Problem- Turned diameter is wrong.

[jimbies]

Hi jhowelb,

Below are the readings :-

Reading of DRO 11.285mm
OD of cut piece 22.52mm

[jhowelb]

The if you set jog on incremental and enter 1.000 as the increment to move then jog the X slide it should move .500.

Otherwise your motor tuning is wrong.

On the Z a jog of 1.000 will produce a movement of 1.000 but on X a jog of 1.000 will produce .500 movement.

[acondit]

Originally Posted by jhowelb The if you set jog on incremental and enter 1.000 as the increment to move then jog the X slide it should move .500. Otherwise your motor tuning is wrong. On the Z a jog of 1.000 will produce a movement of 1.000 but on X a jog of 1.000 will produce .500 movement.

Often times a tool will be ground with a very small radius on the tip. This will result in having to cut in past zero to remove the little tit left in a facing cut.

So the difference between your measured diameter and your cut diameter is only 0.05mm or slightly less than 0.002". That would say that your center (X0) is off by 0.025mm or slightly less than 0.001".

If you have any backlash at all in your system, you need to back out your X axis say 0.050" or about 1.2mm more than your desired cut then move in towards your cut and always approach your cut from the same direction.

I used to have real problems when I needed to make both inside and outside cuts. Backlash would always screw me up.

I would make a cut, measure the diameter, divide the result by 2 (radius), jog z to clear the material, jog x in by the (calculated) radius amount and then set my x0. It is probably a good idea to actually write down the dro radius and the calculated radius and subtract the calculated radius from the dro radius (that way you know whether you have to jog to a positive x value or a negative x value).

Alan

[jhowelb]

But look at post #13.

Below are the readings :- Reading of DRO 11.285mm OD of cut piece 22.52mm

The dro is indicating radius and he is measuring diameter. then a move to X0 puts his tool at the back side of the part. The only way possible for that to be is that he set his motor tuning to move the distance called for as if radial and the software is set for diametrical.

Mach3 compensates for diametric mode by moving the tool half the distance because by cutting a depth of .005 will result in a reduction of the diameter by.010.

I think he just needs to wrap his head around the difference between diametric and radial modes as applied in Mach3.

[acondit]

Originally Posted by jhowelb But look at post #13. The dro is indicating radius and he is measuring diameter. then a move to X0 puts his tool at the back side of the part. The only way possible for that to be is that he set his motor tuning to move the distance called for as if radial and the software is set for diametrical. Mach3 compensates for diametric mode by moving the tool half the distance because by cutting a depth of .005 will result in a reduction of the diameter by.010. I think he just needs to wrap his head around the difference between diametric and radial modes as applied in Mach3.

John,

You are partially correct, but I doubt that a difference of only 0.05mm (about 0.002") is a result of confusion over radius and diameter. In his very first post, (if I read it correctly) he started with a measured diameter of 23.43mm and tried to cut 23mm but ended up with 22.57mm (precisely 0.43mm too small). He in fact moved the X axis in 0.43mm resulting in removing 0.86mm diameter (23.43-0.86=22.57). This appears to be a clear case of confusion of radius vs diameter as you correctly pointed out.

My point was that 2*11.285mm radius=22.57mm dia. He measured 22.52mm. That is a difference of 0.05mm diameter. Since the measured diameter is smaller than the commanded diameter, his center point is probably not correct (off -0.05mm dia. means -0.025mm radius or slightly less than -0.001"). The rest of the post was designed to help him get his X0 set properly.

Alan

[jimbies]

The if you set jog on incremental and enter 1.000 as the increment to move then jog the X slide it should move .500. Otherwise your motor tuning is wrong.

Otherwise your motor tuning is wrong.
[/QUOTE]

Initially the jog give a 1mm on the X axis. Then I half the motor tuning figure and the X axis moved .500mm.

Is this how the X axis should be set ?

All this while, I was thinking that when the Gcode is run, Mach3 would automatically do the compensation for the X axis move if the selection in X Mode is Diameter ???

[jhowelb]

Originally Posted by jimbies Initially the jog give a 1mm on the X axis. Then I half the motor tuning figure and the X axis moved .500mm. Is this how the X axis should be set ?

YES! IMHO this mystery has just been solved.

Mach applies the diameter mode universally. The wizards will compensate and all will be sunshine. Just remember that you are working in diameter and your cutting tool only touches on one side of the work piece to produce a reduction on the diameter, both sides.

I just now produced the same error on my lathe by doubling the increments per unit on the X motor tuning page.

Now, if you use some third party software it can muck things up again by invoking certain gcode commands.

[jimbies]

One final question, just to be sure I get it right.

Pitch of leadscrew = 1 mm/rev
Stepper motor = 1.8 deg (200 step/rev)
Stepper drive = 16 microstep

motor tuning = 1 x 200 x 16 = 3200

So the motor tuning to use will be 3200 / 2 = 1600 (which is what I set now).

Is this correct ?

[jhowelb]

Now lets take a couple of steps back.

Make sure on the Configuration menu, ports and pins>turn options>X mode is checked and that native units are selected properly.

Then jog to a position close to where the cutting will be done then click Zero World X and Zero World Z. (This prevents some crazy initial moves)

Then take a light facing cut an click Z Zero.

The take enough of a turning cut to get a clean surface all round the part and shut the spindle off without moving the tool.

Measure the diameter of the part, enter that figure into the X DRO and press enter.

Jog clear of your part and G0X0 and see if the tool goes to center of material.

Try it and see if it works, you have nothing to lose.

Be aware that there are English and Metric gcodes to confuse things.

I wish I could put hands on your machine with you watching. We could clear a lot of confusion quickly but there are many mile between California and Singapore.

Good luck and keep us posted.

[jhowelb]

Originally Posted by jimbies One final question, just to be sure I get it right. Pitch of leadscrew = 1 mm/rev Stepper motor = 1.8 deg (200 step/rev) Stepper drive = 16 microstep motor tuning = 1 x 200 x 16 = 3200 So the motor tuning to use will be 3200 / 2 = 1600 (which is what I set now). Is this correct ?

I have to confess relative ignorance on the subject of metric threads but I have to question the 1mm per rev. pitch. Are you double sure of that?

In Imperial terms that would be a lead screw of 25.4 TPI. All the lead screws with which I am familiar are on the order of 8 to 12 TPI. Any finer than that and the steppers can't keep up with the speed necessary to do the work we ask of it.

If you have the wrong pitch for that screw the explanation for your problem changes dramatically!

What about the pitch and performance of the Z axis? Is it giving you correct movements and is it the same screw?

[jimbies]

Thank you for your patient all along with me, really appreciate your help.

Was busy weekend doing some test cut with the Wizard... OD turning, OD Taper, OD Arc, and those turn out very well, all within dimension. Thanks to you and also to those who have posted.

have to question the 1mm per rev. pitch. Are you double sure of that?

"One turn of the handwheel causes the leadscrew to advance the tool or part .050" (inch models) and 1 mm (metric models)." ... from Sherline catalog.

You are right, the Z axis is very slow because of the fine pitch leadscrew. The maximum speed of my Z axis is 330 mm/min. (13 in/min), so can only cut fine threads, which is only good maybe up till 10 -32 screw.

Was trying to test cut a 3/4 - 16 thread yesterday day, the max speed I can run the spindle is 150 rpm with the Z axis running flat out. Some suggestion on how to increase the Z axis speed would be nice.

Oh, I love Califonia, last time I was there, was 15 years ago, best place to be on planet earth.

[jhowelb]

Almost universal is the move to ball screws. You can read my journey here.

http://cnczone.com/forums/showthread.php?t=26530

The higher quality screw the better satisfied you will be. You gain accuracy and a big drop in friction. Recommend ball screw on both axes.


You are very welcome! Glad I could help.