Tool dialog

The Tool dialog has data to define the specific type, shape and material of a tool as well as how the machine will use and store data for that tool.

Figure 5: Components of the Tool dialog.

The tool type changes the tool diagram to define different tool shapes. A description of each type's parameters starts in the "Tool Types" section on page 19.

The diagram and the necessary tool specifications change depending on the tool type selected. The shaded sections of a tool diagram illustrate the cutting surfaces of a tool while the white areas are non-cutting surfaces of the tool. If these surfaces come in contact with a part, the system will draw this contact area in red during rendering to show interference. The tool types (detailed "Tool Types" section on page 19) are divided into general groups based on the similarities of the tool diagrams and specifications. The Options checkbox is used to create more complex tools. Additional specifications (not normally required for the standard tool types) are entered in the Options tool diagram. Not all tool types have the Options setting. Detailed information on the Options tool type can be found in the "Tool Options" section on page 25.

There are three options for defining the front end tool holder assigned to a tool including Tool Holder, Custom and None. Selecting None means that the system will not use a holder for the tool. If you do not wish to display the holder when rendering the part, select this option. The Tool Holder option allows you to select from pre-defined industry standard holders, based on the Tool Holder Class set in the Document Control dialog as well as the tool size. For more information on this option see "Pre-Defined Tool Holders" section on page 26. The Custom option allows you to define your own tool holder. For more information on this option see "Custom Holders" section on page 27.

This menu specifies the material of the tool. The information selected here can be used by the Material Database to determine speeds and feeds. The default material for Mill tools is High Speed Steel.

When using a pre-defined tool holder the distance from the tool tip to the face of the holder must be set. This parameter allows the overall tool length to be the actual length of the tool. The Length out of Holder value must be less than or equal to the overall tool length; if it is greater than the tool length a gap will appear between the tool and holder.

This number entered here designates the numeric location in the machine where the Z offset amount is entered.

This number designates the numeric location in the machine where the XY offset amount for Cutter Radius Compensation is found. More information on CRC can be found starting on this page.

This number tells the control the location of a tool in a gang or slide. This is used to override the existing tool number. It refers to a carousel location or "POT" number.

This is a comment associated with each tool. It will be output in the finished code at the beginning of every operation that uses the tool. The comment is also displayed in the Tooltip for the tool in the Tool list.

Tool Types

Milling Tools - Type 1

Tools in this category have a single diameter and include Rough and Finish Endmills, Ball Endmills and Spot tools. Ball Endmills do not have a bottom corner radius specification. There is no setting for Bullnose endmills, but Rough and Finish Endmills may be given a bottom corner radius to create a Bullnosed tool. Descriptions of the Overall Tool Length, Flute Length, Cutting Diameter and Bottom Corner Radius can be found in the "Tool Specs" section on page 23.

Milling Tools - Type 2

Milling Tools - Type 3

Drilling Tools - Type 1

Drills in this category are effectively straight tools that is to say that the system sees the shank as the same size as the cutting diameter. The tools in this category include Drills, Spot Drills, Counter Sinks Taps and Rigid Taps. These tools share the Overall Tool Length, Cutting Diameter and Tip Angle specifications. Countersinks have a Flat Tip Diameter and Chamfer Height dimension which are interactive with the diameter and tip angle specified. You only need to specify the tip angle and any two of the three specifications for the cutting diameter, flat tip diameter and chamfer height. The third value is automatically calculated. Tapping tools have a Non-Cutting Tip Height and a Pitch (for metric parts) or TPI (Threads Per Inch) specification. The TPI is not shown in the diagram but is entered in a separate text entry box. Descriptions of these attributes can be found in the "Tool Specs" section on page 23.

Drilling Tools - Type 2

The only tool in this category is the Center Drill. This item includes a menu of standard tool sizes for both metric and inch parts. Selecting an entry from the menu automatically fills in the specifications for the dimensions of that tool. Any value may be manually changed if it is not exactly the tool you have. A Center Drill's specifications the include Overall Tool Length, Shank Diameter, Cutting Diameter and Draft Angle, Tip Angle and a Flute Length. Descriptions of these attributes can be found in the "Tool Specs" section on page 23. Please note that the Center Drill's Flute Length does not include the length of the tool's tip or what is sometimes referred to as the pilot length.

Drilling Tools - Type 3

This category is comprised of boring tools, i.e. standard Bores and Back Bores. These tools share Overall Tool Length, Cutting Diameter and Non-Cutting Tip Length dimensions. Back Bores have Shank Diameter and Cutting Tip Length values which are not needed by standard Bores. Descriptions of these attributes can be found in the "Tool Specs" section on page 23.

Bore and Back Bore tools use a theoretical insert tip corner as the touch off Z which is shown in the tool diagram. This part of the tool will go to the Z position entered in the drill process dialog (or Hole Wizard) for the hole depth. This is also the Z location of the tool tip in CPR. This position is programmed in the output G-code.

Roundover Tools

Roundover tools are used with a Contour process to mill rounded edges. A Roundover tool's specifications the include Overall Tool Length, Shank Diameter, Body Diameter, Top Corner Radius, Pilot Diameter, a Touch-Off to Top of Radius value and the Body Length. Descriptions of these attributes can be found in the "Tool Specs" section on page 23. The standard 3° angles off the top corner radius are a fixed value and are exaggerated in the tool setup dialog.

When creating a process using a Roundover tool, set the Top Surface Z value and subtract the tool's radius from the Top Surface Z value. The final depth should not be modified, i.e. the final depth should be the intended depth of the tip of the pilot. This is because the pilot diameter of the tool is used to evaluate the Z level to cut. This allows you to determine which part of the tool to offset.

Form Tool

Any tool that can not be created using the standard tools can be created with the form tool. The Form Tool can be used to create custom tools by drawing the profile around X0. The profile is revolved about X0 to determine the tool shape. The profile must be an open, terminated shape. Only connected geometry will be used for the tool. Select any part of the profile and Apply the profile to define the Form tool.

2D milling will offset the form tool from the geometry as if the geometry is at the top Z surface level and the tool is at the final cut depth, similar to the way the system offsets for tapered tools or tools with a bottom corner radius. Form tools are not compatible with 3D milling. For more information about tool offsets refer to the "Tool Offset" section on page 28. Please note that form tools may slow down cut part rendering, especially as their complexity increases.

These pictures illustrate the creation path for a sample form tool. The first image is the profile geometry; the second, the form tool diagram with the example tool loaded in the Tool Creation dialog; and the third image, a rendered image of the tool. Remember that for the system to load a shape as a form tool, the shape must be a selected, open, terminated shape drawn around the vertical axis.

Tool Specs

Generic Specs

The following specs can be found in the different tool types. Each tool type is described in more detail later on in this section. The names listed here can be found using the balloons feature in the measurement specs of the tools.

This is the total length of the tool to be displayed during rendering. The Tool length is usually used to specify the length a tool sticks out of the tool holder, such as how far a drill sticks out of a drill chuck.

This is the largest diameter width that a tool will cut with. Also referred to as the Main Tool Diameter.

For tools that have a rounded edge on the bottom this should be less than the Main Tool Diameter and greater than or equal to zero.

For tools that have a rounded edge on the top this should be less than the Main Tool Diameter and greater than or equal to zero.

This is the length of the tapered part of the tool. Same value as the Flute Length and is usually used in Counter Sink tools or option tool definitions.

This is the angle of the tip of the cutting edge of the tool for drilling and threading tools.

Commonly referred to as "lead in". This is the height of an extra non-cutting surface of a tool measured from the bottom of the tool. If a tool has a non-cutting surface, be sure to give the tool clearance at the floor of a pocket. This is used to accurately render the cut part, ensuring that the tool does not contact the stock.

Drill and Bore Type Specs

This value is the size of a flat tip on counter sink tools. A value of "0" will create a tool with a sharp tip. This value is interactive with the diameter and Chamfer Height.

This is the overall height of the chamfer on a counter sink tool. This value in interactive and will modify the tool diameter or flat tip diameter, depending on which last had a value entered.

For tools with a built in chamfers such as Center Drills this is the draft angle of the tool.

For parts created in metric this is the distance from one thread tip to the next.

This is the height of the tool's cutting surface from the bottom of the tool for Back Bore.

This is the height of the tool's cutting surface from the bottom of the boring bar. This is used for accurate cut part rendering, ensuring that the tool does not contact the stock.

Roundover Tool Specs

This is the smaller tip diameter below the Top Corner Radius and the smallest space the tool can fit to round two parallel edges.

This value is the length of the tool from its tip to the top of the tool radius. This is the cutting area of the tool.

This is the length of the cutting section of the tool, the 4° taper and the wall section of the tool.

Tool Options

The tools shown to the right can have custom definitions for When the Options are turned on, the diagram allows additional specifications for these tools.

Sharp Tip Diameter

The sharp tip diameter is used for tools with a taper angle. Changing the Draft Angle or Cutting Diameter will recalculate the Sharp Tip Diameter or the Flute Length.

Flute Length

The flute length will be calculated when the Sharp Tip Diameter box is clicked or typed into. Entering a value for the Flute Length will recalculate the Sharp Tip Diameter.

Hollow Tool Diameter

The Hollow Tool Diameter specifies the center diameter of the non-cutting surface of the tool tip.

Ball Endmills have a slightly different tool diagram when Options is checked. This dialog allows users to define tapered ball endmills by designating a Draft Angle and Tip Radius. The Cutting Diameter, Taper Angle and Flute Length specifications are all interactive. For example, if a Draft Angle of 10° is entered and the Cutting Diameter is changed, the system will recalculate the Flute Length in order to maintain the specified Draft and Diameter.

Tool Holder Definition

There are two options for defining the front end tool holders that will be displayed during Standard CPR or Flash CPR. The first option is using predefined holders which are based on the Tool Holder Class (the backend of the holder) selected in the Document Control dialog. The second option is to define your own custom tool holder. Each is described below.

Pre-Defined Tool Holders

The Tool Holder option allows you to select the pre-defined standard front end holder for the tool. There is an extensive library of standard mill tool holders that you may choose from. When Tool Holder is selected a menu for the type of holder is available and a rendered image of the tool is displayed. The specific holders available are based on three criteria - the Tool Holder Class (set in the Document Control dialog), the Holder Type (selected in the menu below Tool Holder) and the size of the tool. The holders are grouped by type, e.g. Shrink Fit, Collet and Rotary Clamp. If multiple holders are available you can scroll through the preview window to switch between the available holders. The holder specs will indicate how many holders are available for the current tool definition.

Basic specifications of the holder are seen to the right of the tool and holder image. The specifications shown for each holder include Holder Class, Front Length and Max Diameter.

This indicates how many holders are available for the tool within the holder class. Press the up or down arrow to cycle through the list to choose the holder to be used.

Setting the Pre-Defined Tool Holder

First you must set the tool dimensions. The specific holders available are directly based on the tool size. Once the tool is defined from the menu select the type of holder that this tool will be placed in. Depending on your selection, one or more valid tool holders will be available. Scroll through the list to find the holder you will be using. If no holders are displayed then there are no available holders for the combination of tool size and holder type specified.

Custom Holders

This option is only recommended if you need to create a custom holder shape. Clicking on the tool holder icon in the mill tool dialog opens the Tool Holder Definition dialog. Holders can be defined by a geometry profile (similar to creating a custom tool shape), by a solid model of the holder or by numeric values (Custom). By default the holder is set to None, meaning a holder will not be used. To use a geometry shape, select the geometry, select Profile and click OK. To use a solid model, select the solid, select the Solid option and click OK. The Apply To All Selected Tools option will apply the current tool holder definition to all the tool tiles currently selected. The Show Solid option will show the solid model that is currently set to be the holder. Clicking the Make Profile button will create a geometry profile from the Custom tool holder definition.