The Part orientation in 3D space and the axis of rotation are important to 4 Axis machining. These two conditions affect the rotary axis zero. The part geometry and axis of rotation must be created in relation to the physical placement of the rotary table to insure that the proper NC code and machine tool motion are created.

When a 4 Axis cut is done, SURFCAM displays the tool while it moves around the geometry. The tool motion that is shown is the opposite of the actual rotary motion that is created. The clockwise tool motion is positive rotary motion. The counterclockwise tool motion is negative rotary motion. The post processor can override the direction of the rotary axis motion.

Typical Vertical Milling Machine with Rotary Table along the X Axis

 

SURFCAM 4 Axis creates tool path files along three linear axes and one rotary axis or two linear axes and one rotary axis. You can position the rotary axis at any orientation. The normal position of the rotary axis is along the X axis or the Y axis.

Set Axis for 4 Axis

The axis of rotation can be set at any angle and in any direction in 3D space. It must be set in relation to the physical placement of the machine tool's rotating axis. A common configuration is to have a rotary table mounted on the X positive end of the machine tool table. This requires the axis of rotation to be defined along the X axis. The first selection point is at the X negative end of the rotational axis. (This could be the center of the rotary table face.) The second selection point is at the X positive end of the rotational axis. This produces a positive motion when the rotary axis turns counterclockwise. When the points are selected in reverse order, a positive motion is a clockwise rotation.

In the following illustration, the line in the center of the face is the axis of rotation. When the end with the circle is selected first and the opposite end is selected second, the arrow indicates the direction of positive tool motion.

The arrow indicates negative tool motion if the end points of the line are selected in the opposite order.

A similar drawing can be created to indicate the machine tool's rotary axis orientation and axis of rotation.

Axis of Rotation

The axis of rotation can be selected with any orientation. When this command is not used, SURFCAM defaults to the defined axis rotation. When this parameter is set for the machine configuration, it is not necessary to click the Set axis command.

From the menus, click Tools > Options > NC Defaults > 4 Axis to set the default value.

Rotary Axis Zero

Setting the axis of rotation does not set the Rotary Axis Zero position. SURFCAM designates this position as normal to CView:1 in the Z plus direction.

Viewing a horizontal line from View:2 (Front View) or View:5 (Right Side View), the Rotary Axis Zero position exists when the tool is above, and perpendicular to the line with the tip pointing toward the line as in the drawing.

The tool location on the X, Y, or Z axis does not affect the Rotary Axis Zero position. The axis of rotation is identified with the line entering the right side of the box and exiting the left side.

The Rotary Axis Zero is at the 12 o'clock position. This drawing is in Isometric View.

 

Viewing the box from the right side is View:5 (Right Side View). The front side of the box is View:2 (Front View). The tool is above and perpendicular to the horizontal lines of the Front View and Right Side View sides. This indicates the Rotary axis rotation zero position.

Indexing Operations

You can index the rotary axis for positioning. It can be positioned for each cutting view. These views can be created from part sides, fixture sides, or work offset locations. The views define the index positioning for each SURFCAM operation.

A view to define each index must be created. After selecting the X and Y axis locations for the view, the origin is defined. This location defines the local coordinate system for that view. The origin for the standard views is at World X0, Y0, Z0. It is not required that you create views parallel to the 8 standard views when the desired origin is World X0, Y0, Z0.

It is recommended that the origin be placed at the center of rotation for each view. When different origins are used, care must be taken in selecting clearance plane locations.

The part geometry must be created in 3D space around the axis of rotation. The operation must be performed in View Coordinates. In the main toolbar, Coord must be set to VIEW. The CView must be set to the appropriate view for the operation. See Right hand rule.

The above drawing shows the axis of rotation along the X axis from negative to positive. This is indicated by the line through the center of the box. The arrow indicates the positive direction of tool motion for the rotary axis.

The top of the box is machined in View:1(Top View), the front of the box in View:2 (Front View).

With SURFCAM set to VIEW Coordinates, pocket the top in CView:1 (Top View). The output for the top pocket is positioned at a rotary axis of zero.

The front pocket is cut in CView:2 (Front View). The output for the front is indexed 90º before the pocket is machined.

The Tool Orientation for Indexing during the Pocket Operation

 

Simultaneous Axis Motion

You can select either 3 Axis or 4 Axis simultaneous motion. Select this option with the Options command on the NC > 4 Axis Menu. The options for the Limit Rotary Motion parameter are 3 Axis or 4 axis. The axis number selected determines the tool motion for the 4 axis operation that is done.

3 Axis simultaneous motion uses one rotary axis and two linear axes for motion. 4 Axis simultaneous motion provides one rotary axis and three linear axes of motion.

4 Axis simultaneous motion allows movement of all four axes during the operation. When 3 Axis is selected, axis motion is dependent upon the axis of rotation. When the axis of rotation is on the X axis, no Y axis motion occurs. When the axis of rotation is along the Y axis, no X axis motion occurs. When the axis of rotation is not along any standard axis, all 4 axis motion can occur.

3 Axis

The operation is done with the tool tip pointing through the axis of rotation. Lead angle, in the Lead angle dialog box, has no effect on the tool angle. The tool always points through the axis of rotation.

4 Axis

The tool orientation is often normal to the surface.

Tool Orientation during a Cut
3 Axis Simultaneous Motion	4 Axis Simultaneous Motion

To do 5 axis cutting, SURFCAM calculates I, J, and K vectors to direct the tool shank in relation to the tool tip contact point. These vectors identify the tool shank orientation during the cutting process. You can adjust the tool shank vectors used with lead angle and side angle inputs.

The cutting procedures that are described in this section are all done in the Top View.

With SURFCAM you can generate NC programs in a local coordinate system. Thus you can machine different sections of the work with independent machining orientations—a necessity with most parts. SURFCAM can be used to change the machining orientation of the part by using construction views. This is accomplished by setting the CView (construction view) parameter to the number of the view that matches the machining orientation of the piece currently being cut.

Set Axis for 5 Axis

Set Axis ( ) is used when one or more than one of the axes on the machine rotates. Use Set Axis to change the output of the rapid movements in the toolpath. A cylinder motion defines the rapid moves, not linear.

Before you use Set Axis , set Number of Rotary Axis on the 5 Axis Options tab to 1. See Number Of Rotary Axis (5 Axis).

The first default value for Number Of Rotary Axis is 0. Click Tools > Options > NC Defaults > 5 Axis to change the default value.

Number of Rotary Axis

1

SURFCAM displays the Select Point Menu. Select the first point and the second point on the rotation axis.

0

SURFCAM displays the message that the Number of the Rotary Axis is 0. Press any key to continue.