Tool Compensation

Using the Touch Off Screen in the AXIS interface you can update the tool table automatically.

Typical steps for updating the tool table:

The Tool Table will be changed with the correct Z length to make the DRO display the correct Z position and a G43 command will be issued so the new tool Z length will be in effect. Tool table touch off is only available when a tool is loaded with "TnM6".

The G10 L1x command can be used to set tool table offsets: (these are just quick summaries, see the gcode section for full details)

G10 L1 P(tool no.) - Set offset(s) to a value. Current position irrelevant. (see [sec:G10-L1_] for details)

G10 L10 P(tool no.) - Set offset(s) so current position w/ fixture 1-8 becomes a value. (see [sec:G10-L10] for details)

G10 L11 P(tool no.) - Set offset(s) so current position w/ fixture 9 becomes a value. (see [sec:G10-L11] for details)

In general, the new tool table line format is:

The file consists of one opening semicolon on the first line, followed by up to a maximum of 56 tool entries.
[Although tool numbers up to 99999 are allowed, the number of entries in the tool table, at the moment, is still limited to a maximum of 56 tools for technical reasons. The EMC2 developers plan to remove that limitation eventually. If you have a very large toolchanger, please be patient.]

Earlier versions of EMC2 had two different tool table formats for mills and lathes, but since the 2.4.x release, one tool table format is used for all machines. Just ignore the parts of the tool table that don’t pertain to your machine, or which you don’t need to use.

Each line of the tool table file after the opening semicolon contains the data for one tool. One line may contain as many as 16 entries, but will likely contain much fewer.

The units used for the length, diameter, etc., are in machine units.

You will probably want to keep the tool entries in ascending order, especially if you are going to be using a randomizing tool changer. Although the tool table does allow for tool numbers in any order.

Each line may have up to 16 entries. The first two entries are required. The last entry (a remark or comment, preceded by a semicolon) is optional. It makes reading easier if the entries are arranged in columns, as shown in the table, but the only format requirement is that there be at least one space or tab after each of the entries on a line and a newline character at the end of each entry.

The meanings of the entries and the type of data to be put in each are as follows.

The “T” column contains the number (unsigned integer) which represents a code number for the tool. The user may use any code for any tool, as long as the codes are unsigned integers.

The “P” column contains the number (unsigned integer) which represents the pocket number (slot number) of the tool changer slot where the tool can be found. The entries in this column must all be different.

The pocket numbers will typically start at 1 and go up to the highest available pocket on your toolchanger. But not all toolchangers follow this pattern. Your pocket numbers will be determined by the numbers that your toolchanger uses to refer to the pockets. So all this is to say that the pocket numbers you use will be determined by the numbering scheme used in your toolchanger, and the pocket numbers you use must make sense on your machine.

The "Data Offset" columns (XYZABCUVW) contain real numbers which represent tool offsets in each axis. This number will be used if tool length offsets are being used and this tool is selected. These numbers can be positive, zero, or negative, and are in fact completely optional. Although you will probably want to make at least one entry here, otherwise there would be little point in making an entry in the tool table to begin with.

In a typical mill, you probably want an entry for Z (tool length offset). In a typical lathe, you probably want an entry for X (X tool offset) and Z (Z tool offset). In a typical mill using cutter diameter compensation (cutter comp), you probably also want to add an entry for D (cutter diameter). In a typical lathe using tool nose diameter compensation (tool comp), you probably also want to add an entry for D (tool nose diameter).

A lathe also requires some additional information to describe the shape and orientation of the tool. So you probably want to have entries for I (tool front angle) and J (tool back angle). You probably also want an entry for Q (tool orientation).

A complete description of the lathe entries can be found in the lathe section of the user manual ([cha:Lathe-Specifics]).

The “Diameter” column contains a real number. This number is used only if tool radius compensation is turned on using this tool. If the programmed path during compensation is the edge of the material being cut, this should be a positive real number representing the measured diameter of the tool. If the programmed path during compensation is the path of a tool whose diameter is nominal, this should be a small number (positive or negative, but near zero) representing only the difference between the measured diameter of the tool and the nominal diameter. If cutter radius compensation is not used with a tool, it does not matter what number is in this column.

The “Comment” column may optionally be used to describe the tool. Any type of description is OK. This column is for the benefit of human readers only. The comment must be preceded by a semicolon.

EMC supports three types of tool changers: "manual", "random location" and "fixed location". Information about configuring an EMC tool changer is in the Integrator Manual.