Using the drop-down list in the "Spindle" section, you may select a spindle and a tool. The space below contains the main data of the tool installed in the spindle. In order to see full information about the spindle, you need to click the information button . A window for editing spindle data will appear. In this window you can also edit all data related to cutting modes (cutting feedrate, rotation speed of the spindle, etc.). The data changes can be saved in the following ways:

1.Update properties only for selected operation

2.Update properties in all operations in current technology

3.Update properties for database

For the command to be able to calculate the tool trajectories and generate an operation, you need to select a set of millable surfaces.

Note. Unlike a Mill operation, for this operation, you need to select a pocket bottom surface and not a side as a processable surface.

The trajectories of the mill tool are calculated based on these surfaces. These surfaces are a reference geometry of the Pocket operation. In this command, you may also select a closed 2D sketch as a reference geometry.

But first let us discuss the case where the Reference geometry consists of surfaces. After running the Pocket command, it switches to the waiting mode and waits until a set of such surfaces is created. The following options for creating a set of surfaces are available:

1.Selection of individual surfaces.

2.Automatic selection of millable surfaces.

3.Clearing the set of surfaces.

4.A millable pocket contour expressed as closed-contour sketch geometry.

Selection of individual elements

Surfaces that are suitable for the Woodwork for Inventor CAM Pocket operation are those surfaces of the part model that are flat and make up the bottom of the milled pocket. Also, this surface may be oriented in space in the manner as to ensure that the tool’s capabilities allow it to rotate it with its back facing this surface (see fig. below). A possible vector of the tool’s spatial orientation is specified when configuring the machine’s spindles.

The compliance of the normal vector of the pocket bottom to the tool’s direction vector

You can check if the surface can be included in the set by placing the cursor on the desired surface. Such a surface will be highlighted in white. The inclusion of the surface in the set is performed by selecting this surface with the mouse cursor. Once the surface has been included in the set, it is highlighted in blue. To remove a surface from the set, you need to select the surface while pressing and holding the CTRL key.

Automatic selection of surfaces

This option automatically selects pocket bottoms that can be processed with a given tool.

Clearing the set of surfaces

Clears the current set of millable surfaces.

A millable contour expressed as sketch geometry

Sometimes there is a need to mill a pocket that is not directly expressed as a pocket bottom surface. For example, there exists machines with a vertical arrangement where a workpiece is mounted vertically. In such a machine, you cannot cut out a piece of the part that would separate from the workpiece because if such a piece drops down, it will damage the CNC machine. In this case, such a grove is milled as a pocket by shaving away all the inside material into shavings. Within the part model, such a pocket does not have a bottom and it is impossible to select it as reference geometry in the Pocket operation. In this case you need to draw a closed sketch and select it as reference geometry. Only one sketch can be selected for the mill operation. The plane of the sketch must meet the orientation capabilities of the spindle. The milling depth is set based on the sketch plane.

Only two options are available in the Pocket operation:

In principle, this means that you make a selection as to what type of milling will be performed:

▪Climb Milling: The cutting tool is fed with the direction of rotation.

▪Conventional Milling: The feed direction of the cutting tool is opposite to its rotation.

Sets the landing method of the tool to the starting point of the pocket milling trajectory. There are two landing options available:

- Vertical landing of the tool to the starting point of the trajectory.

- Orbit landing. In this type of landing, the tool performs a spiral movement downwards until it reaches the required milling depth (see fig. below). The orbit diameter and the step are set when specifying the tool. Later these parameters can be edited using the side browser.

Turns on or off stepover contour milling and allows the user to set the stepover distance.

- Stepover is off.

- Stepover is on.

If the stepover is on, you can indicate the depth of one layer.

Note. The functioning of this option is not visualized in the graphic view of the trajectory, but this option will have an impact on the generation of the final CNC program.

The meaning of this parameter is similar to that described in the contour Mill operation. However, there is one important thing to remember. During pocketing, two contours need to be distinguished which occur when calculating the tool trajectory (see fig. Below).

Two contours may be distinguished:

1.A finishing pass contour.

2.A pocket inside removal contour.

You should bear in mind that only the final contour is affected by the change of the correction type in the Pocket operation. The pocket inside removal contour is always calculated and generated as a contour with a tool correction which is calculated in the software.

We have two options to select the correction type of the final contour:

Adjusts the size of the tool overlap when performing the pocketing passes. The value of this parameter is set in percentage from the tool diameter. The higher the percent, the more dense the pocketing trajectory is.

A depth oversize allows the user to select how much material of the pocket needs to be left in terms of depth.

Allows the user to select an oversize with respect to the pocket contour.