Newbie looking at 6040 (China CNC) for polypropylene 15mm sheet

[Zeeflyboy]

Typical stepper is 200 steps per revolution. You have 5mm screws, so you move 0.025 per step (5/200).

Microstepping doesn’t really count, so the fact you have eg 320 per unit (can’t remember exactly what the stock setup is) isn’t really what you’re looking at, though you could argue with little to no load it won’t be far off.

That said, I can move mine in 0.01mm steps on the jogging button but I have 1.2 degree steppers (so 0.017mm per full step) with built in encoders and microstepping gives 800 per unit.

Just edit your jog values so that one of them is 0.01mm and it’ll do it’s best to match. If it is 320/unit then you have a base value of 0.003125 so any movement will be a multiple of that - that means the closest movement to 0.01mm you could theoretically get is 0.009375 which is why the value in the readout looks a bit odd - it’s physically impossible for it to move to any value that isn’t a multiple of 0.003125. Again though microstepping is not really reliable regarding accuracy so your “real” resolution is 0.025 as limited by the motor steps per degree and the pitch of the ball screw.

Btw I would try to use the least amount of travel on the dial indicator - those type can have a fair bit of spring push and you may be deflecting the probe rod slightly. No guarantee that the deflection is equal all the way around.

Do you actually need to jog into the dial for this? I just spin the guage zero so that it sits in the middle of the values for either side and then adjust probe until it reaches close to zero, then move to the next set of screws and repeat, then go back to the first as it may have moved slightly. That will normally get runout to less than 0.01mm for me. Definitely a bit of a knack to it but it only takes me a few minutes now.

Oh and finally have you tried calibrating the machine? Mine wasn’t exactly wonderfully accurate out of the box. I think mach3 even has a screw calibration wizard that saves you doing the maths.

[JOGARA]

I have not changed anything other than adding ProbeIt to the wizard.
Don't like messing with stuff.

This is default.


What would be the highest resolution I can get from this without it being too weak?
That and roundest number possible :p


I moved back on the indicator and got around 0.025mm so tiny bit of movement yes.



Ideally I want to be able to probe my soft jaws and just batch process a load of cases.
Changing tools all the time takes time.

[JOGARA]

The only way around this is to mill the outside and front of my case first, then flip and mill inside with the degree of error being around 0.05-0.075mm.
This would allow me to vacuum plate the first operation on the front of the case, removing the need for super glue.

I think I could live with that...

Ideally I could get it all bang on but that is not looking like it is going to happen on this machine any time soon... :/

[Zeeflyboy]

I wouldn't get overly obsessed with the DRO giving a round number read out - better that it is actually calibrated correctly.

After all, other than for reasons of OCD consider that your 17.9188 from the DRO above is only 0.0012mm away from the commanded 17.92 - 0.0012mm is roughly half the width of a typical bacterium (which are commonly 0.01mm long too for context!) Basically it's a level of precision that your machine couldn't possibly hope to achieve anywhere near so it's irrelevant for all but how neat the DRO looks.

When you correctly calibrate the ballscrews, likelihood is that you will end up with a horrendous number like 321.24 as your calibrated steps per mm which of course means you don't have a snowball's chance in hell of ending up at a round number on the DRO.

I'm not sure how you arrive at your conclusion that you will be working to an error of 0.05 to 0.075mm.... but 0.05mm is nothing to be sniffed at... it's a very good level of accuracy realistically speaking - less than the thickness of a typical human hair.

Increasing the microstepping won't really help... if anything it just makes it harder for your motion controller to keep up at high speeds. Microstepping really only serves to make things smoother, gains in resolution are mostly illusionary.

[Snapper]

I have the same machine. A couple of things. I have recently done a batch run like what you're wanting to do. I did it by marking my vice with a bit of white electrical tape and eyeballing the edge of the stock up to it, drilled all the holes with the same drill bit (smallest hole size, the larger holes I opened it manually with a cordless whilst the next part was on the machine) on the vice then moved them over to a fixture plate for profiling, located by two dowels after reaming two of the holes by hand, then ran the profile paths, chamfer, flip, chamfer.

If you are touching the home switches at any point, don't. They are lousy and will introduce anywhere between 0.04 to 0.32 error on each axis. The machine itself isn't so awfully bad at repeatability, there is a bit of backlash in mine but it ran the ops on all 6 of the parts I made without any major visual error. I chucked up my dti between each tool change and rezeroed off the reamed hole on my bed I use as a reference just to be sure but it was probably a waste of time.

To step jog, press tab on your keyboard in mach3 and you can change between continuous jog mode and step jog, and also change the step value. Spinning a dti in a reamed hole to find zero I use 0.01mm step and I'm normally back out the hole and putting a tool in within a minute.

Tool changing is the enemy. My z setter is nuts for some reason and will never give close to the same result twice so I've been z setting with a feeler gauge for awhile, takes a little longer but it's absolutely on point. Cleaning the spindle taper, spindle threads and collet nut between each tool change is also a real bastard (I've just ordered a second collet nut so I have one clean with the tool mounted ready to screw in). And also spend far too much time making sure I have the mist nozzles pointing in the right place.

[Zeeflyboy]

Tool changing is the enemy. My z setter is nuts for some reason and will never give close to the same result twice so I've been z setting with a feeler gauge for awhile, takes a little longer but it's absolutely on point. Cleaning the spindle taper, spindle threads and collet nut between each tool change is also a real bastard

I do something very similar these days - I have a reel of 0.01mm shim steel and I jog the tool up to just short of the z-zero surface, then jog in 0.01mm increments while sliding the shim material back and forth. Once it grabs you know you are 0.01mm above the surface and it works rather well for me.

Interesting point about cleaning between changes... Until relatively recently I never paid much heed to this and the amount of gunk that I managed to clean out of my spindle bore was eye opening. more than halved my runout by cleaning it out.... now every tool change I use compressed air to clean out the collets and bore, and usually a piece of oiled kitchen towel to wipe out the bore before then re-inserting the new collet if changing collet size.

[Snapper]

I do something very similar these days - I have a reel of 0.01mm shim steel and I jog the tool up to just short of the z-zero surface, then jog in 0.01mm increments while sliding the shim material back and forth. Once it grabs you know you are 0.01mm above the surface and it works rather well for me.

Interesting point about cleaning between changes... Until relatively recently I never paid much heed to this and the amount of gunk that I managed to clean out of my spindle bore was eye opening. more than halved my runout by cleaning it out.... now every tool change I use compressed air to clean out the collets and bore, and usually a piece of oiled kitchen towel to wipe out the bore before then re-inserting the new collet if changing collet size.

I use a thicker 0.55mm gauge purely because it's more solid so easier to keep straight and flat. I eyeball down then step jog back up until it fits under.

Yeah cleaning everything is absolutely paramount to getting a nice cut. Specially with alu, chips get in the slots in the collet and cause absolute carnage. I use isopropyl alocohol on paper towel. It's quite amazing just how much black comes off everything, even after a relatively short op. I have a piece which got scrapped anyway because I didn't realign the flip properly, but each side done using the same tool in the same collet in the same nut and the difference in surface finish between the two sides is incredible. The difference being when I first inserted the tool for the first side I forgot to clean everything up first. I will dig it out the scrap box tomorrow and upload a pic as it's a great example.