Auto Square, Dual EndStops¶
The Dual EndStop firmware update enables unprecedented precision more easily than ever before. Since day one I have never encouraged endstops be used, until now.
The Mostly Printed CNC and LowRider CNC are unique in the fact that two of the axes are powered at each end of the axis. Using this fact and the new dual endstop firmware we can now more precisely and accurately set the position of every single stepper on the machine independently. This should reliably give you repeat-ability on the order of your endstops resolution, even after powering off.
Before this new firmware update all the machines in this category relied 100% on the users build accuracy, or manual measuring. This involves setting of each axis before engaging the steppers and locking it in place. If the steppers are ever disengaged during use only the side of the axis with an endstop can accurately be accounted for. This makes fixturing, tool changes, and multi-day jobs extremely difficult to get repeatable results. A poor build or lack of axis alignment before each job will result in a non square skewed axis. A skewed axis will result in ovals and parallelograms instead of circles and 90° cornered rectangles. Changes in build accuracy due to use and environmental conditions need to be adjusted out or accounted for manually. Now just a minor offset adjustment will correct this.
Plugging In The Steppers¶
Marlin’s extruders=0 or remapping of pins is used in the firmware to allow the use of all the control boards drivers. The unused extruder driver/s are used for the extra stepper/s.
If the firmware is set for EXTRUDERS=0 then E0 becomes X1 and E1 becomes Y2. (or LR would be E0=Y2 E1=Z2)
This board only has 4 drivers available and can easily be used with the LowRider CNC but can not full take advantage of the new firmware with the MPCNC.
The min pins are used as normal for the first stepper and the max pins are used for the second stepper on that axis (X2, Y2, Z2), still as a min. For example, X1 pairs with Xmin, X2 pairs with Xmax.
DO NOT USE THE + (positive) Terminal. S & – (signal and Negative) Only
- Xmin=X1 limit switch
- Xmax=X2 limit switch
- Ymin=Y1 limit Switch
- Ymax=Y2 Limit switch
- Zmin=Touch probe. Signal pin to plate, negative to tool.
For the safest configuration the endstops should be wired in the Normally Closed position (NC), to prevent wire disconnects from damaging the machine during the homing sequence.
Mechanical endstops are connected to the signal and ground pins filtered or optical endstops use all three pins, connect these with extreme caution. Using the wrongs pins will damage your control board.
Optical endstops are not recommended on a machine used for milling or routing. The debris can inhibit there function.
Do not use the + (positive) pins or you will ruin your SKR Pro board.
Pay attention the pins are opposite each other, but clearly labeled on the board.
This board only has 4 drivers available and can easily be used with the LowRider CNC (Y axis) but can not full take advantage of the new firmware with the MPCNC.
The dual endstop firmware is on the V1 Engineering Marlin Builder page page.
Remember small 1mm moves when initially powering it up, if driving your steppers the wrong way you can rip your machine apart. If your steppers are moving the wrong direction, completely power off your board before flipping the plug over.
Testing and Calibration¶
After all the endstops have been connected issuing a
M119 command will let you see the current
status of each endstop. You should check that each endstop registers both an open and closed status
before proceeding. Open when not touching and closed when they are. You can test them individually
by closing each one by hand and running an
M119. Also verify the X1 corresponds to the X1 stepper.
Then verify a positive movement is away from the end stops.
The unfortunately designated
M666 lets you test your offset to quickly calibrate your machine. Using
M666 X0.72 would offset the X1 stepper 0.72mm away from it’s endstop, Y! can also be
used. To verify your current settings during calibration just an
M666 will show the current offsets.
Once the correct offset are found you should input them into your firmware.
This is to simplify the actual placement of the endstops themselves, you only need to get them such that the X1 or Y1 endstop is at or slightly behind where it needs to be within a few Millimeters is best.
- You can verify how square your axis is by measuring the diagonals of the largest rectangle you can draw in your build area. The larger the more accurate…but also harder to measure. I only have 6″ calipers but I was more accurate with a tape measure at my 440mm available diagonal.
- Measure the diagonals to the X1 and Y1 endstops blocks.
- Offset the endstop that has the short dimension by the amount it is short or just a hair over. So if the X1 diagonal was 1mm short you would offset X1 by 1mm. M666 X1. Tip – If it is more than 2mm off move the stop block, each belt tooth is 2mm.
- Draw a fresh one to verify. If that is correct you should edit your firmware to make this change permanent in configuration.h Or add it to all of your Gcode.
Care should be taken to use as little pen pressure as possible with the finest tip possible to get the most accurate results and a pen mount with some give should be used, example pen mount.
My trials and tribulations figuring this out….Feel free to make fun of me. Forum link.
First, most jobs will not benefit from using endstops. Getting the machine close and just running a quick one off carving or sign has no need to go through all the extra steps. People new to the CNC world should not use this, this is a advanced technique. My support for this will be limited.
You can now use the machine in two ways. Quick one off jobs as you always would setting the home position by hand and just running the job. Or by starting each job with a
G28(if using a touch plate) you can now reference or return to that position at any time. If you are not using a touch plate you can use
G28 X Y
You can use fixtures at a set reference points on the table to do repeat jobs or multiple sided cuts utilizing CAM based work offsets or scripts.
Tool changes can be done with multiple gcodes so you can do repeat jobs in order of bit used instead of per piece depending on if changing the part of the bit is the faster choice.
Jobs can be restarted in case of power outage, tool breaks, long multi day jobs, apply paint between cuts, etc.
If you don’t need the endstops you can just insert the command,
G92 X0 Y0 Z0, in your gcode before the cut starts. This should allow for normal use without homing or work offsets, also no squaring.
For more info please see the Milling Basics page.
Make sure your job has a work offset if you use the endstops.
A typical part has the gcode built with the origin at the parts corner. If you where to cut out that part it would result in going negative past your endstops and misalign your machine.
Negative moves do not work on the X and Y axis with endstops.
Moving the origin in your CAM program is the easiest fix.
To get a more precise work offset it is best to add it in your CAD file. This can be done with a bounding box, cut it as a separate path and used to position your material.