Rough/Finish: Helix Bore
Use the options on this page to create roughing and finishing passes for a helix bore toolpath. You can set feed rate overrides separately for each type of cut. You can enter either a percentage override or an absolute value; Mastercam automatically adjusts the other field when you type a value in one.
Choose Finish to enable the finish pass options. Typically, if you use this option, you would set the Stock to leave values on the Cut parameters page to 0.
Common Toolpath Parameter Controls
Rough pitch
Sets the distance that the tool advances with each rotation.
Number of rough passes
Tell Mastercam how many rough passes to create. Set this value to more than one if you want to provide a rough pass stepover value.
Rough pass stepover
If you specify more than one pass, enter the distance the tool moves between the passes.
Feed rate at final depth
After the tool makes a complete pass, you can slow the feed rate to do the finish at the bottom. Enter a percentage value in the first box to override the programmed feed rate by that amount, or type in the desired feed rate directly in the second box.
Lock
Locks the value of the corresponding parameter. Mastercam will no longer recalculate the value when changes are made to the Tool page and you cannot edit the value until the parameter is unlocked.
Finish method
Choose a finish method from the drop-down selections.
- Helix upwardly: The tool feeds to the finish bore dimension and then generates a helix from bottom to top.
- Helix downwardly: The tool retracts to the top of stock, moves to the finish bore dimension and then generates a helix from top to bottom.
- Circle: The tool feeds to the finish bore dimension and creates a single circular cut at the bottom of the hole.
Finish pitch
Sets the distance that the tool advances with each rotation.
Finish stepover
The absolute distance between finish passes.
Feed rate
Enter a different feed rate for the finish passes than the feed rate used for roughing. This lets you adjust the chip load for the finishing operation.
Lock
Locks the value of the corresponding parameter. Mastercam will no longer recalculate the value when changes are made to the Tool page and you cannot edit the value until the parameter is unlocked.
Spindle speed (RPM)
Enter a different spindle speed for the finish passes than the spindle speed used for roughing. This lets you adjust the chip load for the finishing operation.
Lock
Locks the value of the corresponding parameter. Mastercam will no longer recalculate the value when changes are made to the Tool page and you cannot edit the value until the parameter is unlocked.
Spring passes
Enter the number of spring passes for the toolpath. Spring passes create additional finish passes along the same path as the last finish pass. You can use spring passes for parts with thin material that may have flexed away from the tool during previous passes or in cases of tool deflection.





