This guide outlines the basic workflow and best practices for programming 2-Axis pocketing operations in RhinoCAM.

what is a pocket operation?

A Pocketing operation is used when you want remove all material with a closed boundary down to a set depth. Pockets can be programmed to cut through the full-depth of the materials or partial depth.

getting started

program stock

see the stock setup guide

import tool database

see the tool database guide

 

locate geometry

the approach taken in this demonstration is to locate the geometry at he maximum depth of the cut.

for example:

  • if the desired depth of the pocket is .375″, then, you would move the geometry to that elevation
  • if you would like the pocket to cut all the way through the material, you would move it slightly [no more then .02″] below the bottom of the material.

please note: This one method of establishing a relationship between stock, geometry, and toolpaths. There are many scenarios where one would want or need to take a different approach. There is no right or wrong way!

 

2 1/2 Axis pocketing operation programming

select the Pocketing operation

select ‘Pocketing’ in the RhinoCAM Machining Browser 2-Axis machining operations drop-down menu

Control Geometry

Select control geometry:

  • Select the ‘Select Curves/Edge Regions’
  • Select the curves that define the boundary of the pocket
  • Once added, they will appear in the  to the ‘Selected Machining Region(s)’ list

 

Tool

Select a tool by highlighting it in the Tools list

The ‘best’ tool is generally the largest available which allows you to cut your design geometry. Larger diameter tools are stiffer [and are therefore more precise], cut more material per revolution, and can handle a greater cutting depth [which reduces overall cutting time].

 

Feeds & Speeds

Select Load From Tool’ option to load tool data from the tool database.

Clearance Plane

The Clearance Plane describes the X-Y plane where tool travel motions can safely occur across the CNC bed . This needs to be set above anything on the CNC table in order to avoid collisions.

Select the Stock Max + Dist. option and enter a distance of 0.25″. This ensures that all tool travel moves across the bed will happen at an elevation 0.25″ above the stock.

Sorting

  • Leave No Sort selected (This should be the default selection)

 

Advanced Cut Parameters

  • This tab can be ignored

Pocketing Entry/Exit

Best practice is to program a “lead-in” motion for vertical ramp motion to every toolpath level. Introducing the tool gradually into the material increases tool life and avoids sudden forces which could dislodge workpieces or break tools.

Under Engage Motion:

  • Select Path
  • Set ramp Angle (A) = ~5 degrees
  • Set Height (H) ≤ cutting pass dept
  • Select Apply entry/exit at all cut levels

 

 

Cut Levels

  • In this example, we will select the Location of Cut Geometry as At Bottom. This is because we initially positioned the control geometry at the bottom of the cut.
  • Set the ‘Total Cut Depth’ value to the depth of the pocket. In this example, this will be the distance between the top of the stock and our control geometry.
  • Enter a value less than or equal to 50% of your tool diameter for ‘Rough Depth/Cut’
    Note: Enter a value in inches here, not a percentage

 

Pocketing Entry/Exit

Best practice is to program a “lead-in” motion for vertical ramp motion to every toolpath level. Introducing the tool gradually into the material increases tool life and avoids sudden forces which could dislodge workpieces or break tools.

Under Engage Motion:

  • Select Path
  • Set ramp Angle (A) = ~5 degrees
  • Set Height (H) <= cutting pass dept

Select Apply entry/exit at all cut levels

Cut Parameters

  • set Stock to 0. This value defines the dimension of material left between the control geometry and the actual cut. Typically, you will want your cut to precisely match your geometry.
  • Cut Direction should typically be set to Climb, which typically results in the best surface quality and accuracy. For more information, MecSoft, the creator of RhinoCAM has produced an excellent article explaining the difference between climb and conventional milling.
  • set Stepover Distance less than or equal to 40%. A larger stepover value results in faster milling time at the expense of reduced surface quality.