Setting Tool Lengths with the Touch-Off Plate

There are a number of ways to use the Touch-off Plate. This guide will go through the most basic method, for Z-offsets only. The idea here is that we use the probe to establish the top surface of the touch plate as the Z-zero plane. We then call up each tool and move the machine until the tool tip breaks this plane.

NOTE: Make sure you have the latest DWC files installed (the zip file found here), and upload the necessary routines, specifically touchoff_z.g to your machine.

First, attach and connect the touch-off plate. 

Mechanical attachment on the print bed is achieved with the outer-most screw positions. (Other holes are for use with other setups such as the dovetail bed or rotary vise). Tighten the screws finger-tight so that the touch-off plate is firmly clamped to the bed.  Use M3x16mm screws to fasten the touch-off plate to the bed.

Connect the 3-pin connector to the mating connector on the back of the base of the machine (behind the X-bellows):

If you plan to leave the cable in place when the touch plate is not in use, make sure you route it along the back of the base casting so that the X-bellows covers do not scrape across it (as shown below). It is not recommended that you leave the touch plate attached to the bed when running the machine, especially during milling cycles.  Chips and dust will interfere with proper function of the device.

Confirm that the "E4_STOP" LED is ON, then turns OFF when pushing the pin of the touch-off plate:  The LED will be in the electronics box behind the tablet.  There is a single latch holding it down on the right side of the machine.

In the "Offsets" page, the TouchoffZ button will run the Z-axis down until the touch-off plate is hit (or a maximum of 10mm, whichever comes first).

To get started using the touch plate to set your tool offsets, follow this procedure:

Note: Before trying to find the tool length of any of the FDM Extruders, make sure that the nozzle is clean and the tip is free of any filament.

1. Call up the Touch Probe (T10)
2. Jog the machine in xyz until the probe is centered and approximately 5mm above the touch-off plate stud (Note: when you are in the offsets page, you can bring up the jog interface by clicking "show jog buttons" in the top right corner of the screen)
3. Now that the probe is positioned above the touch plate, click TouchoffZ to bring the probe down until it makes contact with the touchplate. The purpose here is to define the location of the touch plate with respect to the probe because all tool offsets are defined in reference to the "probe zero."
4. In offsets page, activate an unused Work Coordinate System (59.3 in example) by clicking the button on the right side of the row.
5. Adjust the Z offset of this WCS so that the current Z-position of the machine is 0.00 (Note: if you start with a value of zero in the z-offset for this WCS, you can just copy the probed height into the z-offset to get to Z=0.00)
6. Jog machine up to a safe height (+50mm) and call up the tool to be calibrated
7. Jog machine in xyz so the tool is centered and approximately 5mm above the touch-off plate stud. If additive tool, make sure nozzle is completely clean where it will contact the pin
8. Run TouchoffZ probe cycle If the tool head is not moving down, check the touch-off plate probe to make sure it is not stuck and then try again.
9. In Offsets page, right click on the value of the z-offset for the current tool and set that current value to 0
10. Click on Set to Current Value (Located on the far right of the z offset value) to save the current value as the Z-offset for the specified tool.
11. Verify that the Z position should be at 0.00.  And jog the machine up to a safe height before swapping to any other tools.
12. Repeat for any other tools to be set
13. Jog to safe height
14. Remove touch-off plate
15. Return to previous WCS (generally G54)

Setting Tool Lengths without the Touch-Off Plate

This video details how to set tool length offsets:

Setting tool length offsets is critical to achieving accurate parts and also to preventing crashes into the build surface. This process is done mostly in the Offsets tab of the H-Series Control interface, by controlling the Z value of the tool offsets.

Procedure:

1. Ensure that you have the Additive print bed installed on the printer.
2. Press Home All and Home Z from the Machine Control tab. This will ensure that the Probe is zeroed on the bed. Then navigate to the Offsets page.
3. Click on the tool you would like to set the offset for (in this case, Tool 1), so that the turret moves that tool into the active position. Click on the Z-offset value for the tool and set it to 0.0

3. From the Machine Control page, move the Z-axis down until the tool just contacts a shim of known thickness, or until the tool barely contacts the print bed.
4. In the Offsets tab, set the Z position of the tool to the negative value of the Z-axis. (So if the tool is in contact with the bed and the Z axis position is 9.5, then type -9.5 in to the Z offset for that tool). If you use a shim to find the Z position, then subtract the shim thickness from the Z axis position, and type the negative value into the Z-offset. 

Note: The effect of this will be immediate - so the tool Z-axis position should be correct after typing in the offset. (That is, if the tool is in contact with the bed, the Z-axis position will be 0.0. If a shim was used, the Z-axis position will be the thickness of the shim.)

Repeat this process for all tools.