Right, you pushed me in the right direction to check settings & I missed a really obvious one between the 2 aspires!!! On the good aspire it was set to climb mill as it was a newish install for the milling machine & never really used it yet. On the bad it was set to conventional. Creating both gcodes set to conventional, both were bad. I fixed the z & created the gcode on the bad aspire set to climb & it was back to normal with the teeth in proportion. I have most definitely never ever used aspire in climb so something still changed at some point. I'm now going to create the squares gcode on the bad aspire in climb & conventional & run both. See what happens
Mach3 movement on CNC is driving me mad!
- Thread starter Arckivio
- Start date
Help Support UKworkshop.co.uk:
Run my 50mm squares & conventional is undersize & climb is OK. I've added the 2 gcodes. Still weird as I always ran conventional. Also, in that area of aspire there is an allowance offset but I'm pretty sure that has always been at zero
sploo
Somewhat extinguished member
So that's really odd; because conventional vs climb should just reverse the path direction; it shouldn't make any difference to the dimensions in the gcode. It's possible that when a part is actually cut, a small diameter bit may experience differing levels of deflection (meaning the two cutting paths might produce slightly different sized parts).
What I'm seeing in the two square gcodes you just posted look correct - that is, they're both following a path whereby they're cutting 0.75mm outside of the 0,0-50,50 square (0.75mm being the radius of the cutter), and there are a few moves where the cutter arcs around each corner before making the next straight move.
I.e. from a visual inspection only (I've not run them on a simulator) I'd guess that both of those files should produce the same size square. If in practice they're not then it's bit deflection. It looks as though you're cutting in depth increments of around 1.814mm, and with a feed rate of 6000.0mm/minute (assuming that is the format/style your machine uses). That feels exceptionally high to me; especially for a 1.5mm diameter bit. I don't have any of my CNC stuff on the PC I'm using at the moment, but from memory, I'd run a 6mm bit at around half that feedrate, and thinner bits much slower.
If I'm right with the feedrate setting, maybe try lowering it to 1500mm/min, and maybe a shallower depth of cut (rough rule of thumb is no deeper than the bit diameter) and see if the conventional and climb jobs now produce the same size part. If so, the problem is bit deflection.
My guess is that 1.5mm cutter would be bending like a wet noodle at 1.8mm DOC and 6000mm/min feed.
What I'm seeing in the two square gcodes you just posted look correct - that is, they're both following a path whereby they're cutting 0.75mm outside of the 0,0-50,50 square (0.75mm being the radius of the cutter), and there are a few moves where the cutter arcs around each corner before making the next straight move.
I.e. from a visual inspection only (I've not run them on a simulator) I'd guess that both of those files should produce the same size square. If in practice they're not then it's bit deflection. It looks as though you're cutting in depth increments of around 1.814mm, and with a feed rate of 6000.0mm/minute (assuming that is the format/style your machine uses). That feels exceptionally high to me; especially for a 1.5mm diameter bit. I don't have any of my CNC stuff on the PC I'm using at the moment, but from memory, I'd run a 6mm bit at around half that feedrate, and thinner bits much slower.
If I'm right with the feedrate setting, maybe try lowering it to 1500mm/min, and maybe a shallower depth of cut (rough rule of thumb is no deeper than the bit diameter) and see if the conventional and climb jobs now produce the same size part. If so, the problem is bit deflection.
My guess is that 1.5mm cutter would be bending like a wet noodle at 1.8mm DOC and 6000mm/min feed.
The feedrate you're seeing is just what I set in aspire, I reduce the speed in mach3 to 40% but I did try running at 10% when I was fiddling with all this & was still rubbish. What's really odd is that at one point, I ran 2 larger clock gears & I actually used them & then aspire decided to throw a wobbly. I looked up the offset allowance & this is what it says:
The Allowance Offset only applies to the Outside / Right and Inside / Left options. It provides a quick and easy way to calculate different size toolpaths using only one defining vector.
The Allowance Offset only applies to the Outside / Right and Inside / Left options. It provides a quick and easy way to calculate different size toolpaths using only one defining vector.
- For the Outside / Right option, a positive offset value will leave more material on the outside of a closed vector or to the right side of an open vector. Likewise, a negative offset value will remove more material from a closed vector or leave less material to the right side of an open vector.
- For the Inside / Left option, a positive offset value will leave more material on the inside of a closed vector or to the left side of an open vector. Likewise, a negative offset value will remove more material from the inside of a closed vector or leave less material from the left side of an open vector.
J-G
Established Member
I'll agree there! - I also make gears, from Tufnol, Maple, Walnut etc., and use 1.5mm end mills and my roughing DOC is never greater than 1mm - more often 0.5 - 0.8 and feed rate 200 - 300mm / minute. The other factor which may also impact upon the situation is spindle speed but I can't see any reference to such in past posts. I tend to run my 1.5Ø mills at 18-23k and suspect that with that high feed rate (even modified to 40%) if the spindle speed is in the low 1000's there is likely to be a great deal of side pressure which could lead to tool deflection.
For final cuts - taking off the last 0.2 or 0.3mm - I would use a DOC of up to 5mm but reduce the feed to 100 - 150mm/min - and certainly use the 23k spindle speed.
J-G
Established Member
Certainly! - an increase of nearly 70% in DOC will definitely have an impact - the amount - 0.8mm might not seem very great but at the distances we are talking about it is massive. Regrettably I don't have the knowledge to give you the mathematical calculations but it is (to me) quite obvious that the stresses placed on the cutter would be different between conventional & climb milling as well.
I wouldn't have thought that your spindle speed of 18.5k out of place for a 1.5mm cutter though.
You have mentioned that the 1.5mm dimension is 'accurate' and that is one factor that you've addressed but I suspect that it may well be that the tool-holder is an area which would benefit from a close inspection. I made my own holder for 1/8" shank cutters - I assume that is what you are using but could well be wrong in that - and if your 'collet' or whatever you use has an eccentricity of even 0.1mm or the 1/8" hole is actually (say) 3.3mm (rather than 3.175) then the fact that the cutter is good for size is of secondary importance.
sploo
Somewhat extinguished member
So, I have a tool that suggests suitable feeds and speeds for cutters vs materials. It suggests that a 2 flute 1.5mm carbide endmill, with 10mm of stickout from the collet, running at 18.5k rpm and 2400mm/min (40% of your 6000mm/min), running a 1.8mm depth of cut in plywood will be at (wait for it): ~300% of accepted deflection (100% being the max allowed). I.e. bending like wet noodle as I noted earlier. I'm surprised it hasn't snapped TBH.
The tool says a 1mm depth of cut and 1000mm/min feed is about 75%; so fairly safe. Certainly that's closer to my gut feel settings (though I'd probably have erred lower in CAM).
As for climb vs conventional; in climb milling the feed direction + cutter rotation will see the flutes "stake" over the material cutting edge, whereas conventional will be driving the cutting flutes into the material being cut (the flutes "grab" the material edge). With large bit deflection that will likely cause overcutting for conventional and undercutting for climb (which I think is what you're seeing - at least for the conventional pass).
The tool says a 1mm depth of cut and 1000mm/min feed is about 75%; so fairly safe. Certainly that's closer to my gut feel settings (though I'd probably have erred lower in CAM).
As for climb vs conventional; in climb milling the feed direction + cutter rotation will see the flutes "stake" over the material cutting edge, whereas conventional will be driving the cutting flutes into the material being cut (the flutes "grab" the material edge). With large bit deflection that will likely cause overcutting for conventional and undercutting for climb (which I think is what you're seeing - at least for the conventional pass).
sploo
Somewhat extinguished member
2mm DOC with a 1.5mm dia bit is asking for trouble. Even at 10% feed rate (600mm/min) the tool I have suggests you're into risky territory. If you have more than 10mm of the cutter extending from the collet then you'll definitely be over an acceptable deflection limit (i.e. even 11mm stickout would be too much).
Take that DOC down to 1mm and you're back within safe deflection limits at 600mm/min feed (1000mm/min feed would be too much with 11mm of stickout, but safe with 10mm).
Now I can't wait to get down my workshop to try this out! Cutters never snapped so I went with it!!! My initial thoughts regarded the new motors & new breakout board as they were my major changes, but along the way I upped the DOC too!
I will now be using Artcam LOL!!! I dropped down to 2mm second, DOC to 0.8mm, did it come out better? Yes, but it's still not behaving as it did previously. I definitely didn't run in climb mode before without noticing as I remember switching between the 2 for certain things. Also, parts run with Artcam were run at the higher speed & in conventional & came out as they did before with Aspire. Even more confused than before but I've accepted that aspire needs to run in climb mode or just use Artcam!!! Thanks for all your suggestions & help
