Tool Table
4.1 Tool Table
Overview
When the MILLPWR
G2
runs a program step that activates a tool, it only activates the diameter, and length values on that row of the Tool
Table. The tool number, or tool type are not activated in dialogues that have these fields. The tool type must be entered in the dialogue.
Tool Table values are automatically converted to their inch or millimeter equivalents when the MILLPWR
G2
mode is changed. All typed values must match the current unit mode of the MILLPWR
G2
.
Define and store up to 99 tools on the tool table. Type of data stored on the Tool Table is information specific to each tool. Diameter, and length offset are the only values used from the Tool Table.
The Tool Table can only be used with G-code programs.
Tool Compensation Required Data
You usually program the coordinates of path contours as they are dimensioned on the work piece drawing. To allow the MILLPWR
G2
to calculate the tool center path, e.g. the tool compensation, you must also enter the diameter of each tool you are using.
Tool data can be entered either directly in the part program or separately in the Tool Table. In the Tool Table, you can also enter additional data for the specific tool. The MILLPWR
G2
will consider all the data entered for the tool when running the part program.
44
4 Tool Table
Tool numbers / Tool names
Each tool is identified by a number between 0 and 99. The tool name is its tool number.
The tool number 0 is automatically defined as the zero tool (empty spindle) with the length L=0 and the diameter D=0.
Sign for the length difference
Δ
L
If the tool is longer than the T1 tool:
Δ
L > 0 (+).
If the tool is shorter than the T1 tool:
Δ
L < 0 (–).
The tool length offset can be entered as a known value, or use the
Teach
soft key. The MILLPWR
G2
can determine the offset automatically.
The tool length offset may be entered as a known value, or the
MILLPWR
MILLPWR
G2
G2
may determine the offset automatically. To have the
determine a tool’s length offset involves touching the tip of each tool to the part’s Z0 surface, and pressing the Teach soft key.
This provides information to the MILLPWR
G2
to determine the tool length offset for each tool.
Tool Diameter “D”.
Enter the tool diameter ”D” directly.
The Tool Table should not have any tool length for a tool that is not repeatable.
Locating the Tool Table
The Tool Table is accessed from the DRO setup screen.
To activate the tool table, press the SETUP key.
Then press the Tool Table soft key.
ACU-RITE MILLPWR
G2
45
Tool Table
Editing the tool table
When the tool table is open, a new tool can be added, or an existing tool can be edited by changing the existing information for that tool.
It is necessary to first select the unit of measurement before entering values into the tool table.
To enter a new tool, a blank numbered row will need to be selected.
Using the ARROW keys, highlight the next available blank row number.
Highlight the Diameter field, and using the numeric keypad, enter the tool diameter.
Press the ENTER key.
Arrow over to the next field and enter the tool Length if it is to be used.
Press the ENTER key.
Arrow over to the Type field and press the ENTER key. The Type is only for informational purpose.
From the drop down menu, arrow down to select the description of the tool that is being added (e.g. flat end mill).
Press the ENTER key.
Continue to add additional tools as necessary.
When all tools have been added, press the Exit soft key, or USE key to save changes to the tool table.
Press the Teach soft key. The MILLPWR
G2
calculates the tool length offset for the selected tool putting the data to the length column.
Additional data can be input such as Diameter Wear,
Length Wear and Plunge Angle. These fields are not required to use the tool selected. See the Tool Table
Structure on the following page.
46
4 Tool Table
Editing an existing tool
To edit an existing tool is similar to adding a new tool using the same dialogues.
Highlight the desired field of the tool to be changed.
Type in the new value, then press the ENTER key.
When all changes have been made, press the Exit soft key, or USE key to save changes to the tool table.
Only add the tool diameter and length if it is repeatable each time it is selected.
When running G-code programming, the tool length for each tool in the program is provided from the tool table. As an example, T1 M6 prompts the operator to load tool 1 into the spindle. The tool length and diameter offset are retrieved for tool #1 in the tool table, and used to adjust the tool path and Z axis position. This is repeated for each tool used.
Tool Table Structure
Tool table: Standard tool data
Abbr.
Tool
Inputs
Number by which the tool is called in the program (e.g. tool 2 = T2).
Diameter
Length
Type
Compensation value for the tool diameter D.
Compensation value for tool length L.
D. Wear
Tool type: A popup menu appears where you can select the type of tool being used.
Tool diameter wear value.
(Only used in G code programs)
L. Wear
Plunge Angle
Tool length wear value.
(Only used in G code programs)
Angle of plunge cut.
(Only used in G code programs)
ACU-RITE MILLPWR
G2
47
4.2 Tool Data
Tool-Length Offsets
Tool-length offset is the distance from Z0 Machine Home to the tip of the tool at the part Z0 (the surface of the work).
Tool-length offsets allow each tool used in the part program to be referenced to the part surface. In an idle state, the MILLPWR
G2
does not have a tool-length offset active. Therefore, Tool #0 (T0) is active.
When T0 is active, all Z dimensions are in reference to the Z Home position. When you program T1, all Z dimensions become referenced to the surface on which the tool-length offset of Tool #1 was activated.
For machines that do not have a Z axis automatic homing feature, you must set the Z0 position of the Z axis. Usually, it is the fully retracted
(Up) position of the quill or machine head. Tool-Length Offsets are referenced to this position.
Because tools differ in length, Z0 axis (Part Zero) is not set the same way as X0 or Y0. The tool-length offset is the distance from the tip of the tool to the top of the part. Enter a length offset for each tool in the
Tool Table.
With tool-length offsets active, the Z axis position display reads 0.00 when the active tool moves to Part Zero. Tool-length offsets simplify programming.
Teaching Tool Length Offsets in the Tool Table
The Tool Length Offset data is placed in the “Length” column in the
Tool Table.
Activate the Tool Table by pressing the SETUP key from
DRO
mode.
Then press the Tool Table soft key.
Select the tool number that is to be edited.
Use the arrow keys to highlight the “Length” column field.
With the tool in the spindle, move the tool down until it touches the top surface of the work piece. This is referred to as “Part Zero”.
Press the Teach soft key. The MILLPWR
G2
calculates the tool length offset for the selected tool putting the data in the length column.
48
4 Tool Table
Diameter Offset in Tool Table
When you activate a tool, you automatically activate the length offset and diameter values recorded on the Tool Table (DRO mode only activates a tool when GO is pressed). When a tool is activated, the length offset is applied immediately to provide an accurate Z axis position display.
The active diameter value is important when you program compensated moves and use cycles with built-in tool compensation.
If tool diameter is correct, compensated moves and cycles are performed accurately.
Enter tool-length offsets and tool diameter values on the numbered lines of the Tool Table. The numbered lines on the Tool Table identify the tool number (T-Code) that activates those values.
On machines equipped with collet-type tool holders, it is impractical to use the Tool Table to store tool-length offsets. You can set tool-length offset at tool change. Tool Table diameters are still required for compensated moves and when using cycles that have built-in compensation.
ACU-RITE MILLPWR
G2
49
Tool Radius Offset
Tool radius offset is available with the MILLPWR
G2
. The tool center moves in the working plane along the programmed path or to the programmed coordinates. When programming a part profile, the path of the tool is a half of a diameter away from the depth of the cut.
Offset the tool to the right-hand or left-hand of the cutting edge.
“Right” or “Left” refers to the side of the cutting edge to which the tool offsets. Program tool offset as Right or Left according to the desired cutting edge.
Moving without radius offset
The tool center moves in the working plane along the programmed path or to the programmed coordinates. Program tool offset as Center when no radius offset is needed.
Applications: Drilling and boring, pre-positioning.
50
4 Tool Table
Machining with radius offset
The tool center moves along the contour at a distance equal to the radius. “Right” or “left” are to be understood as based on the direction of tool movement along the work piece contour as viewed from behind a moving tool.
ACU-RITE MILLPWR
G2
51
Radius offset: Machining corners
Outside corners:
A programmed path around the outside corners on a transitional arc should have the feed rate at the outside corners reduced to relieve machining stress. Typical for any great changes of direction.
Inside corners:
The operator must program the MILLPWR
G2
for the intersection of the tool center paths at inside corners. From this point it then starts the next contour element. This prevents damage to the work piece.
The permissible tool radius, therefore, is limited by the geometry of the programmed contour.
Danger of collision!
To prevent the tool from damaging the contour, be careful not to program the starting or end position for machining inside corners at a corner of the contour.
52
4 Tool Table
