The tool icon bar on the top of the dialog displays the all various types of tools available in MILL module. Different tool types can be defined by selecting the desired icon in the dialog box.

Note: The actual tools that you will see listed in this toolbar will depend on what module and what configuration you are currently running.

The dialog box shows the tool name of the current selection if there is one selected in the list-box under Tools in Session. If there is no selection then the tool name will be the name used for a new tool definition. The list box itself lists all of the tools of the corresponding type.

Tool Representation

The icon representation of the tool shows where the dimensions listed below are measured from.  Please refer to this image when entering your tool dimensions.

Name

Enter a unique name for the tool.  Tools are defined by their Name.  You cannot have more than one tool with the same name.

Dimensions

Enter the tool dimensions using the fields provided.  It is best to have the Tool Dia. and the Shank Dia. the same dimension even if your tool is different. Shoulder Len. must be larger than the Flute Len.

Holder

If you have Tool Holders defined, select the holder that you want assigned to this tool.  To create and manage Holders select the ... button to display the Create/Select Holder dialog.

The geometry definition of the tool contains edit boxes for the diameter, corner radius, taper angle, flute length and the tool length. These definitions are standard APT parameters for the tool definition. The flute length denotes the cutting length while the tool length denotes the total length of the tool to the tool holder.

Save As New Tool  

Saves a new tool and lists under Tools in Session. If a tool of same name already exist under Tools in Session, Save as New tool button will be grayed out.

Save Edits to Tool  

Saves edits or changes made to tool parameters.

When you Save Edits to Tool, each Mop in the Machining Job tree that uses the Load from Tool option, will be updated with the new feeds/speeds for that tool automatically.

Delete Tool  

Deletes the selected tool. A tool will not be deleted a tool if is being used in a machining operation.

As the tool geometry is defined, a preview of the tool is shown in the graphics window.

The Properties tab to the right side of the tool preview allows you to set the Tool Material, the Cut Material Color (for that Tool), Number of Flutes in the tool, Tool Number, Adjust Register, Cutter Compensation Register, Axial Offset, Coolant Type. The Number of Flutes is used in Feeds & Speeds calculations. The tool number is used when post processing toolpaths.

The Cut Material Color selector will allow you to assign colors to each Cut Material created by this tool.  set a  you Save Edits to Tool, each Mop in the Machining Job tree that uses the Load from Tool option, will be updated with the new feeds/speeds for that tool automatically.

Material

This sets the material definition for the active tool.  This material is also used in the Load from File option, also referred to as the Feeds & Speeds Calculator.

Cut Material Color

You can set the cut material simulation color for this tool.  To view this color during simulations, set the Simulation Display State to Tool.  This control is located to the right of the toolbar at the bottom of the Simulate tab.

Number of Flutes

This defines the total number of flutes for the active tool.

Adjust Register

This is used to set the Tool Length Offset (an integer). Generally this is set the same as Tool Number.  The posted code would output H<#> and the # corresponds to the offset value in the controller’s tool table. Note the post processor needs to be configured to output the Adjust Register.

For example

N20 T1 M6

N30 G43 H1 Z0.25

Where H1 points to the controllers tool table for tool length compensation.

Cutcom Register

This is used to set the Tool Diameter Offset (an integer) for cutter compensation / tool wear compensation at the controller. Generally this is set the same as Tool Number.  The posted code would output D<#> and the # corresponds to the offset value in the controller’s tool table.

For example

N30 G41 X 2.0 Y 1.0 D1

Where D1 points to the controllers tool table for diameter compensation.

Note the post processor needs to be configured to output the Cutter Compensation. Refer to Cutter Compensation for detailed description.

Axial Offset

This parameter offsets the Z value in the posted g-code by the specified value. This can be set to a positive or negative value and can be an integer or decimal.

Use of Dove Tail, Fillet Mill, Lollipop cutter and User Defined tools are limited to 2½ Axis Profiling and Engraving operations.

Coolant

Here you can override the Coolant that is specified by the Tool. Coolant can be set to Flood, Mist, Through or Air. Coolant codes are defined in the post processor generator under Misc tab. Coolant Off is also supported as a variable that can be added where needed using the post-processor generator.

Comments

Outputs specified comments in the posted g-code before a tool change.

Adding $ as prefix would skip the comment start and end characters in the posted output file.

The posted code would include the comments in the output as shown below.  

Make sure comments to output is selected in your post processor.

(END MILL – 0.5 INCH)

M00

The Feeds & Speeds tab located next to Properties tab allows you to set feeds and speeds for each tool.

Refer to the Feeds and Speeds section for additional information.

Cut Depth

You can set the Cut Depth specific for each tool you create.  If you set this value here, you will see a Depth From Tool icon next to the Rough Depth/Cut parameter in the Cut Levels tab of each operation where it applies. Selecting the icon will use this value for Rough Depth/Cut. If Cut Depth is left at 0 in this dialog, the icon will not appear in the Cut Levels tab.

Taper Angle is set for VeeMill, ChamferMill and TaperMill. This angle is the included angle. For a 60 degree taper tool, the Taper Angle is set as 30.

Flat Diameter is set for ChamferMill and TaperMill. When Flat diameter is set =0, the tip converges to a point.

To define a ball mill with taper, set Flat diameter = 0 and Corner Radius = tool radius.

In the example shown below, Flat Dia = 0 and Corner Radius = 0.25. This creates a 0.5” ball mill with a 10 degree taper.