G68.2P0

[JSwistak]

to cncappsJames because of an older thread he was on:

      I have been reading an older thread from 2022 about setting workpiece error, so I am coming into this conversation because we have a new 5 axis horizontal trunnion machine here and we are all new to G54.4 and TCP G43.4 programming. I am working with the operator on the machine to figure out where we put in our fixture offsets and any workpiece location errors or differences-- and that is covered above. Its funny but the Fanuc America videos on the subject are very clear about G54, G54.4 and finally G68.2 EXCEPT where to store fixture offsets and workpiece location errors. All of the work in the videos is done by probing with values loaded automatically.  We are currently working on all of this based on the excellent thread above and the screenshots of the machine control. 

     We have done lots of vertical 5 axis programming using G54.2P1 so we are moving up to the G54.4 etc. My question is why is G68.2 in the code at this point?  We have a brand new post from Postablility and so we have a few kinks to work out- but isn't G68.2 a specialized local work plane for only certain tilted work plane scenarios?  Is it okay to turn it on right away, because our new post turns on G68.2 right away.  In the Fanuc America videos G68.2 is on a .pdf but not really covered as much as G54.4 and G05.1Q1 nano smoothing. 

[Leon82]

our Camplete format uses g68.2 to get into position and then cancels it on g43.4 5 axis work.

They can work together 54.4 would compensate for a crooked casting or fixture and 68.2 will let you have a work offset other than the center of rotation.

I TRIed it on ours once but with a table table setup it couldn't get to a proper solution

on the work offset screen page over with the right arrow untill work error shows up. thats the 54.4 table

[Kyle F]

21 hours ago, Leon82 said:

our Camplete format uses g68.2 to get into position and then cancels it on g43.4 5 axis work.

yup even Haas goes about it the same way, G254 DWO to position and then turn off, and activate G234

[cncappsjames]

What the pre-position does for you is create a safe and known transition from path to path. 

If you want sexy, YouTube worthy machine porn, there's a path in Mastercam (5-Axis Linking) or CAMplete's Auto-Link function (it requires an NC Format that supportsthe function. It has to be turned on also... by default it's off.

If you want to know how to turn it on, let me know. 

[Kyle F]

I've never had an issue with the mastercam 5 axis link. Generally I'll prove the program out with forced tool changes between each multiaxis path and then once I have them all dialed in I'll go back in and add the multiaxis link. Then go re-prove it out again lol

[JSwistak]

You guys are great- we are working on all the above. Thank you

 

[cncappsjames]

On 4/24/2024 at 4:38 PM, Kyle F said:

I've never had an issue with the mastercam 5 axis link. Generally I'll prove the program out with forced tool changes between each multiaxis path and then once I have them all dialed in I'll go back in and add the multiaxis link. Then go re-prove it out again lol

I typically do not use those 5-Axis linking strategies, or if I do, I use them sparingly. Transition from operation to operation can be tricky. You can get wild unpredictable motion. Much of the motion is dictated by machine parameters (wind/unwind/rotary axis rollover, etc...)

In a multi-pallet production environment where unattended operation is the main goal, safe and predictable is your friend.

[Kyle F]

1 hour ago, cncappsjames said:

I typically do not use those 5-Axis linking strategies, or if I do, I use them sparingly. Transition from operation to operation can be tricky. You can get wild unpredictable motion. Much of the motion is dictated by machine parameters (wind/unwind/rotary axis rollover, etc...)

In a multi-pallet production environment where unattended operation is the main goal, safe and predictable is your friend.

I can definitely see your point. I will stick to forced tool changes between multiaxis operations on the Matsuuras then

For the Haas I have found some "workarounds" that seem to really smooth out the process. Main one being under "feed rate control" in a multiaxis toolpath I will have checked "custom feedrate for clearance blend spline" and "replace rapid with feedrate".

and then under the multiaxis link settings I'll have it checked to output feedrates as well. I'll usually have them set around 50-100 inches per minute (with butt puckered and hand on the feed stop button) to first prove it out and if the motion is smooth out at the machine I'll up it to 200-250. Essentially this will force all of the multiaxis toolpaths to stay in TCPC during relinking (while in that operation) but during the actual multiaxis linking moves it does swap back to dynamic work offsets (haas g68.2) so I am still technically rolling the dice a bit. 

Now really thinking about it I'll probably stop using the multiaxis link on the haas just for standardization's sake though  especially since eventually I'll be too busy to prove out every single multiaxis program.

Appreciate the insight!

[Leon82]

On 4/24/2024 at 11:07 AM, cncappsjames said:

 

We have the 1053 delimit tool path setting on as a recommendation from Camplete. What this does is on 5 axis paths since there is no transition block it zero returns z and starts the next path, no tool change spindle keeps running. It doesn't affect 3plus2 because there is an approach block short that transitions to the next path.

 

I did mess around with the multi axis linking in Camplete but for us it's not worth using.

[cncappsjames]

I've got my NC Format set to be able to use both Auto-Link or Mastercam's Linking... just on the off chance I want it.

Being in feed mode (as opposed to rapid mode) while in 5-Axis is essential for smooth positioning. Some CAM systems struggle with this. Fortunately CAMplete can correct that issue if it presents itself. 

[Kyle F]

16 hours ago, Leon82 said:

We have the 1053 delimit tool path setting on as a recommendation from Camplete. What this does is on 5 axis paths since there is no transition block it zero returns z and starts the next path, no tool change spindle keeps running. It doesn't affect 3plus2 because there is an approach block short that transitions to the next path.

That's awesome. I have only ran 3+2 jobs so far on the matsuuras so I have yet to feel the need to tackle this subject but this sounds like a great way to go about it. I do not mind a Z retract at all, but the M05 + M09 for no reason between toolpaths would probably be a little annoying if I was feeling O.C.D. haha

Always a fun line to walk when trying to appease my O.C.D. and just let "good enough" be good enough. Usually how busy I feel dictates my decision.

[cncappsjames]

Appeasing the OCD and what the machine actually cares about are more often than not completely seperate issues.

For example I will typically have an S code, then have the M03/M04. In my NC Format, one situation will have the M03/M04, then the S code. I twitch when I see it... but I leave it there on purpose just as a reminder that it REALLY does not matter one single bit. The control executes the block just fine with zero issues. My OCD with code borders on the absurd.