Resetting to 0 after each line of code

[Exhibitology]

Greetings,

I finished installing an Acorn board into a DynaMyte 3300 slant bed lathe retrofitted with stepper motors.

To test my work, I was going to create 3 replacement registration popup pins for one of our CNC routers.

I created two seperate turning files with Intercon. One to turn down a .875" aluminum rod to 20mm. The other to put a shoulder on the end.

The first file ran flawlessly. The shoulder file not so much. I've attached photos of what Intercon graphed the file as and what the lathe cut.
I've also attached G-Code for both files and a Report.

It appears to me that rather than returning to Z0 after each pass, it is resetting Z0 to the end of the first pass. I can confirm that after aborting the job, Z0 was no longer at the end of the stock where I set it.

Thinking that it was a software corruption, I reloaded CNC12 v4.18 Lathe. I re-ran Intercon for the first file--turning .875" down to 20mm. This time this file behaved the same way the shoulder file did. After its first pass, it didn't return to Z0 but reset Z0 and proceeded to the next X depth.

Any insight or help you can provide is much appreciated.

Richard

[cnckeith]

axis motors and drives being used?

loose motor to screw coupler?

loosing steps on the rapid retrack move?

[martyscncgarage]

Greetings,

I finished installing an Acorn board into a DynaMyte 3300 slant bed lathe retrofitted with stepper motors.

To test my work, I was going to create 3 replacement registration popup pins for one of our CNC routers.

I created two seperate turning files with Intercon. One to turn down a .875" aluminum rod to 20mm. The other to put a shoulder on the end.

The first file ran flawlessly. The shoulder file not so much. I've attached photos of what Intercon graphed the file as and what the lathe cut.
I've also attached G-Code for both files and a Report.

It appears to me that rather than returning to Z0 after each pass, it is resetting Z0 to the end of the first pass. I can confirm that after aborting the job, Z0 was no longer at the end of the stock where I set it.

Thinking that it was a software corruption, I reloaded CNC12 v4.18 Lathe. I re-ran Intercon for the first file--turning .875" down to 20mm. This time this file behaved the same way the shoulder file did. After its first pass, it didn't return to Z0 but reset Z0 and proceeded to the next X depth.

Any insight or help you can provide is much appreciated.

Richard

Your pictures are very small, can't see much detail. Take them in higher resolution like 640x480 or so.
Post the intercon file .icn created as well.
Marty

[Exhibitology]

Thanks for the quick reply.

The motors are Keling KL34H2160-62-8A wired bipolar at 4.4 amps at 61 VDC.

The drives are Pacific Scientific 6410's at 1/16 microsteps.

The couplings are solid.

Just in case, I halved my maximum job rates.

It is definitely not loosing steps. It is resetting my Z zero work coordinate. You can watch it in real time.

It has to be something I'm doing wrong in Intercon. I have one file that works correctly and one goes haywire. One file,

popup.ItM

, correctly turns down a -1.7 inches of a .875" diameter aluminum rod to .787". The other

popup retry.ItM

, starts at Zero, resets Zero 1.8" in the positive direction, goes there, resets Zero 1.8" in the positive direction, goes there, etc.

All the while, it has also reset the machine position's Z axis Zero point. After loading and running

popup retry.ItM

, I have to rehome my machine because machine Zero has been changed. Running again puts me out of limits.

I went thru this three times. Home machine, Zero X and Z, load and start

popup.ItM

. No problem. Load and start

popup retry.ItM

. Problem.

I've attached screen shots of my Intercom turning screen. You'll probably see something that jumps right out at you. I wish I did.

Thanks for your help.

Best Regards

Richard

[Exhibitology]

By changing a G99 to a G98, the files now run identically.

Previously the file with a G99 was resetting work and machine coordinates
as the G code was executed. After a cut path, instead of a rapid return
for the next cut path, home was reset to the end of the first cut path
and a new cut path would begin from there.

The lathe has an working encoder connected to the inverter that
controls the spindle.

Why would a command for feed per revolution instead of one for
feed per minute would cause the resetting of work and machine
coordinates in the Z axis.

[martyscncgarage]

Can you please post the intercon files? They have a .lth extension.
We'll see if we can get Centroid's lathe tech to look at this. He will want to see the Intercon files along with the G code you posted.

A video of it cutting the part would be helpful too.

We'll try and get you squared away. This area is not my forte'
Marty

[DICKEYBIRD]

The lathe has an working encoder connected to the inverter that
controls the spindle

Shouldn't that be "The lathe has a working encoder connected 1:1 to the spindle that is controlled by the inverter."? I don't think it will work any other way.

[cnc_smith]

It has to be something I'm doing wrong in Intercon. I have one file that works correctly and one goes haywire. One file,

popup.ItM

, correctly turns down a -1.7 inches of a .875" diameter aluminum rod to .787". The other

popup retry.ItM

, starts at Zero, resets Zero 1.8" in the positive direction, goes there, resets Zero 1.8" in the positive direction, goes there, etc.

All the while, it has also reset the machine position's Z axis Zero point. After loading and running

popup retry.ItM

, I have to rehome my machine because machine Zero has been changed. Running again puts me out of limits.

I went thru this three times. Home machine, Zero X and Z, load and start

popup.ItM

. No problem. Load and start

popup retry.ItM

. Problem.

For the file popup retry.cnc running G99 - Feed per Rev you have F22 which would be 22 inches per rev. In inches per minute this would be over 6000 inches per minute. This would cause you to loose position. When using G99 the feed rate you should be like .010 - .020 per rev for roughing and .002 to .004 for finish pass to get a 32 finish or better. For the file pop-up.cnc you have the G98 in you have the feed rate at F3 which would be 3 inches per minute which .0015 feed per rev.

[Exhibitology]

Thank you. I had a hunch it had to do with the
inches per rev. setting only because if I switched
that setting the problem disappeared.

Your explanation makes complete sense.

Best Regards

Rich