How to Pause, Move x,y,z, Resume?

[GJeff]

Often times when I pause a program is it to make workholding changes, which means i need to move axes in order to do so. However, pathpilot won't let you move xyz when paused, even if you're a good boy and move them back to where they were.

What I'd really like is an easy way to interrupt a program, move, turn off spindle, do my stuff, return to the previous state where spindle is on and XYZ is recalled, then resume the program. Does such a thing exist? Resetting the program and restarting from the line you were at is not it!

Similar Threads:

• Pause/Play and power off resume is possible with our prusa i3
• Automate Pause / Resume of NC Program
• Problem- When I click Feed Hold, then move Z, then Cycle Start - does not resume properly...
• Need Help!- How to Pause G-Code Program, Manual Tool Change and ReZero, and Resume
• How to pause and resume tool

[wtopace]

It doesn't exist. I sent a few suggestions early on to them regarding this, but nothing was ever implemented.

The best work around is just to hit reset, make your changes and use the right click -> set start line option in PathPilot to resume.

[GJeff]

Yeah I'm not happy with that method. Hard to find the line again with big files.

I guess if you know where you want to break you can put a force tool change in the code. Gonna try to get that to work.

[wtopace]

As far as I know, a tool change won't allow you move control.

[Jim Dawson]

Is it possible to make it do a ''tool change'' at that point in the program? Or perhaps just manually write in some code that sends the Z and table to a safe location then execute a G4, M0, or M1? Or maybe just make the cut in two separate operations with a G4 between them?

EDIT: OOPS, we were posting at the same time.

[wtopace]

When you move your work piece around, you probably need to reconfigure your G54-59 offsets, right? Unless you have a bunch of fixtures you're moving in between, in which case it wouldn't take much longer to just load different code or run the fixtures simultaneously.

If you're just wanting a pause - hit spacebar and turn off the coolant, keep yourself away from the spinning tool though. PathPilot will still lock out any ability to set zeros, tool offsets, etc...

[GJeff]

Forcing a manual tool change is working out well since it moves the spindle to max Z and waits for me. I don't think it allows movement, but I don't really need it so long as it's out of the way.

[mountaindew]

They added search in the code window! This helped me to go back to having fun. Stop program, Change fixture, change and or set offsets, whatever then
I search for offsets g54 -g59 because that is where I do the most "AU" Auxiliary operations . Pointer jumps to that area, scroll around to logical start of operation or offset or at the point you stopped , set start point. Then hit run. Not Ideal but solid simple way to navigate large programs with multi sided parts.
If your careful how you setup your cam operations and offsets and work stops. I can do one complete part setting all the ucs for that part along the way. Next part all I have to do is re-fixture stock for each operation set and no need to set any offsets.

[GJeff]

Ah ok, having search makes it a lot more manageable.

[RTP_Burnsville]

Thanks for the tips.....

I still wish the tool change for PP operated like MACH. I mostly do one-offs so having to enter every tool in the table is a huge pain. I like PP overall, but the tool change run-around is almost a deal breaker.

Robert

[GJeff]

Wait a minute.......

I haven't actually had to do real tool changes yet. This means when I change an end mill on my companion spindle, there's absolutely no way I can set the Z without restarting the program.

That.
Sucks.

I officially regret spending the extra money on the legit Tormach controller. I should have just built a Linux machine and did my own linuxCNC controller. A controller should give you control, not take it. *Trump Tweet Voice* Not cool. *End Trump Tweet Voice*

[GJeff]

And I just want to be sure: This is a special limitation that Path Pilot has put in place, correct? Or is this the way it works with all LinuxCNC setups? Is there a way to allow motion in the LinuxCNC config file?

[RTP_Burnsville]

GJeff,

I believe the tool change limitation is built-in to PP which is just a tweaked version of LinuxCNC. From what I have read, there is no current work-around. BTW: I have PP running on an older ASUS motherboard which I had sitting around. It has been working fine for several years and ran MACH prior to the update. I initially tried PP on an IBM ThinkCentre, small form factor PC, but it did not play well with the built-in display adapter so used the ASUS box.

Robert

[phomann]

Not being able to pause, jog around for tool changes, clean swarf, etc is the main reason I use Mach3 instead of LinuxCNC.
For me it is a necessity I can't do without.

Cheers,

Peter


Sent from my iPhone using Tapatalk

[pickled]

Begged for this in the beginning and was told "not going to happen" several times. I have changed my workflow a bit and have gotten used to not having the ability that I had in Mach3, but I still WANT to be able to do it on the fly. When you are prototyping, just working on a one off or changing out a dulled or chipped tool being able to pause, reset Z and move on without dinking with offsets and finding line numbers is handy! There will be many weeks where I will run with NO tool offsets at all in the table when I'm shaking things down and optimizing tool paths. When I want to make a production batch then things are quite different. I sure can't complain about the stability of PathPilot though!

[petenc]

Begged for this in the beginning and was told "not going to happen" several times. I have changed my workflow a bit and have gotten used to not having the ability that I had in Mach3, but I still WANT to be able to do it on the fly. When you are prototyping, just working on a one off or changing out a dulled or chipped tool being able to pause, reset Z and move on without dinking with offsets and finding line numbers is handy! There will be many weeks where I will run with NO tool offsets at all in the table when I'm shaking things down and optimizing tool paths. When I want to make a production batch then things are quite different. I sure can't complain about the stability of PathPilot though!

I've been thinking about this, and can't see it without edits to PP. What if... there was just a way, that whenever the program was aborted, it would take a snapshot of the safety line (work offset,tool offset, spindle rpm) and generate a "new" program that had the remainder of what you were running. And if life was really great, add it to the dropdown list? I know I am reaching, but hopefully it stirs up some other ideas.

Pete

[wtopace]

Wait a minute.......

I haven't actually had to do real tool changes yet. This means when I change an end mill on my companion spindle, there's absolutely no way I can set the Z without restarting the program.

That.
Sucks.

I officially regret spending the extra money on the legit Tormach controller. I should have just built a Linux machine and did my own linuxCNC controller. A controller should give you control, not take it. *Trump Tweet Voice* Not cool. *End Trump Tweet Voice*

It sounds like you may be new to your Tormach (congratulations!) and maybe new to CNC in general. Here's a free tip (so take it for what it cost you) - ALWAYS maesure and enter all tools into the tool table. The TTS system gives you a very decent amount of repeatability and by touching off every tool at runtime you absolutely will break tools due to negligence (not to mention inaccuracies in Z). I attempted to go down that route in the Mach3 days when I first received my 1100, broke 2 tools day 1 due to offset issues. After that, I vowed to never "touch off" a tool again - not a single broken tool due to tool-length-offsets.

My workflow:
1) Keep tool table up to date
2) Before a new part - add new tools if any
3) Set G54-G59
4) Run a quick sanity check: Insert a few of your programmed tools and "G0 Z6" - then put a 6" rule standing up on the G54 Z0 of your part, does it meet up with your tool tip? Great. Nope? Uh oh, stop!

Using a tool table isn't a Mach3 or PathPilot thing - It's a CNC thing. If you have a repeatable Z-height tooling system, learn to use it and don't look back.

I think you'll find a 99.9% agreement that PathPilot / LCNC are in a different league than Mach3. I would compare them closer to my "real" Fanuc controller than Mach3 in most areas.

Good luck!!

Edit: Just realized you were talking about your companion spindle (guessing this is the router that clamps on the main spindle?). I don't own anything like this and have never had the need for it, so I can't offer any assistance there.

[samco]

That is a fundamental limitation with linuxcnc. Lots of discussions about it. I don't see it changing any time soon. In linuxcnc prime there is a 'move off' component that will allow you to move while paused. this will not let you change a tool length on the fly.

2 things come to mind that work very well (as stated above)
- run from line.
- tool length probing. (having a switch on the table that probes the tool length after tool change and uses the measured tool length. - I don't know if path pilot allows this?)

I can see where jog while paused would be cool - but I have never missed it.

sam

[109jb]

Unless things have changed since I worked on production machines (25 years ago), they don't allow jogging while paused either and this may be why LinuxCNC/Pathpilot don't either. Basically to remain consistent with commercial offerings. When I worked on those commercial machines, operators would commonly watch through the glass for a spot in the G-code run where the tool was clear and the machine could be paused to check something or do what is described here. For production runs we would occasionally modify the G-code to include a Z-retract, spindle off, coolant off, and M0 or M1 command once we knew where in the program it was desired.

I can think of one reason not to offer jogging while paused. If the machine is allowed to jog during a pause, and then when resumed the next line is a G91 move. This could have catastrophic results.

However, particularly for smaller machines without automatic tool changers, it would be nice to have a way in either PathPilot or LinuxCNC to be able to jog during pause for a variety of possible reasons. I myself have split programs apart for this very reason.

[mountaindew]

production machines (25 years ago), they don't allow jogging while paused either and this may be why LinuxCNC/Pathpilot don't either. .

Tormach basically told me this, and noted they would research this behavior. I was totally frustrated when I started using Path Pilot because of this.
After fretting for weeks over this I decided to refine a process to work with it. I tend to resist what I dont like then adapt. Doing almost 100% multi side and offset parts I was surprised that I could setup sprutcam to pause and prompt me to do whatever was required.. At that point I stop program and code pointer returns to start. Then I perform fixture change or whatever. In past, on long programs I would note about where the scroll bar control was on screen then drag it back to that point and was in the right area of program code. Then set start point on a line I had sprutcam pause on. Hit start and with no frills it begins. Recently they added search and what a difference for me. It's easy to find that exact line and better yet have your cam put a note at points in code to search for.
As I noted above with good position stops for fixtures or material you can do one part complete on the fly setting all offsets and changes. Then next part can be done with little effort and reason to stop code, Just perform the changes to fixtures and stock and continue.

Mach confused me with its preparatory moves and the code pointer jumping around in code window. Not bad after you get use to it but confusing at first.