Optimization Parameters: Highfeed Machining
Use this tab to
choose whether the selected operations include both Roughing
and finishing, or Finishing only.
You also use this tab to edit feed rate parameters for individual
tools. Mastercam uses this information, together with the stock
setup parameters, to compute feed rates that result in an appropriate
chip load. The large window contains a table of reference information
for each specific tool; the parameters on the bottom apply to
all tools.
Highfeed generates the reference tool table automatically when
you select the operations to optimize. The tool diameter, shape,
corner radius, and feed rate are taken from the toolpath parameters
for each operation. Mastercam sets the reference depth of cut
to the tool radius, regardless of the toolpath parameters. Mastercam
calculates the plunge rate and material removal rate based on
the feed rate and depth of cut.
To make changes to any of the information, click on the line
for the desired tool and choose Edit tool.
Whenever you change one of the following parameters, Mastercam
automatically changes the others:
- Depth of cut
- Plunge rate
- Feed rate
- Volume/min (material removal rate)
NOTE
- Highfeed automatically changes the
reference cut depth to half the tool diameter. You may need
to check and adjust the reference cut depth.
- The reference cut depths in the
material removal table do not modify the cut depths in the
NCI file.
- If you select Finishing
only, the Stock
Setup tab is unavailable. Mastercam uses only the machine dynamics parameters
defined in the Machine
Definitions Manager.
Parameters
Finishing only
Choose this option to optimize feed rates for selected finishing operations only.
For finishing operations, Mastercam uses only the machine dynamics parameters defined
in the Machine Definitions Manager.
Roughing and finishing
Choose this option to optimize feed rates for both selected roughing and finishing
operations.
Reference tool list
Lists all of the reference tools that have been defined. Use the buttons on the right
to edit the list or individual tools.
Add tool
Opens the Add reference tool dialog box so that you can add a tool to the reference tool list.
Edit tool
Opens the Edit reference tool dialog box so that you can edit a selected tool in the reference tool list
Delete tool
Removes the selected tool from the reference tool list.
Scan NCI
Scans the NCI file for a list of tools used in the toolpath. Uses the diameter, shape,
corner radius, and feed rate from each tool.
Minimum feed rate
Keeps the feed rate within a reasonable range. The feed rate that is written to the
NCI file will not fall below the minimum feed rate.
Maximum feed rate
Keeps the feed rate within a reasonable range. The feed rate that is written to the
NCI file will not go above the maximum feed rate.
Maximum air cutting feed rate
Applies to blocks where no material is removed. This parameter can usually be set
to a higher value than the maximum feed rate.
Up feed rate scale factor
Adjusts the constant volume feed rate according to this factor and the angle of cut.
This scale factor recognizes that it is possible to cut faster in the upward direction
than in the horizontal direction, given the same volume removal rate, and increases
the feed rate accordingly.
Down feed rate scale factor
Used to calculate plunge rate. This scale factor recognizes that it is not possible
to cut as fast in the downward direction as in the horizontal direction, given the
same volume removal rate, and adjusts the feed rate accordingly.