Warning
The current version of MillMage is a Release Candidate — a stable version of software that is nearly ready for official release, but in need of additional public testing. Please report any unexpected behavior in the MillMage Software Questions section of our forum, including screenshots and as much detail as possible. Ask hardware compatibility questions in the MillMage Hardware Compatibility section.
Users new to MillMage should follow the Getting Started guide.
Video: How to Use a Release Candidate
This video features our sister software, LightBurn. While there may be slight differences in appearance and layout, the demonstrated processes are similar in MillMage.
Warning
This documentation is in active development and in a prerelease state. These documents are not complete and may include missing pages, broken links, and placeholders. Content is being updated as feedback is reviewed. Your patience is appreciated.
Tool Length Probing
This guide covers using a Tool Length Probe with the Probing Wizard to automatically calculate the length of an installed tool to determine and apply the tool offset needed to maintain the project Z axis zero point.
Using a probe to do this isn't strictly necessary for basic CNC work – you can manually re-zero your Z axis zero after changing a tool, but probing can perform that process automatically, and more quickly.
A tool length probe is especially helpful when a project's Z Axis Zero Point is set to Top and has been machined away during previous operations, and can aid in project recovery when the spindle, router, or tool has slipped and been re-secured, but potentially in a different position.
To follow this guide, you'll need a CNC machine with a tool length probe located within the travel area of the machine. The probes may be built into the machine or may need to be installed as a separate accessory. Refer to and follow your CNC manufacturer's instructions when installing a tool length probe.
How Tool Length Probing Works¶
Tool length probes vary in type, location, and material, but typically work the same: your CNC will jog/move over the position of a probe in your CNC's work area, then lower the tool until it makes contact with the probe, sending a signal to the machine's controller to calculate and establish the new tool Z axis zero point.
Setting Up a Tool Length Probe¶
Set the position and motion parameters of your tool probes in the Probe Configuration window. If you have already defined your probing settings, you can skip ahead to Activating Tool Length Probing.
1. Find the X and Y Axis Tool Length Probe Location¶
Use the Move Window to determine the tool length probe location.
Warning
Make sure that before you start probing for tool length that the spindle or router collet is tight and the tool secure. The spindle or router must be off and not rotating.
- Close the Probing Wizard if open
- Select the Move Window
- Use the jogging buttons to move and roughly center the tool above the probe location
- Note the machine X and Y Axis coordinates in the Move Window, labeled Tool Position (M)
2. Open Probe Configuration Window¶
Open the Probe Configuration window to define the parameters of your tool length probe by selecting either:
- CNC Tools → Probe Settings
- CNC Tools → Probing Wizard → Manage Probe Configuration
- Move Tab → Probing → Manage Probe Configuration
CNC Tools Menu
Move Tab/Window
3. Update Settings¶
Select Tool Length Probe to open the Tool Length Probe settings panel.
Position X and Position Y¶
- Position X is the location in machine coordinates of the tool length probe along the X axis (left/right).
- Position Y is the location in machine coordinates of the tool length probe along the Y axis (towards/away).
Search Z¶
Search Z is the maximum distance the tool will move downward when seeking the tool length probe.
The tip of your tool must be within this distance from the top of the tool length probe activation point when you start the probing process. Measure the distance between the tool and the tool length probe, adding a small percentage of the measured value — like 10 mm — as margin to allow for tool length probe microswitch travel.
Fast Probe Feed and Precise Probe Feed¶
- Fast Probe Feed is the initial speed at which the tool will search for the tool length probe. This can be fairly fast, depending on your risk tolerance.
- Precise Probe Feed is the lower speed at which the tool will search for the probe after initial contact. This movement will be a very short distance and should be kept to a fairly low speed for accuracy.
4. Save Settings¶
Select Okay to save the settings. Select Yes if prompted, to overwrite the previous Tool Length Probe Custom GCode entry in Device Settings. The Probe Settings window will close when saved.
Activating Tool Length Probing¶
Warning
Make sure that before you start probing for tool length that the spindle or router collet is tight and the tool secure. The spindle or router must be off and not rotating.
1. Ensure Spindle or Router is Powered Off¶
Always power off your CNC router or ensure that the spindle is not rotating before executing the probing process. An active spindle or router tool can damage the tool length probe, the tool, and machine and can lead to personal injury.
2. Install Desired Tool¶
Install the desired tool into the CNC router or spindle, ensuring that the collet has been tightened enough to securely hold the tool.
If the CNC router or tool is not securely installed, the Tool Length Probing process may fail or the tool may move, leading to inaccurate results.
3. Verify Probing Distance¶
The tip of the tool must be within the user-set Search Z value of the probe trigger point. Check the distance between the tip of the installed tool and the approximate trigger point of the Tool Length Probe. Use the Jogging controls in the Move window to move the tip of the tool closer to the tool length probe if necessary.
Alternatively, you can change the Search Z value in the Tool Probe Configuration window, or manually edit it in the Tool Length Probe value in the Custom GCode tab of the Device Settings window and reopen the Probe Wizard.
Updating the Z Axis Search Distance in Custom GCode
Update the Tool Length Probe Z Axis Search Distance manually by adjusting the Tool Length Probe value in the Custom GCode tab of the Device Settings window, on the line starting with:
G38.2 Z-YourValueHere F600
4. Open Probing Wizard¶
Open the Probing Wizard by selecting CNC Tools → Probing Wizard, or by clicking the Probing button in the Move window.
CNC Tools Menu
Move Tab/Window
5. Select Tool Length Probe¶
Click on Tool Length Probe to open the Tool Length Probe window.
6. Start Tool Length Probing¶
Check that the CNC machine tool is within the Z axis probing distance displayed in the Tool Length Probe Window.
If the tool needs to be repositioned along the Z axis, close the Probing Wizard and move the tool using the Move window, or select Previous to return to the Probing Wizard and select Mange Probe Configuration to update the Search Z distance.
Once the tool is within the Search Z probing distance, select Execute Tool Length Probe.
7. Monitor Probing Process¶
Once executed, the Probe Wizard will automatically:
- Move the tool to the user-defined probe location along the X and Y Axes
- Home the Z Axis
- Move the tool down the user-defined Search Z distance at the Fast probe feed speed on the Z axis until the probing switch or sensor is triggered
- Move the tool up away from the probe
- Approach the probe again, this time at the slower Precise probe feed speed until the probing switch or sensor is triggered
- Set the new Z Axis zero point
8. That's it!¶
You are now ready to run the operations in your project that use the tool you installed. Check the operations listed in the Operations window and turn on related operations that match your installed tool and turn off the remaining entries that do not match. Remember to run the Tool Length Probe again after each additional tool change within your project.
Related Topics¶
For more help using MillMage, please visit our forum to talk with MillMage staff and users, or email support.