Note on using drills in the turning environmentwww.kxcad.net Home > CAM Index > EdgeCAM Index >
Strategy - Selects how to create the hole:
Drill - The tool retracts between pecks at the rapid rate.
Chipbreak - This cycle works in the same way as Drill, but the tool retracts by 1mm or .05" after each peck.
Ream - The tool feeds to Depth, then feeds up to the Clearance plane.
Bore - The tool retracts between pecks at the rapid rate. When the tool reaches the specified Depth for the cycle, the tool spindle stops. The tool then indexes, locks and shifts before retracting to avoid scoring the bore hole.
Tap - This is selected as the only available strategy if a Tap tool is selected. The tool feeds to the specified Depth and dwells as required. The spindle is then reversed and the tool feeds out.
Plunge Feed - Specifies the feed rate in the workplane in units per revolution (for a Boring tool, for example) or in units per minute.
Note on using drills in the turning environment
If the 'Static Tool' checkbox on the Mounting tab in the ToolStore is not checked, the plunge feedrate from the ToolStore is not passed through to the hole cycle.
Percentage Feed - Speed adjustment for tapping only. Percentage of nominal feed to be used, in range 90% -110%
Speed - Specifies the rotational speed of the tool in revolutions per minute.
Dwell Time - Specifies the time (in seconds) the cutter spends at depth.
Subroutines - The parameter is present in milling cycles that could allow the machine tool controller to generate subprograms. Choose between:
Controller - Allows the controller to generate subprograms if more than one operation is performed on an identical pattern (for example, a set of points).
Pathtrace - Stops the controller from generating subroutines.
Feature Name - Enter a name here to allow labelling of digitised information for this cycle to enable "pickup" of this information in another (similar) cycle.
Tap Cycle - Selects a Right or Left-handed tap cycle.
Optimise Path - Selects the toolpath optimisation strategy:
None - The holes will be machined in the order in which they were selected.
Return to Start - The holes will be machined in an order to give the shortest path based on a need to return to the start point at the end of the cycle.
Closest Neighbour - The holes will be machined in an order to give the shortest path based on always machining the next nearest hole.
Alternatively, the holes can be machined in one of the following patterns:
|
X Lace |
X One Way |
Y Lace |
Y One Way |
|
|
|
|
|
|
Please note that the direction of drilling is dependent on the tool position at the start of the toolpath. |
|||
Note on merging optimised hole cycles
When sequences are rationalised or otherwise re-ordered, a number of cycles are frequently grouped together for machining by a single tool. In the case of hole cycles this gives rise to a canned cycle (G81 etc) in the NC file for each EdgeCAM cycle instruction. The Merge Hole Cycle option on the Rationalise Sequence (Instructions menu) dialog enables you to group such instructions into a single cycle so that multiple, identical holes may be drilled with one G81 canned cycle instead of many individual canned cycles each drilling one hole.
If cycles have different
optimisation the combined cycle is set to <none> and is not
optimised. The order of drilling will be as if cycles had never been optimised
and thus the toolpath may change.
