How to recover a CNC program from power failure?

[Bryan Cowan]

Yesterday I was running a sheet of plates to be drilled and profiled. I set the program up to drill all 200 holes for 21 plates. Once that was finished, I secured each plate to the table and loaded the profile program. The program got half way through when we had a power failure.

Whenever I turn off the computer or CAMaster, neither ever remembers the coordinates of where the current placement of the router is. Before the power failure, according to program, the router was at X21 Y15. After I rebooted the computer, Mach3 said the router was at X10 Y42. I have no idea how to "recover" from something like this. This is not good considering the holes were already pre-drilled. My choices at this point are to either scrap that half sheet or take it on the bandsaw by hand (which is what I'm going to have to do).

Is there anything I can do to "recover" from something like this in the future? It makes me to never want to do a full sheet of aluminum (28 x 40) from start to finish again in fear of a power failure, or the computer freezing up.

Any ideas?

Regards,
Bryan

[Eric Mims]

I use Wincnc on my Camaster, but do it like this. If I am doing a big job and am worried about it, I will Home my machine (which uses the hard limit switches). Then I will zero out again on the corner of my piece and then save that position (Wincnc has an option for saving the positions of 10 or so 'home' positions). It always saves them as absolute coordinates. So if all goes to hell, I could come back later, re-home the machine, call back up the home position for that job which takes me to say x10,y11.5, then zero XYZ there and run it. Everything should line up.

If I had not done that, I would probably manually move the machine by .001 until the bit fell perfectly into one of the predrilled holes, assuming the bit diameter was same as hole diameter. Then I would retoolpath the file using that hole as my 0,0.

[Bryan Cowan]

I use Wincnc on my Camaster, but do it like this. If I am doing a big job and am worried about it, I will Home my machine (which uses the hard limit switches). Then I will zero out again on the corner of my piece and then save that position (Wincnc has an option for saving the positions of 10 or so 'home' positions). It always saves them as absolute coordinates. So if all goes to hell, I could come back later, re-home the machine, call back up the home position for that job which takes me to say x10,y11.5, then zero XYZ there and run it. Everything should line up.

If I had not done that, I would probably manually move the machine by .001 until the bit fell perfectly into one of the predrilled holes, assuming the bit diameter was same as hole diameter. Then I would retoolpath the file using that hole as my 0,0.

So all is not lost? I'm brand spanking new to Mach3, so hopefully others who are more versed in the program can chime in and calm my nerves

That's almost what I tried to do. When everything shut down, the router stayed in the profile position. When I powered it back up, I raised the Z-axis but left the X and Y the same. I tried to manually follow the tool path within Mach3 to see which line of code best resembled where I was on the work piece. I found the right line, but even then because Mach3 said the g-code's X and Y were some place else, I didn't know how to tell it otherwise.

I was a very unhappy camper yesterday; still am until I can get this behind me and get those plates cut.

[Rob Wright]

Bryan - I hope you get this worked out.

I use mach3 on my homebuilt. What I have found is that I always do a Ref All Home on startup. This moves the x,y,z back to the home switches and resets the MACHINE COORDINATES to 0,0,0 then I jog the machine to where my JOB 0,0,0 is and zero the JOB COORDINATES by pressing the Zero X, Zero Y, Zero Z buttons. If you then hit the MACHINE COORDINATE button - it will change the X,Y,Z,A coordinates to the Machine coordinate view (redlight lit in around the machine coord's button) I write these numbers down and hit that button again to get back to the job coord's.

If you have a power failure:
restart the machine
REF ALL HOME
Zero X,Y,Z on the screen with the buttons - this sets the JOB Zero at the MACHINE HOME ZERO
go to the MDI tab, type in g1,x???,y??? and hit enter, where ??? is the corresponding x,y coordinates written down.
The machine will then slow feed to the x,y coordinates.
Hit the X zero and Y Zero buttons again to zero the JOB coordinates out.
Reset your Z to the proper elevation (either materail top or bottom) and re-zero that with the Zero Z button and you are good to go!

I know that the camaster Mach3 uhandles the offsets a little different than the Vanilla mach 3, but in the Config Menu, General Config - in the lower right of this dialog there is an option to have persistent DRO's, Persistent Offsets, Otional Offset save, and Copy G54 from G59.253 on startup. If you have all of these checked, when you exit out of mach3 at the end of the day (NOT a power failure ) it will ask you to save the existing position of the tool. When you startup the next time, the tool may still say 0,0,0 or some other corrdinate, but all you would need to do is hit the REF ALL HOME button and mach would then be able to determine just where you are in the world.

At least this is how the Vanilla version of Mach3 works for me. Good luck!

[james mcgrew]

does mach three have a restart function where one can pick the line # to start?

jim

[Bryan Cowan]

does mach three have a restart function where one can pick the line # to start?

jim

No idea. It doesn't even need to start again where it left off. I'll let it go through the motions from the very beginning. It's just the power failure reset all the coordinates. Resetting the home after drilling the holes would have been a crap shoot.

[james mcgrew]

byran, this is something we have all had to learn, i like eric set machine home in the am then i set xy job home for each separate job i also save this position in relation to machine home each time as i do some large 3d and cut work. i know this is possibile in mach as it has been disscussed here on the creek and other forums. i will look at mach today

jim

[Guy Mathews]

Bryan,

Instead of learning Mach 3 to solve your problem, lets solve your problem first and then learn Mach 3.
You layed out a group of parts and drilled all the holes and the power went out. When you layed out the parts in the computer you did it in one of 8 quadrants. I will get into more of that in another post. For now I will set you up in X Positive, Y Positive and Z Positive. Z Positive meaning that I zeroed my cutter off the table top and not the parts.

As you look at this attachment that is the way these holes are laid out.

Untitled-1.jpg

Start your machine and reference it for the manufacturers home position. G28 or whatever command Mach 3 uses to do this. Once this is finished, put in the bit that you bored the holes with and find the hole that is closest to the XY Home that you worked from in the computer. Position the bit over that hole and slowly drop your Z until you are just above the opening. Jog X and Y to get centered as Eric had mentioned earlier. Lower the Z slowly until the bit enters the hole or looks like it will enter with no rubbing on one side to the other. When you are happy that all is centered, zero your X and your Y.
Now use the command line to move the machine position the distance that the center of that hole is to the computer model home position. In the case of my attachment it is Negative X-.75, Y-.75. When the machine reaches that position re zero X and Y. Your machine should now be setup to your computer model.

Raise your Z so you are not going to plunge into the material and zero your Z. half inch or so is fine. When you dry run the program (and you will dry run the program) the bit will just about touch the material but not actually enter the holes. Dry run one time and watch the machine positioning to the holes. If you followed and understood my instructions you will notice the bit centering over all the holes dead center. You can lower it later to rezero off the table, or to the aluminum if you zeroed off of it originally. If you can not zero off the surface, zero off the aluminum and then move the machine to a location that you can hopefully drop the Z the thickness of the aluminum and then zero Z.

This will work because your model has not changed and the parts locations have not changed. The only thing that may be an issue for you is whether or not your CAD or Art program will tell you the location of the hole center. It should, if not, you got robbed!

I will PM you my home number and you can call me this evening if you want me to walk you through it on the phone.

Guy

[james mcgrew]

guy is correct on this, aspire vcarve will set a drill hole based on its center,

[Gerry Grzadzinski]

When the PC loses power with Mach3 running, Mach will not know where it is when restarted. One thing you can try is to use an offset like G55. By default, Mach3 works in the G54 offset. When you home the machine, you zero the machine coordinates. Then, when you zero the X and Y in reference to your part, you're actually setting the G54 offsets. Since G54 is Mach3's default, I **think** you'll lose them when you restart. So, I'd try this.

Home (Ref) the machine to your home switches. Then, switch to G55 offset. Now, set your X and Y zero. Now, go to the offsets page and save the G55 offsets. Then, run your parts.

Now, when the power goes out, restart mach3, home it, and switch to the G55 offset. This should get you right back where you were.

I haven't tried this, as my home built machine doesn't have home switches, but I believe it should do what you want. Just do a dry run test first.

And yes, Mach3 has a Run from Here function which will let you resume from any line in the code.

[Guy Mathews]

Bryan,

...Raise your Z so you are not going to plunge into the material and zero your Z. half inch or so is fine. When you dry run the program (and you will dry run the program) the bit will just about touch the material but not actually enter the holes. Dry run one time and watch the machine positioning to the holes. If you followed and understood my instructions you will notice the bit centering over all the holes dead center. You can lower it later to rezero off the table, or to the aluminum if you zeroed off of it originally. If you can not zero off the surface, zero off the aluminum and then move the machine to a location that you can hopefully drop the Z the thickness of the aluminum and then zero Z. ...

Bryan, one other thing. Once you are satisfied that the machine is or would be redrilling the holes in the same spot and you have rezeroed Z for cutting, disect your code and eliminate the drilling and just do the cutting. You can either post process just the cutting portion, or you can drop the drilling portion of the code if you are comfortable doing it that way. This way, if you are off slightly, your holes will not be elongated and your product will not suffer being off .01.

For those of you who are raising your eyebrows at my last statement, I know what Bryan manufacturers and in this case they are not any parts that are required to orbit the shuttle Atlantis. He can be off .01 and no-one will be the wiser! I am willing to bet he could go to .03 and still be okay since he was cutting and dressing these freehand.

Let me know how it all works out Bryan.

Guy

[Bryan Cowan]

Bryan, one other thing. Once you are satisfied that the machine is or would be redrilling the holes in the same spot and you have rezeroed Z for cutting, disect your code and eliminate the drilling and just do the cutting. You can either post process just the cutting portion, or you can drop the drilling portion of the code if you are comfortable doing it that way. This way, if you are off slightly, your holes will not be elongated and your product will not suffer being off .01.

For those of you who are raising your eyebrows at my last statement, I know what Bryan manufacturers and in this case they are not any parts that are required to orbit the shuttle Atlantis. He can be off .01 and no-one will be the wiser! I am willing to bet he could go to .03 and still be okay since he was cutting and dressing these freehand.

Let me know how it all works out Bryan.

Guy

Excellent, Guy! Sorry I didn't get your PM until this morning, but what you have said I can visualize quite well. I also need to get into the habit of saving the Cut2D .crv file every time I make a change. When I lost power, I also lost the Cut2D drawing with the exact position of everything. The only thing I had going for me was the .tap file for the g-code and the router staying in the last place it was before stopping. I took Rob's advice and Ref All Home, zeroed coordinates, moved to my material's X0, Y0, re-zeroed, and then wrote down the machine's coordinates. I didn't have time to test if this method works, but I will later today.

Fool me once, shame on me...fool me twice, there's a CAMaster for sale.