Pocketing Toolpath

This specifies the depth at which the toolpath is calculated from.

When cutting directly into the surface of a job the Start Depth will often be 0. If machining into the bottom of an existing pocket or 3D region, the depth needs be entered.

When a toolpath is created, the Pass Depth value associated with the selected tool (part of the tool's description) is used to determine the number of passes needed to profile down to the specified Cut Depth. However, by default the software will also modify the precise step down by up to 15% in either direction, if by doing so it is able to total number of passes required to reach the desired cut depth. It is nearly always desirable to benefit from the significantly reduced machining time of cutting using less passes if possible. Nevertheless, there are some occasions where the exact step down for a given profile pass needs to be more precisely controlled - when cutting into laminated material, for example. The Passes section page indicates how many passes will be created with the current settings.The Edit Passes... button will open a new dialog that enables the specific number and height of passes to be set directly.

The Pass Depths section at the top of the form shows a list of the current pass depths. The relative spacing of the passes is indicated in the diagram next to the list. Left click on a depth value in the list, or a depth line on the diagram, to select it. The currently selected pass is highlighted in red on the diagram.

To edit the depth of the selected pass, change the value in the Depth edit box and click Apply.

The Delete button will delete the selected pass.

The Clear All Passes button will delete all the passes.

To add a new pass, double left click at the approximate location in the passes diagram that you wish to add the pass. A new pass will be added and automatically selected. Edit the precise Depth value if required and then click Apply.

The Set Last Pass Thickness option will enable an edit box where you can specify the last pass in terms of the remaining thickness of material you wish to cut with the last pass (instead of in terms of its depth). This is often a more intuitive way to specify this value.

El primer método simplemente establece las pasadas según la propiedad Profundidad de paso de la herramienta seleccionada. De forma predeterminada, este es el método utilizado por Aspire cuando crea pases de perfil inicialmente. Sin embargo, la opción Mantener la profundidad exacta de paso de la herramienta está marcada, el software no variará el tamaño del paso para tratar de optimizar el número de pasadas (ver arriba).

El segundo método crea pasadas espaciados uniformemente según el valor especificado en el cuadro de edición Número de pasadas.

Para aplicar cualquiera de los métodos, haga clic en el botón Establecer pasadas asociado para crear el conjunto resultante de profundidades de pasada en la lista de pasadas y el diagrama.

If this option is selected two tools are used to clear the pocket. A large tool to do the bulk of the area clearance and a smaller tool (the first tool selected) to remove the remaining material and do a final profile pass.

When a pocket toolpath is created, the Pass Depth value associated with the selected tool (part of the tool's description in the Tool Database) is used to determine the number of passes needed to pocket down to the specified Cut Depth. However, by default VCarve Pro will also modify the tool step down by up to 15%, if by doing so it is able to reduce the total number of passes required to reach the desired cut depth. It is usually desirable to benefit from the significantly reduced machining time of cutting pockets using less passes if possible.

Nevertheless, there are some occasions where the exact step downs for a given profile pass needs to be more precisely controlled - when cutting into laminated material, for example. The Passes section of the Pocket Toolpath page indicates how many passes will be created with the current settings. The Edit Passes... button will open a new dialog that enables the specific number and height of passes to be set directly.

There are two choices of the type of fill pattern that will be used to clear away the area to be machined with the Pocket Toolpath, Offset and Raster.

Clear Pocket - Offset Strategy

Clear Pocket - Raster Strategy

Calculates an offset area clearance fill pattern to machine inside the selected vector(s). Options for Cut Direction to be either: Climb (CCW) cutting direction Conventional (CW) cutting direction.

Offset larger than 50%

Tails to clean out corners

Calculates a Raster based area clearance fill pattern to machine inside the selected vector(s). Cut Direction for the final pass to be either:

• Climb (CCW) cutting direction
• Conventional (CW) cutting direction

This option is used to leave material on the inside of the pocket for the Profile Pass to clean-up. This is often very useful for ensuring the cutter does not mark the edge surface of the pocket when roughing out.