2D Pocket

2D_Pocket_Icon

Advanced 2D Pocketing uses advanced algorithms based on the wire frame input geometry and contains many options to control the creation of the tool path than the other pocketing cycles. This method allows for more complex geometry to be handed to the tool path generator.

The Advanced 2D Pocketing utilizes numerous parameters to generate the most efficient toolpath around a pocket. There are parameters to control the lead in motion, stepover distance, stepover type, and more.

The Advanced 2D Pocketing will start at a point inside the pocket and create offset tool paths, moving toward the outside of the pocket.

Advanced_2D_Pocket_Example

Advanced_2D_Pocket_Example2

Advanced-2D-Pocket-Parameters

The following parameters effect the toolpath creation:

Stock Offset <0.0000>

The value entered here will be added to the cut offset to provide material left for a clean up pass on the pocket with a separate tool.

Stepover <TW75>

This value defines the stepover made after each offset.

1) Default of TW75 will step over by 75% of the tool diameter

2) Number followed by the % sign. This needs to be entered as a percent number such as 25% or 50%. This will stepover the percentage of the tool diameter

3) Number only. You can identify a specific stepover offset by just putting in the value as long as it does not exceed the diameter of the tool. Value of 0.25 would stepover 0.25 regardless of the tool diameter.

Stepover Type <Retract-to-Clearance-Area>

There are different methods for moving from one step to the next step in the cutting cycle. This parameter defines the type of connection move between the offset cuts of each pass.

1) Direct - This is a straight line connection between passes on the shortest way without any retracting movements keeping the cutting tool at the current Z level for the pass.

2) Blend Spline - Tangential arcs connecting between the passes

3) Retract to Feed Distance - The cutting tool will retract to the feed distance to material variable after each stepover offset pass before moving to the next stepover offset.

4) Retract to Clearance Area - The cutting tool will retract to the safety plane after each stepover offset pass before moving to the next stepover offset.


Direct Stepover	Blended Spline Stepover	Retract to Feed Distance Stepover	Retract to Clearance Area Stepover

Stay Down <Y>

If this parameter is set to <Y>, it will keep the tool down while in the pocket to continue the shape. If it is set to <N>, it will keep allow the tool to pick up and move to another area of the pocket to continue the shape.

Clean Corners <N>

When set to “Y”, the toolpath will be extended into corners if the stepover does not reach.

Cut Direction <Climb>

The value represents if the cutting cycle will be doing Climb (CCW) milling or if you want the cutting cycle to do Conventional (CW) milling when pocketing inside geometry.

Lead Feedrate <0.0>

This sets lead-in and lead-out feed rates. The default is 50%. Setting this parameter to any number will override the lead-in feedrate to the number specified. Setting this parameter to a percentage, 25% (must include the % symbol) will adjust the lead-in based on the feedrate identified by the percentage defined on CNC machines with this capability.

Lead-In Type <Automatic>

This parameter defines the type of entry move the toolpath will make when making its initial approach.

The possible options are:

1) Automatic – The approach type will be picked automatically to avoid collision

2) Line – The ramp move is a slanted line when a Lead-In Angle is used

3) Helical – The ramp move is helical

4) ZigZag – The ramp move is alternating slanted linear moves in opposite directions

5) Profile – The ramp follows the toolpath contour shape while gradually plunging


Lead-in Line No Angle	Lead-In Line 30 Degree Angle	Lead-In Helical 30 Degree Angle

Lead-In ZigZag 30 Degree Angle	Lead-In Profile 30 Degree Angle

Lead-In Angle <0.0>

The parameter will need a numeric value defining the degrees of the ramp such as 30 or 45.

**Changing values in the cycle parameters may yield unexpected results with some settings or on some geometry. Examine the toolpath and NC Code carefully before running your machine tool if you change these default settings.