4th axis woes... parameters question

Hey guys, a bit of a complicated question here;

i'll start with the machine specs:
mill: bridgeport GX480
controller: fanuc oi-mc
4th axis: hardinge model: ?

I'm trying to get the 4th axis working properly. in the past they've just indicated the 4th axis fixture flat and rebooted the machine. as long as you do a g28 c0. before you turn off the machine and never home it, it's good when you turn it back on.

this has caused several machine crashes, which in turn caused .1deg of backlash in the 4th axis, which due to a bunch of reasons gets aggravated if you try to fix it without fixing the ENTIRE problem, so that's where i am right now. i've already set it to be an incremental dog-search type axis as opposed to whatever it was, and changed the rotational direction to be correct.

i have everything fixed except one thing; the machine position shows up as 360 minus the actual position.

eg:
i turn on the machine and home everything.

i put the fixture in and it's 15.5 degrees off (just as an example)

i use the handwheel and indicate it flat

i go to my work offsets page and go to G54 C section, type in C0. and hit MEASUR. it puts in 344.5 degrees.

the machine position reads 344.5 degrees. everything is good so far.

i go to MDI and put in G00 G90 G54 C0.; and it takes me to 15.5 deg. not good.

i manually change my g54 workshift to 15.5 degrees and everything is fine, but that's not what the machine position reads when it's at that position.

ALSO:
when i use the hand wheel and turn it in the positive direction, the RELATIVE and MACHINE coordinates go down and the ABSOLUTE coordinates go up! (only for the C axis though...)

this issue pre-dates the changes that i've made today.


any idea what's going on here?? i've already spent hours setting this up and getting it this far. as far as I am concerned, it's good enough for ME to use, i'm just worried about the next guy to use it. you guys know everything, so as a last ditch effort, i figured i'd post here. Thanks in advance!

The G53 (machine position) of the 4th is set when it is homed. Changing a work offset is not going to change that G53 coordinate. What matters is that when you level it and set a zero in G54, that it stays there when commanded to G54 C0.

If using automatic digitizing to set the 4th doesn't work properly, then don't use the machine input measure function to input a value. Put it in yourself. Same as I never measure a Z work offset using the measure function of my Haas. I have to key in the value. I determine the value by using the machine readouts in jog mode, but it won't write the value I want it to write, so I never use it.

@HuFlungDung: i'm getting repeatability when doing what you suggested, ie. not using the automatic measur input, however, there's no easy readout to use, i have to do actual math! (just kidding) like I said, it's not a huge issue for me, i just want the job to be done correctly for other setup guys in the future. in my experience, if i give them an excuse to crash the machine, they'll do it.

@barbter: there are no grid shift values in the params for the 4th axis, in fact, it couldn't be a grid shift issue, because it's a problem with the coordinate getting inverted, ie. 100 degrees becomes 260 degrees, 1 degree becomes 359 degrees. basically, to get the right number, i have to go all the way to zero and then the same distance past it. the value that i'm getting plus the value that i need equals 360. i've seen machines run the c axis as a rotary one in the past, it's not technically correct, but it's not really an issue. I've already got our post set up for it. edit: we've had no luck with the company that we bought it from. i figured out more in 2 hours today with very limited experience than they were able to in the year that my predecessor hounded them.

edit: thanks so much for the quick replies guys!

Another option would be to set the C axis position with a G92 command when the fixture is leveled. I don't normally recommend using G92, but sometimes on a rotary axis, it's the cat's ass. For example, it can save a lot of unwind time if doing multi-turn work and you don't want to watch the thing unwind it's way to zero all the time. Basically, that is what they're doing if they are using the 'Power off' position to establish a home position. But I'd rather home the indexer and then work from there.

a longer explanation on why we need to home the indexer: since i put in a backlash comp value, that compensation only comes into effect on the first move towards the reference position. normally, i would just tell the person running the machine that as soon as they turn it on, they need to turn the 4th axis in the positive direction, but again, button pushers can't be trusted. my solution was to fix it and make it so that the 4th axis can't be used automatically without homing it first. problem solved, home position is always machine zero, instead of whatever position it was at when the machine was booted up.

the strange thing for me is that two different coordinate systems move in different directions when the hand wheel is turned! the absolute position increases while the machine position decreases...

Are you just homing the machine, or homing and zeroing the machine properly?

On the older Fanuc controls I've operated, after you use the homing mode to move the machine to the home position, you have to go to the position page, press origin and either key in an axis, or hit the "ALL-_AXS" soft-key.

I have a feeling this is your issue, not a parameter or setting.

You have to remember that there is typically no stroke-limit set for a rotary axis, so it will just go around and around and the position display will add up each revolution. 360... 720... 1080... etc.

The same is true for -360...-720...-1080... If you've gone through to -360° and you want to go to 90° in G90 (absolute) the machine can go to -315° in the machine coordinate system.


I made a quick video clip for you showing how this works on my 11M control. Sorry but my 4th axis is not on the machine at the moment, but the procedure is the same. In the video clip, you'll see that after I home each axis, the green light comes on. The Y and Z axis each had 0.0001" showing for the machine coordinate system at the home position. Pressing "origin" softkey and then either keying in an axis, or pressing "all-axs" softkey tells the control to make this position zero in the machine coordinate system.


If you home your 4th axis and it shows anything other than zero in the machine coordinate, you need to use the origin softkey.

On the other hand, some controls are setup to retain the G92 coordinate system offset when power cycled. If homing and zeroing the axis don't solve your issue, go to MDI mode and set G90G92X0Y0Z0A0; That block will clear the coordinate system offset G92 if you execute it at the home position.

@cwtoyota: all of the axis reset to zero automatically when homed. it's not that the value is shifted by a certain amount, it's that when it should be at +15deg, it goes to -15deg (345) the same is true if i try to go to +90deg, it goes to -90deg (270)


@barbter: the axis turns the proper direction, just to the wrong side of zero. it's looking like i'll just have to make a note that you need to make the work shift negative for the C axis and yell at anyone who crashes it :/ Edit: to clarify, it goes to the wrong side of the home position by the amount in the work shift

If i am understanding your issue correctly, have you checked the "mirror image" setting on the settings page? If I remember correctly the "machine" position and actual position will be opposite of each other if it is set to "on"

pgmrmike said:

If i am understanding your issue correctly, have you checked the "mirror image" setting on the settings page? If I remember correctly the "machine" position and actual position will be opposite of each other if it is set to "on"

Click to expand...

That's it! thanks you so very much! i was convinced that with all of the bodging that had gone on, someone had screwed up a parameter.