance for slowing down into and accelerating out of
corners. The suggested setting is 10%.
Maximum feed rate change per block
Limits the feed rate changes in each block. Smaller values increase the number of
segments, thereby increasing the distance for slowing down into and accelerating
out of corners. The suggested settings are 20 in/min and 500 mm/min.
Accelerate to smooth feed rates
Allows the machine to slow down gradually as it approaches a corner and speed up
gradually after leaving a corner. It breaks the toolpath into smaller segments than
it has already been broken into by the look-ahead value. The maximum feed rate change
per block is limited by the acceleration value.
This option is not advised for controls that have a slow processing speed.
For these controls, this option could result in a longer processing time since it
produces more blocks to process.
Segment length (% of tool diameter
)
Segments longer than this value are broken into shorter segments. This parameter
is only available if you choose Accelerate to smooth feed rates.
Slow to minimum cornering feed rate when direction changes
When the toolpath approaches an area where the direction changes more than this value,
the feed rate is reduced to the minimum cornering feed rate.
Minimum cornering feed rate
Sets the feed rate to use at sharp corners and small-radius arcs.
Cornering acceleration
Opens a dialog box where you can enter the maximum feed rate for corners and arcs
before causing axis over-travel.