Enable 2D / 3D Cutter Compensation /

Depending on the NC procedure, one or more of these options may be available.

Using cutter compensation enables accurate hole diameters, using any milling cutter.

One of the following cutter compensation parameters is displayed (cutter compensation can either be 2D or 3D):

The Enable Cutter Compensation (2D/3D) parameter is displayed in the Machine Parameters Table.

• Parameters
• Detailed Parameter Explanations
• Invoking Geometry Location as Cutter Compensation
• List of Procedures (where each type of cutter compensation appears)
• Cutter Compensation and Post Processing Parameters

The following dropdown list options are available for the Enable Cutter Compensation (2D/3D) parameter (see Detailed Parameter Explanations for more detailed explanations with G-Code examples). In the explanations below, the following example part is used; a toolpath for this part has been programmed using the white contours as an input.

Parameters

The following cutter compensation options are available:

Depending on the NC procedure, one or more of these options may be available.

No	Do not use cutter compensation. See Detailed Parameter Explanations.
Tip Location	Cutter tip location. Create the G-Code with an offset (equal to the cutter radius) to the user contours and compensate with the difference between the actual cutter radius and the programmed radius. In the example below, the toolpath "as tool tip location" (shown below in blue) will allow the shop floor to input the difference between the diameters of the current tool and the old tool at the machine. See Detailed Parameter Explanations.
Geometry Location	Cutter geometry location. Create the G-Code on the user contours and compensate with the entire cutter radius. In the example below, the toolpath "as geometry" (shown below in blue) will allow the shop floor to simply input the diameter of the tool they are using. Note: In this example, in most areas the blue toolpath and the white input contours coincide. However, in the areas that were too small for the cutter, the toolpath is different than the input contours to prevent over machining. When the Geometry Location option is selected, an additional parameter is displayed in the Machine Parameters Table - Cutter Compensation Additional Radius: This parameter appears only with "Geometry Location" and enables an extra margin to ensure that the controller will not reach a conflict if the real tool is exactly ø10 mm (R 5.0). By default, the Geometry Location method of cutter compensation initially does not appear in the dropdown list of cutter compensation options displayed in the Machine Parameters Table. See Detailed Parameter Explanations and Invoking Geometry Location as Cutter Compensation.

Detailed parameter explanations

The following example is used to explain each of these options - milling on the right side of a straight line from X0, Y0 to X25, Y0, with a cutter of diameter 10 mm.

Sometimes the tool that was used to calculate the toolpath is not available on the shop floor. Or perhaps there is a desire to use a re-sharpened tool that has a slightly reduced diameter. Using the example above, we still want the cutting edge of the tool to mill along the line from X0, Y0 to X25, Y0. To do this the whole toolpath needs to be moved. Given the proper commands, the CNC machine controller can take the G-Code and offset the toolpath.

FANUC (and many other controllers) use the G40, G41 and G42 commands mentioned above. They work with values that are stored in the controller "D" registries in the same way as the length compensation works with the "H" registry.

• No

• Tip Location

• Geometry Location

• Invoking Geometry Location as Cutter Compensation

No

Do not use cutter compensation.

In the milling example above, the tool tip moves from X0, Y-5 to X25, Y-5. The G-Code for this will look like this:

Tip location

With this method, the machinist enters a correction value for the tool into the appropriate registry on the controller (ie: -0.1 for a re-sharpened ø10 mm tool that now has a radius of 4.9 mm).

In the milling example above, the G-Code for the same motion using Cutter Compensation - Tip Location would look the same up to N60:

In Registry D51 on the machine controller, the operator must input the corrective value; ie. the NC program was created with a ø10 mm tool in mind. But if the real tool is ø9.8 mm, the value of 0.1 must be placed in Registry D51.

Geometry location

This method of Cutter Compensation uses the desired profile of the finished piece as the toolpath, and lets the machine controller calculate the real toolpath according to the real radius of the tool.

In the milling example above, (with the approach/retract on the left) the G-Code for the same motion using Cutter Compensation - Geometry Location would also look the same up to N60:

Taking the example from above of a ø10 mm tool re-sharpened to ø9.8 mm, the value entered in Registry D51 would be the real radius of the tool: 4.9.

By default, the Geometry Location method of cutter compensation initially does not appear in the dropdown list cutter compensation options displayed in the Machine Parameters Table.

Invoking geometry location as cutter compensation

In the following example Geometry Location is selected as the Cutter Compensation method.

Selecting Geometry Location as the Cutter Compensation method

1. UseUse (for more, click Access at the top of this Help topic) the required Cutter Compensation type.

2. When invoked from the NC Utilities menu, messages are displayed informing you that all relevant procedures will become suspended except for procedures with active 3D Cutter Compensation.
   The options under NC-Utilities > Cutter Compensation are grayed out if 2D cutter compensation has never been activated in an NC file in Cimatron 10.0 and above.

3. In the Preferences > GeneralNC, depending upon the current procedure type, change the Cutter Compensation - Milling Output option or the Cutter Compensation - Turning Output option to Geometry Location (from the dropdown list).

4. In the Machine Parameters Table, change the Enable Cutter Compensation to Yes-Geometry Location (from the dropdown list).

When the Geometry Location option is selected, an additional parameter is displayed in the Machine Parameters Table - Cutter Compensation Additional Radius:



This parameter appears only with "Geometry Location" and enables an extra margin to ensure that the controller will not reach a conflict if the real tool is exactly ø10 mm (R 5.0).

List of procedures

The list of procedures where each type of cutter compensation appears, is shown below.

Cutter compensation and post processing parameters

All compensated motions are linear. The post processor supports the cutter compensation vectors using SRF_NORX, SRF_NORY and SRF_NORZ as variables.

The touch point is available as parameters to the post using SRF_TOUCHY and SRF_TOUCHZ.

The post parameter COMP_3X (default = false) assumes true on approach, milling passes, retract and "On Surfaces" connections.