Lathe – Turning functions

Grooving tool profiling

A grooving tool has a flat side that is aligned parallel to the OD of a turned part, and a width. With the Vector grooving functions, the tool can have symmetrical radiused corners, and a specified positive angle tangent to each radiused corner. An under cut tool should be treated as a 0 degree side as the function cannot undercut with the side of a groover.

As with the Previous Lathe roughing and finishing, the Vector 10 lathe contours are defined as the wire frame representation of a cross section of the 2 axis contour. The radius is represented as a Y value and the length along the rotational axis is represented by the X coordinates. The contour should be a single trimmed chain. Grooving tools can be used to both rough and finish contours.

Both the profiling and area clearing functions can use predefined tools created in a JTS tool library. Check the Tool/job button to use a predefined grooving tool.

Select the contour with Shift Select from either end, then: NC-Lathe-Turn Profile Groove

See the tool definition section below for the grooving tool parameters. The tool origin can be specified as shown:

The other parameters are as shown in this drawing. Note that stock can be left on the Y-radius, and X-shoulder directions. The Clear Distance is placed on layer DOWN, with a long dashed line style. This is the reduced feed rate condition. The Pullout Distance is placed on layer UP with short dashed line style. This is a rapid. The width of the tool is automatically offset to the minus X direction, to prevent gouging of the contour with the back side ( right ) of the grooving tool. Change the Y direction to “Bottom to top” for ID groove tool profiling.

A grooving tool can also be used to rough out deeply convoluted lathe parts. The parameters are identical to the Groove profiling with 2 exceptions.

To use this function, draw a single chain profile the same as for Groove tool profiling. Then NC-Lathe-Turn Area Groove

The Step dX value is the distance between the vertical plunges.

In some cases it is desirable to alternate from side to side when cutting with a grooving tool (to allow for even tool wear and better chip clearance). To create this type of tool path, check the Alternating box on the dialog. Shown here with the Special-Simulate sequence numbers. Note that the grooving starts in the center and works out toward the ends of the profile to be cleared.

Symmetrical Right and Left hand area clearing (lathe roughing)

Symmetrical tools can be used to area clear or rough out volume of material on complex lathe contours. With this function a lathe right hand tool is used first, with a cut that proceeds from large diameter to small diameter and from right to left. When all the material that can be reached with this tool geometry is removed, a mirror image tool ( left hand) is then used to clean out from top to bottom and left to right. This enables automatic cleanout of corners with 2 tools, that would otherwise require flimsy tool geometry, or that may be impossible to cut with a single tool.

Access the function with NC-Lathe-Turn Hor. Area Lathe 2 Tools.

If using the JTS, predefined tools can be selected from the lathe tool library by pressing the Tool/job button. Specify both tools from a right hand orientation.

Tool 1 and Tool 2 are oriented as a right hand and left hand tool respectively, but use the same tool definition orientation for both. See the next section for the turning tool angular definitions.

Finish stock allowance can be specified as distance in X, Y, or a composite distance.

Step Distance is the radial cut depth per pass, and the safe distance is the distance that is traveled at a reduced feed rate before the contour is encountered.

No overlap in X, controls the over/undercutting or the contour between the two different tools. Non Descending will prevent cutting “behind” contours.

The right hand tools cuts first and removes all the material that the tool geometry will allow.

The left hand tool then clears only the area that the right hand tool cannot reach.

Lathe Tool Definitions

Lathe tool definitions are used for the lathe functions with the JTS capability. To define a lathe tool NC-Tool Lib-Define Turn Tool

. .

Enter a descriptive name for this tool type. T2 CNMG 85 deg diamond 0 deg clear

Tool number is the position within the turret at which the tool is stored

Correction D and Correction L are used to identify the machine controller, tool offset locations in which the operator has entered the tool measurements

The Lathe Tool section has the following data:

Radius – the radius of the tool tip

DX – The length of the insert if laid flat along the X-axis

DY – The height of the insert if laid flat along the X-axis, also the inscribed circle of the insert.

DZ – The thickness of the insert, used in simulation

DAngle – Cutting tip angle of the turning tool

Angle Bottom – Angle from flat that the insert is positioned. ( see drawing above)

The Lathe Toolholder section is defined as shown in the drawing. These values are not presently used in simulation.

Technology section has feeds and speeds associated with this tool and the target material.

Feed – Usually in units per rev, such as .006 inch per revolution

Feed Reduced – same units as feed, but used when approaching the first cut of a contour.

Speed – Spindle speed. May be in revolutions per minute (rpm), or is surface speed units such as surface feet per minute. This will vary depending on the lathe in use.

Groove tool definitions are used for Lathe grooving functions with JTS. To define a Grooving tool, NC-Tool Lib-Define Groove Tool

Enter a descriptive name for this tool type. T8 1/8 wide 1.5 deep Iscar groover

Tool number is the position within the turret at which the tool is stored

Correction D and Correction L are used to identify the machine controller, tool offset locations in which the operator has entered the tool measurements

The Groove tool section is defined per the drawing at the right above.

Radius - is the corner radius of both corners. Radius can be = 0

Width - is the distance between the corner radius centers.

Height - is the maximum cutting depth of this tool.

DZ - is the insert thickness, and is used in simulating the grooving tool

Angle Left – is the left side angle of the tool. The smallest allowed angle is 0

Angle Right – is the right side angle of the tool. The smallest allowed angle is 0.

Technology section has feeds and speeds associated with this tool and the target material.

Feed – Usually in units per rev, such as .006 inch per revolution

Feed Reduced – same units as feed, but used when approaching the first cut of a contour.

Speed – Spindle speed. May be in revolutions per minute (rpm), or is surface speed units such as surface feet per minute. This will vary depending on the lathe in use.