This has happened a few times: My machine, not an OX but my own build using OpenBuild parts, is behaving erratically. Controller: Chinese all in one board, 4x170oz steppers. 2.2kw Chinese spindle with VFD Cutting area 840x780mm Design in Sketchup CAM with Sketchucam Machine control with Mach3 Belts recently retensioned. No play in gantry. If I run the code with the spindle above the wood, everything tracks perfectly, so no gcode issues. Cutting Birch Ply 18mm, Spindle speed 18000rpm, X&Y at 2000mm/min (80ipm). Cutting depth 2.5mm per pass. Cutter is a 6.35mm compression bit from Amana. So what happened: First three 'laps' of the cut following perfectly. At 7.5mm cutting depth, the spindle just goes completely off course per the pic. No obvious change in noise of steppers or spindle. So, I carefully reset the position to the start point and rerun the code from scratch (after PC reboot). Spindle perfectly tracks the previous cut, then on the 4th lap, does exactly same thing in almost the identical place. What I do know: Cutter is probably not as sharp as a new one I had cut another shape to full 18mm depth (in 2.5mm) steps slightly earlier, followed by a 1mm closer full depth cut to clean the edge. No problems. Being plywood, alternating grains will mean unlikely that the bit grabbing the grain Cut where it happened is a sweeping left curve going from across the surface grain into the line of the grain. All motors felt cool to touch Please tell me how I am getting it wrong. I am very elementary in my use of Mach3. Know enough to make the cut, is there a way to see an error log. does it get feedback from the control board or the steppers if an error occurs? Thanks for your input.
Hi Dave, I have seen some similar issues to this before and it could be caused by a variety of different reasons. Perhaps as a first step you should check with licensing http://www.machsupport.com/contact-us/ to verify that the license you are using is truly a genuine Mach3 license. (Quite a few people have been sold a fake (or pirate) Mach3 license, believing it to be genuine). Tweakie.
Interesting. Would Mach3 without a proper licence do a random act of vandalism on my workpiece? I am pretty sure my key is genuine, but will check.
unlicensed Mach3 limits the number of lines it processes, so if it is getting to the limit it should just stop processing, not go off randomly. I am thinking that vibration might be causing the Y axis to go into oscillation, thus preventing the steppers from taking the next step. your steppers running cool tells me you could increase the current a little for more torque at speed. or you could reduce the number of microsteps, this also increases torque and also changes the active resonance bands for the motors. running at 80ipm means you may be running fast enough to be getting into the torque falloff area of the torque curve on the steppers. the faster they go, the less torque they produce. to counteract this, either slow down, or reduce cut depth. reducing cut depth is the better option since it is better to maintain the cut depth per tooth for the rpm being used. in fact, following the high speed machining principles, you could reduce cut depth 'a lot' and increase feed 'a lot' for the same overall time to cut. note that due to the angle of the cut neither axis is actually doing 2000mm/min, that speed is maintained on the diagonal. thus the Y is doing a lower speed which may be putting it into a resonance band. however, you would hear that clearly! compression bit - could it be getting clogged at that depth? where does the compression portion start? is the cut depth per pass a multiple of the plywood layer thickness? I am thinking you could be getting all of the current cut in a single grain direction layer, thus producing a lot of side force (to the left) on the bit. so, those are my thoughts, would love to know what it really is (-:
Thanks David Very interesting points. The error was happening at line 800 odd, so not the licence and I have done lots of bigger files. The ply are 1.5mm thick so always cutting more than one ply at a time. Bit is not getting clogged, dust extraction keeps the kerf pretty clear. My table is very solid, the way it is bolted to the heavy table makes the platform strong. Any vibration/resonance is in the gantry itself. I tried at 250ipm previously on 1mm cut depth but 90deg corners were getting rounded and losing a little accuracy. Caused quite a lot of tremor in the gantry on direction changes. I will increase the current to the steppers. I remember they were not set on maximum. I will also reduce the microsteps, which note to self will mean changes in the steps config in Mach3. Will then try both a slower same depth and faster shallower cut and see what the outcome is.
There is a code for that (-: G61 sets absolute stop mode, where it will go exactly to the programmed point. right now you are in G64 mode, where it tries to curve through the corners to keep the speed up, so called constant velocity mode. Cannot recall if Mach can take a parameters for G64, LinuxCNC accepts G64 P0.5 for example in mm mode, to set it to stay within 0.5mm of the programmed point. ok, googled it, Mach does not take parameters for G64 cool
So made some progress on solving my problem. Changed the steps from 1/16 to 1/2. Tried single step but that was noisy and missing steps. I also pushed the power from 75% to 100% on the dip switches but the motors went from running cool to running quite hot very quickly, so took the setting back to 75%. I also found this which I thought was worth sharing: Microsteps/full step Holding Torque/Microstep 1 100.00% 2 70.71% 4 38.27% 8 19.51% 16 9.80% 32 4.91% 64 2.45% 128 1.23% 256 0.61% At 1/2 steps, I have approximately seven times the holding torque of 1/16 steps. Put on a new 12mm bit while my new 1/4" bits arrive from Toolstoday later in the week and then cut some hardwood. The machine now cuts the most accurate it ever has. Very pleased. Thanks for the help everyone. Some more questions: With the 12mm bit, the spindle is much quieter. How much of the noise if from vibration of the bit? The dip switches allow me to set the Decay Rate. Currently set to FAST. What does this do? Do I need to worry?
