Router-CIM Automation Suite



Previous topic Next topic  


Previous topic Next topic  

Advanced Rest Pocketing (Adv. Rest Pocketing)



This version of Advanced Pocketing allows you to use this cutting cycle in order to find the REST of the material left over from a previous pocketing cycle.


An example of this would be if you were to use a cutting tool that has a diameter larger then twice the diameter of the tool you may be using to apply a finish pass around a pocket. The Advanced Rest Pocketing would calculate the clean up needed in order to not leave material by adding additional cut paths.


Note: This cycle is only available on 64-bit Operating Systems. If you are running a 32-bit Operating System, you will be unable to use this cycle.


Advanced Rest Pocketing Tool Path

Advanced Rest Pocketing Tool Path




The following parameters effect the toolpath creation:


Spiral-IN <N>

The value is not applicable to a Advanced Rest Pocketing function.


Rest Cutting <Y>

The value of 'Y' initiates the Advanced Rest Pocketing cycle.


Prev. Radius <0.0>

The value entered in this parameter is what the Advanced Rest Pocketing cycles uses to determine the amount of clean out passes it will need to make based on the tool that is selected for use in this cut cycle and what is entered into this parameter.


The value should be the radius of the tool that was used to pocket the overall geometry.


Finish Allow

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


Step Over %

This value is the percentage of the tool diameter between each pass of the tool in the pocket. This needs to be a real number such as 25.0 or 50.0.


Climb Mill <Y>

The value represents if the cutting cycle will be doing Climb (CCW) milling <Y> or if you want the cutting cycle to do Conventional (CW) milling <N>


CleanUp Pass <N>

A CleanUp Pass is described as an additional tool path that travels around geometry allowing you to use Cutter Compensation for the boundary of the geometry.


Ramp-IN <N>

A Ramp-In set to <Y> will allow you to have the cutting cycle enter the cut with a ramp instead of a plunge. If this parameter is changed from the default of <N>, then the parameter of Ramp Angle will need to be defined in degrees.


Ramp Angle

If Ramp-IN is set to <Y>, then this parameter would need to be defined. The parameter will need a numeric value defining the degrees of the ramp such as 30 or 45.


Stay Down <N>

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 allow the tool to pick up and move to another area of the pocket to continue the shape.


Save Shape

If this parameter is set to <Y>, it will apply the cut cycle as usual but it will also give you the geometry that was used to create the cut cycle. The geometry will be added to the layer 'NC_Shape' for additional tool paths if needed.


**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.