Hi All,

Having a small issue with Mach 3 Turn.

Turning a part with of varying diameters of 7mm, 5mm and 3mm. Created a DXF and used LazyTurn to create the G Code.
Load it in Mach3 Turn. Set the tool to touch the Z (start of part) and set the X to the diameter of stock (8mm Dia so using 4mm as X value). I've checked and I am in radius mode!

Program cuts fine. Part length is correct but the Diameters are out bay a long way. 7.9mm, 6.56 & 4.6mm

Any ideas on what could be wrong?

I do have backlash enabled on Mach3 with some values added as measured in my initial setup.

Any information to solve this would be appreciated. Cheers.

Dave

Hi Dave, there could be a few issues here.

First, how did you set the tool to the X value (4mm)?  Was it by touching the tool to the stock, and if so how did you judge "touch"?  Was the stock running concentric?  Was the tool accurately on centre height?

How much was the stock projecting from the chuck, could it have been bending under the cutting force?

Did the G code generated by Lazyturn have the correct X values in it, i.e. finishing at 7, 5, and 3mm?  Could you post the code?

I always use the lathe in diameter mode and find it much less confusing - it's more or less standard on metric manual lathes to work in diameter and the X slide handwheel is calibrated in mm off diameter.  I have a ballscrew on X axis though I haven't converted the Z yet, but I've never been convinced that backlash compensation works very well in M3 Turn so I don't use it, just avoid moves where it will be an issue.  Depending on how you have it set up and how you are moving the tool before each cut it could contribute to your problem.

The stock wasn't far from the chuck, just enough for the part plus a little extra. I also used a tailstock.

I slowly jogged the tool to the stock and took a very light skimming cut and measured with Verniers. Original stock was just over 8mm Dia as skimmed stock was exactly 8mm. Moved the tool to the corner of the stock, zeroed x and z. Pressed the touch button for the tool. Changed the x to 4mm by overtyping in the X DRO.

I've attached the code.

Thanks for the help.

The code looks wrong for the sizes you quoted.

It could be the drawing that is wrong or the tool path.


N435  S3000 F50.00 M3
N445  G0 X4.1000
N455  G0 Z0.2000
N465  G1 Z0.2000 X1.5000
N475    Z-0.1000 X1.7000
N485    Z-4.6000 X1.7001
N495    Z-5.0999 X1.7046
N505    Z-5.5989 X1.7362
N515    Z-6.0966 X1.7832
N525    Z-6.5927 X1.8456
N535    Z-7.0866 X1.9233
N545    Z-7.5779 X2.0162
N555    Z-8.0661 X2.1242
N565    Z-8.5507 X2.2473
N575    Z-9.0312 X2.3853
N585    Z-9.5073 X2.5380
N595    Z-9.9794 X2.7000
N605    Z-14.9794 X2.7001
N615    Z-15.4772 X2.7463
N625    Z-15.9738 X2.8047
N635    Z-16.4689 X2.8744
N645    Z-16.9623 X2.9551
N655    Z-17.4538 X3.0469
N665    Z-17.9431 X3.1497
N675    Z-18.4300 X3.2633
N685    Z-18.9142 X3.3880
N695    Z-19.3955 X3.5233
N705    Z-19.8737 X3.6695
N715    Z-20.3690 X3.7000
N725    Z-24.8690 X3.7001
N735    Z-25.0000 X3.6332
N745    Z-25.0000 X3.6332 (X7.2664 Dia)
G0 X4.1000

I agree with Graham - as well as his point between lines 715 and 725 the g code says cut 7.4mm whereas you said you were aiming at 7.  Also in the finishing pass the X value increases as Z decreases which wouldn't work very well if the backlash isn't exactly eliminated.

What machine are you using?  Does it have ballscrews?  Have you tried some simple parallel cuts using the Mach3 wizards with BLC turned off?

And an obvious point, have you checked the calibration (i.e. steps / unit) using for example a dial gauge?

Something else I noticed is that having made a cut in the -z direction at a given radius the tool returns at the same X setting using a G0.  Best practice would be to withdraw the tool slightly before moving back as the tool will cut on the return move otherwise.