Is this an example of what backlash can do?

Hi....

So I decided to try and mill a sphere as a test piece to check the functioning of my mill and the software I'm using. I figured a sphere would be tough - and I turned out to be correct.

I'm using Vectric Cut3D to produce the toolpath and Mach3 to control the mill.

I used a piece of pine 70mmx70mmx43mm and aimed for a sphere 40mm in diameter.

However, it became very obvious on the 2nd pass that the circles being left after each pass were not concentric. I could see clearly that when Mach3 said the X-axis was at 70mm it was in fact probably 75mm!! It seems as though Mach3 no longer knew where the exact position of the mill was. I shut the mill off when it became apparent that the Z-axis had suffered the same fate.

Here's the piece after about 12 roughing passes.

It's a mess:

http://farm6.static.flickr.com/5020/...12534c8923.jpg

Does anyone have any ideas why this may have occurred and possible solutions please?

Is this backlash at work?

Regards

Simon

HOLY S**T!!!!:rofl:
dont you just hate it when that happens!
looks like the mountain off close encouters :)

looks like a shitload of lost stepps to me
id zero your tool and DRO's in mach on a point rapid XYandZ back and forth for a spell and get mach to go back to zero

im gussing it will stop miles away from your refrence point, if it dose you need to back off your rapid speed in motor tuning

going off what you are saying, if its reading +70 on the X axis and is more like +75 then your losing stepps when the X axis is moving in the minus direction, it maybe during a rapid or during a cut (cant tell without seeing the tool path)
what ever it is you need to lower friction on your X axis or stop driving your X stepper so hard

Ok... thanks for that..... I'll try that right now....!!

And yes... it's the worst example of a sphere I've ever seen.... mind you it's first attempt at anything on the mill.....

Looks more like lost steps to me. Backlash would have the circles concentric but not circular.

You could try it at a lower feed rate to see if it's lack of power in the steppers.

A more scientific test is to put a dial gauge against the axis, creep up to a sensible setting and then rapid traverse away from it then come back to the same position at a low feed rate. The dial gauge should have the same reading.

If it's happening on all axes with no pattern it might be noise or if it's happening when doing moves on all axes it might be the power supply struggling.

Have you tuned the top speed and acceleration settings of Mach3? What are you using for steppers / drivers / power supply and what feed rates were you using?

Quote:

---

Originally Posted by Minnican

And yes... it's the worst example of a sphere I've ever seen.... mind you it's first attempt at anything on the mill.....

---

all part and parcel of building a cnc in my opinion, i think we have all had our share of disasters but yours has really tickled me, i actualy laughed out loud when i saw that picture.... it reminds me that im not alone on the planet

it looks like it will be a pretty simple fix with a bit of messing about in motor tuning

let us know if you manage to carve anymore square spheres :)

Ok..... suggestions thick and fast...... I like it.

Right, after zeroing and whizzing around on all axis.... the DRO's no longer correspond with the home. X=-1.3675mm; Y=-0.5475 and Z=+1.9063, all approximate figures.

I looked at the setup of the motors and see: X-axis "steps per"= 800; "velocity"= 1500; "acceleration"=200; "step pulse"= 5; "dir pulse"=3

Y-axis "steps per"= 800; "velocity"= 1500; "acceleration"=200; "step pulse"= 5; "dir pulse"=3

Z-axis "steps per"= 800; "velocity"= 700.2; "acceleration"=100; "step pulse"= 5; "dir pulse"=3
Velocity and acceleration in the above is mm.

The stepper motors are 57BYGH488 1.8 degrees and 2.5A. Can't really answer regarding drivers and power supply as I'm not sure where to find this info.

Yep..... the photo's certainly worthy of a giggle...... I did..... after the cursing!!!

Oh.... and feed rate box on mach3 reads:

FRO=6.00
F=6.00
100%
units/min=0.00
units/rev=0.00

I have no idea what any of that means...!!!

I'm no expert but have you set up the machine correctly? It seems to me that the machine is moving further than it thinks. Double check that you have set the number of steps per linear measurement correctly. These may not all be identical by the way. What works for the X-Axis might not be right for the others etc.

Martin.

1500 sounds a bit quick for a mill using 2.5A steppers
id leave the other settings for now and work on the velocity
i would have though below 800 on all and try again
if it works well up them bit by bit and visa versa

ok..... i'll adjust the X and Y to 800 and rerun the sphere. I presume I need to lower the Z from 700 as this is losing steps too.....?

Quote:

---

I presume I need to lower the Z from 700

---

yea, thats the one, dont run the sphere unless your sure youve cracked the problem (or you have a boat load of wood and time) might be wiser to cut a hole in something and measure how round it is

The fact that all three axes are loosing steps is suspicious but the feed rates do seem high so that might explain it - are you running ball screws. Where did the configuration parameters come from?

I use EMC2 and don't know much about Mach 3 but a quick skim of the manual found a couple of references to step pulse width and inversion...

"Pulse width is another consideration. Most drives will work well with a 1 microsecond minimum pulse
width. If you have problems with the test moves (e.g. motor seems too noisy), first check that your step
pulses are not inverted (by Low active being set incorrectly for Step on the Ports and Pins>Motor
Outputs tab), then you might try increasing the pulse width to, say, 5 microseconds. The Step and
Direction interface is very simple but, because it can still “sort of work” when configured badly, it can
be difficult to fault-find without being very systematic and/or looking at the pulses with an oscillo-
scope."

So if the motors sound rough at moderate feed rates it might be worth checking that the low active or high active setting is set to match your drivers. What machine is it you've got? Are there any technical documents with it?

As Mark says, it's all part of the learning experience - I've got a couple of parts on the mill that need remaking due to it loosing steps while I was making the parts needed to stop it loosing steps :-)

ok..... so I've just found a setting for axis calibration and adjusted as follows.....:

X set to move 80mm and moved only 77mm
y set to move 80mm and moved 80.5mm
z set to move -50mm and moved -48.5mm

lets see if this make a significant difference.

Also noticed this line in the GCode:

N80X0.000Y0.000F2400.0

Is the F for feed rate and is it too fast...?

Thanks in advance!!!

Hmm, that 'sphere' looks familiar! :whistling:

I think you should try running back and fourth with a greatly reduced feed rate. Say 50%. If it does go back to zero accurately you then know it's missed steps, not something more interesting happening.

You may find that it runs fine when jogging, but not in reality due to there being multiple motors running when cutting. So try jogging both X and Y by pressing multiple arrow keys at the same time.

If you really want to do it properly then get a piece of string, a pulley and a suitable weight (say 10N ish, much more if you're thinking of cutting aluminum) to simulate the cutting force. Set it up so that moving the X axis lifts the mass vertically and ideally have it so the string from the Z axis to the pulley is horizontal. Shouldn't be too hard ... Repeat the process for Y, and Z if you're keen!

Hope that helps...

Oh and to answer the original question - no that's not what backlash will do. Poor backlash would cause 4 lines to be visible on the surface of the sphere, each at the point where the X or Y axis changes direction.

Quote:

---

Originally Posted by Minnican

N80X0.000Y0.000F2400.0

Is the F for feed rate and is it too fast...?

Thanks in advance!!!

---

Yes that's right. 2400mm/min is much too fast for your machine seeing as the x/y will only do 1500. Mach3 will automatically limit the feedrate to 1500, but still if your machine only just manages to rapid at that speed it's no wonder it looses steps with the additional force due to cutting.

I'd set the feedrate to maybe 800mm/min to start with and see how it goes. Be careful though - too low a feedrate and too high a spindle speed will burn the cutter. So check it's not getting too hot...

This forum is great........ thanks for all the advice...... I'll let you know how my next sphere gets on in the morning......!!

Ok.... so had a day off yesterday but back today.....

I have changed and rechanged every setting I can find without any change in performance but finally I changed the "step pulse" to 10 and the "dir pulse" to 15 for each of the axises. The whole mill now sounds sweet without the "grinding" noises I had experienced from day 1. It actually sounds like other mills I have seen on Youtube etc.

I've run the top half of the sphere again and this is the result......

http://farm6.static.flickr.com/5055/...6636d43406.jpg

Note my cutter seems to get very close to the sphere on the roughing toolpath, this was something I didn't expect and a potential problem, I presume this is solved using longer cutters?

Thanks for all the advice...... I've learnt much following all your suggestions....... and above all found a cure for this problem.

That looks a whole lot better

Quote:

---

I've run the top half of the sphere again and this is the result......

---

Splendid!!..... i bet that felt a whole lot better:smile:

Quote:

---

Note my cutter seems to get very close to the sphere on the roughing toolpath, this was something I didn't expect and a potential problem, I presume this is solved using longer cutters?

---

not sure if i get what you are saying...
i cant see any rough cut marks through the last cut... if your having problems though you will have to stipulate at the CAM stage of your G-code production how much clearence you want between your rough cut and finish cut

Quote:

---

Originally Posted by Minnican

Note my cutter seems to get very close to the sphere on the roughing toolpath, this was something I didn't expect and a potential problem, I presume this is solved using longer cutters?

---

I think you're referring to the chuck colliding with the sphere? If so then yes a longer cutter is the way to go. Be careful though - cutter rigidity is inversely proportional to the cube of the length of the cutter.