Hello All,

I have been in a Hiatus status for over 2 years, but am back finally. I retired and then moved to Washington State to be near the grand kids. We have a great 2 ½ acre plus site in the trees which even has a pond with an island. It is off the beaten path, but close enough to amenities and is absolutely gorgeous. This has been keeping me busy to say the least for a while.
Anyway, finally found time to unbox the CNC outfit and get it up and running. Everything seemed to function and of course I am having to relearn almost everything. Unfortunately I have a couple of problems that I did not have before. Hopefully you Guru’s can understand my wording and help me come up with a solution.
First issue is the machine will be chugging along and then just stop. No repeatability and completely random. I have tried various things to stop this and nothing has helped. Second issue which is the real problem is that when I try to continue it takes off in X and Y all on its own. It then plunges to the depth that Z was at before it stopped and of course “Bang” there goes an expensive carbide cutter plus wasted expensive material. This obviously can’t continue.
I have now started air cutting, trying different things and have found some interesting issues. It looks like I can force mach 3 to throw an error which appears to match what has been happening. The code will be running and I will hit the screen stop button. Everything of course stops, but when I restart the program X and Y will swing out and circle around clockwise. Eventually it finds the correct and original cutting line and then continues on as if nothing was wrong. Now the strange one is that if I hit the screen pause button and then restart things everything is OK and works like it should. Even stranger is that the buttons on my pendant act just the opposite of the screen buttons. Stop allows me to stop and start without issues, but pause causes the X and Y error.
I am going to try add a copy of the machine code and a screen shot showing the original circle cutting path and the obvious crazy error path.

Running under Windows 7
Version of Mach 3: Licensed and whatever was current January 2012
(I know, I should just go ahead and load the latest)

Thanks in advance

Mark

I would venture to bet the first issue is noise/electrical interference. This can be resolved a few ways. First I would check to see if you are running any debounce. If not I would use a value of say 500 to start (500 x 40us (microseconds). If it works with 500, try 250. Keep working it down though numbers in this range are fine. Other options included ferrite beads on your limit or Estop, capacitors, shielded wiring, star grounds and wire management. Mostly just a methodical approach to correct grounding procedures.

I would reload Mach preferably with a newer version but even the older versions are fine if you have been successful with it. Some form of file corruption pops up every now and then.

I too have had weird and seemingly unexplained actions after pressing different switches whether they are on screen or thru my Shuttle Pro. I run so many different products I expect it. The 1 thing I now try to implement is a contactor also tied into my Estop switch (separate set of contacts on the Estop switch) that kills ALL power to the drivers, BOB's, relays or whatever, everything (except PC power which is not plugged into the machine). You wouldnt guess what motivated me to do such a thing.  

Thank you for your input and I apologize for the delay in getting back.

Well, I did some checking and the CNC itself seems fine. All cabling is good, shields are grounded and nothing is bound up. I then ran the code within Mach 3 by itself with the CNC off in what I guess would be called SIM mode. Problem was still there. OK, time for upgrading the program, must have a corrupt file somewhere. Went through the gyrations and installation went smooth. I then ran the code on just the computer and once again I still have the problem.
Since it seems to be an issue when cutting a circle or something I drew up just a simple circle by itself and generated the code. Ran it and how about that, the problem did not occur. One interesting thing that did occur on just the circle code was when I pushed the stop button an error message came up saying “Radius to end of arc differs from radius to start” (whatever that means). I did not get this when running the code that has the issue.
So far,
•   I push the pause button and the program slowly stops and then I can push start and things start up again OK with both codes
•   I push the stop button and receive the error message when running the circle code, but not when running the issue code.
•   When in stop mode with the circle code running I have to rewind back to the start to get things running again
•   When in stop mode with the issue code I can push start and the program will start running again. It seems Mach 3 is still running the code in the back ground while stopped. And when started the cutting point moves around slowly trying to catch up with where it is suppose to be and eventually gets there. Depending on how long I wait to push the start button is directly related to how long it takes for the cutting point to catch back up too.

This is a strange one and once again any help would be appreciated.

Thanks

Mark

First issue is the machine will be chugging along and then just stop. No repeatability and completely random.

Are there any messages on the screen when this happens?

You should never click the Stop button on the screen while the machine is in motion. You should always use Feedhold, and wait until it stops moving, before hitting Stop. Hitting Stop while the machine is moving will result in a loss of position.

When restarting, you need to either start from the beginning, or use Run From Here. When using Run From Here, don't start on an arc. Typically, the g-code for an arc or circle references the previous position of the tool for the center point. If the tool isn't in the correct position, you'll get the error message you're seeing.

Gerry,

Thanks for the heads up on the differences of the "stop" or "feedhold" buttons.

I have just gotten lucky in the case of continuing on as I mostly use stop.

If this is known to happen everytime (loss of position when using the stop and not feedhold), shouldnt Mach show red leds on the references? I believe mine are still green. Though without some form of feedback thru a scale or encoder Mach would have no way of knowing.

Correct. Mach3 has no way of knowing if position is lost or not.

Thanks All for your inputs,

Gerry, In answer to your question, no there are no messages on the screen.

I have solved my radius error message. Found I had CB and Mach3 set opposite on where the center of a arc is referenced. Set everyone the same, re-ran the tool path and g-code generation in CB, loaded code and ran Mach3 and error message is now gone.
Found my issue with my pendant. I guess I had a brain fart when I built the thing a couple of years ago and I have the pause and stop button wired backwards. No big deal to fix, just swap the plugs inside the pendant. Never noticed the difference, but I pretty much only used the pendant's joystick in the past.
Great explanation on the pause and stop button usage. Explains a lot.
What if one was to set the arc references in both CB and Mach3 to absolute which I have read references the center of the arc instead of a last previous position? Could this setting alleviate the getting lost syndrome?

Thanks

Mark

If this is known to happen everytime (loss of position when using the stop and not feedhold), shouldnt Mach show red leds on the references?

No, it shouldn't.
If you want to stop a program for any reason, you hit Feedhold. Then you need to hit Stop to be able to jog, or edit or anything else other than resume. If it de-referenced and the LED's went red, it would require re-referencing.
Feedhold, then Stop is the proper procedure.

Russ
 

All,

Well, I answered my own question on the arc reference. It does not make a difference changing to absolute as Mach3 still goes haywire trying to regain it's reference.

My issue was trying to resume from program halts which I have learned one does not do. Just re-reference things and start over (Providing one still has a cutter in one piece and the material is not ruined).

Thank you again everyone for the help.

Mark

You can recover, but as I said, you need to use Run From Here, and don't try to start on an arc.