V2 Series Tool Length Offsets (Kinetic Control)

Owned by Matt Rounds (Unlicensed)
Last updated: Mar 11, 2024 by Q Rothing
7 min read


Revision History

First Release: November 2021 (MR)

This tutorial uses the Kinetic Control user interface released on 11/1/2021; if you are using the old user interface, please refer to the original version of this tutorial posted under “Legacy Resources”

Section 1: Tool Length Offset Definition

The tool length offset (TLO) is the distance between the Z home position and the machine home when the tip of the tool is a specified distance from the B table. Basically, this tells the Pocket NC where the tool is in space so that the correct compensations can be made to the program in order to cut the part successfully.

The Pocket NC V2 is equipped with a tool probe that will automatically measure the tool length offset for most tools. However, some tools will still have to be measured by hand. This tutorial will explain how to use the automatic tool probe as well as how to measure the tool length offset by hand.

Section 2: Tool Change

Section 2.1: V2-10 Tool Holder Change

  1. Turn off spindle and loosen the (3) spindle screws using the 3mm wrench.

  2. Tap spindle holder with the back end of the 3mm wrench and take out the tool holder.

  3. Reverse process for installing a new tool holder, being sure to tighten the (3) spindle screws incrementally.

Section 2.2: V2-10 Tool Change

  1. Use the Pocket NC spindle wrench and the 3mm driver, both are found in the tool kit.

  2. Turn off spindle and place the 3mm driver into one of the 3 spindle screws.

  3. Using the Pocket NC spindle wrench loosen the collet nut while holding the spindle in place using the 3mm wrench.

  4. Change out or move the tool and then reverse the process to tighten the tool into tool holder.

  5. Remember to adjust or remeasure the tool offset after changing or adjusting a tool.

Section 2.3: V2-50CHB Tool Change

  1. Rotate the spindle lock lever to the “OPEN” position (towards the front of the machine).

  2. Remove the tool and insert the new tool with the same diameter shank.

    1. If using a tool with a different diameter shank, the collet will also need to be swapped. Only install or remove the collet while the lever is in the “OPEN” position and while a tool is inside the collet (to prevent the collet from collapsing). Use the small wrenches provided to hold the end of the spindle still and unscrew the collet. Insert a tool in the replacement collet and repeat in the reverse order to seat the collet.

  3. Rotate the spindle lock lever to the “LOCK” position to tighten the collet and secure the tool.

  4. Remember to adjust or remeasure the tool offset after changing or adjusting the tool.

Section 2.4: V2-50CHK Tool Change

  1. The 12mm and 14mm wrenches provided with this spindle option will be needed.

  2. Use the 12mm wrench to hold the spindle in a fixed position and use the 14mm wrench to loosen the nut at the end of the spindle next to the tool.

  3. When loose, pull out the nut, collet, and tool assembly, then pull out the tool.

  4. If switching shank sizes, pop out the old collet and snap in the new collet. (There is a snap feature on the collet that will only snap into/out-of the nut if no tool is present).

  5. Insert the new tool into the collet and nut assembly.

  6. Use the wrenches to tighten the nut assembly back onto the spindle.

  7. Remember to adjust or remeasure the tool offset after changing or adjusting the tool.

Section 3: Using the Tool Probe

Section 3.1: Tool Measurement

Do not run the probe cycle for any tool sticking out more than 1.5 inches from the end of the extended tool holder with a V2-10. On any machine, do not use the probe cycle for any tool with a diameter greater than ¼ inch. Doing so will cause a crash and may result in damage to your machine and/or a broken tool. 

Ensure that the machine is connected, powered on, and has been homed. The TOOL OFFSETS table is found under the SETUP tab on the Kinetic Control user interface.

The TOOL OFFSETS table is where all tool information will be stored. The “T#” column is the tool number, and the “TLO” column displays the tool length offset that is set for that tool. All the tools are set to 5.000 inches by default before being measured. The “Diameter” column displays the tool diameter and the “Flutes” column can be edited to list the number of flutes (the default is 1). Note that the diameter is the diameter of the cutter not the diameter of the shank and all the tools are preset to 0.125 inches by default. The user can add a description of the tool in the “Description” column.  

The “Diameter”, “Flutes”, and “Description” columns are just for you to add information for yourself. They will have no effect on the machine function and do not need to be filled, but filling in the details is the best practice for commonly used tools. The TLO field will need to be updated any time the tool’s position in the holder is changed (this can be done manually or by measuring the tool using the steps below).

Click on the green probe icon for the tool that you wish to measure and set the tool length offset.

The machine will move the X-axis towards the front of the machine to the tool loading position and the green button on the front of the machine will begin to blink. A notification will also pop up in the lower right hand of the UI reminding you to load a tool. If you haven’t already, install the tool you wish to measure. Make sure to fully tighten the holder as previously described.

When ready, press the green button on the front of the machine to initialize the probe sequence. The machine will automatically reposition and measure the tool length using the tool probe button on the side of the B-table housing.

The probing will begin with Z retracting to a safe distance, X moving to align with the probe, and then Y will raise to align the probe. After that, Z will advance until it triggers the tool probe button. It will then retract a short distance, and then approach at a lower speed until the button triggers again. Finally, the machine will return to the position it was in when the the cycle was started.

 After the probe cycle has finished, the tool length offset will be updated in the tool table.

Section 4: Measuring Tool Length Offsets by Hand

If the automatic tool length measurement probe cannot be used for a tool, you can measure the tool length offset by hand.

You will need to know your machine’s B Table Offset. This is the distance from B Table to Center of A axis rotation.  This number is 0.8xx inches. This value changes for each machine and is written in the back of the Quick Start Guide that is included with each machine.  If you have misplaced yours, please email us at info@pocketnc.com and we can find it for you.

You will also need to have a 1-2-3 block. These are available through Amazon as well as many other vendors. Any precision machined or ground 1-2-3 block will work for this procedure. 

  1. Home machine and remove any fixturing and components from the B-table

  2. Clear any offsets in the SETUP tab, WORK OFFSETS section, by clicking the “G54” dropdown and selecting “Clear Current System”:

 

 

3. Move the A table to 90 degrees using the command “g90 g0 A90” within the MDI command window on the “MANUAL” tab of the UI and hit the enter key:

4. Clean off any debris on the B-table. Hold the 1-2-3 against the B-table with the long edge of the block parallel to the tool. Make sure that the 1-2-3 block is flush with the B-table and that you have it against center part of the B-table (the raised part that rotates), not the B-table housing (the part that doesn’t rotate).

5. Jog Z in the negative direction until the base of the tool is close enough to the B-axis table that the 1-2-3 block will not fit between the two.

6. In increments of 0.01 inches or less, jog the Z axis positive until the 1-2-3 block slides between the tool and the table.

7. Repeat this step with smaller increments until the tool position is measured past 3 decimal places.

8. Use the current Z position on the digital readout (DRO) in the user interface to calculate the tool offset using the equation below:

            -(1-2-3 block height) + (B table distance “above”) + (Z value readout)  = (Tool Offset)

Example     -(3.000)+(0.8861)+(-0.9131)=(Tool Offset) = (-3.027)

 

 

9. Input the calculated Tool Offset in the TOOL OFFSETS table of the SETUP tab for the appropriate tool. Click in the appropriate box in the “TLO” column (based on the tool number). Type the tool offset that you calculated and be sure to hit the ENTER key on your keyboard. Make sure that the sign is correct. Update the tool diameter if needed.