[peter.blais]

Hi guys

I've got a new lathe here with a fanuc Oi-TD controller on it and i'm using gibbs 2010.

I was dry running the very first program last night, with the feed on like 10% and the rapid on zero, door open, etc. All was well roughing with the first tool, it moved out to the clearance point.... (Xd 2.25", Z .1" - on 2" bar)....

Then the damn thing rotated the turret right there and whacked a .625" HSS drill off on a chuck jaw.... Not a good way to break in the new machine. I was running it in the air, with 4+ inches from the chuck- but apparently not quite far enough lol. Damn turret was just too fast to catch too.

Anyways, when it goes to change tools, I now see that it just does a G00T0202... There is no position move, I was thinking there should be a G28 in there first, to get it far away & safe... This lathe is just a baby, and it's fast, so I don't mind it going all the way home to change tools. It can't hit the tailstock either, if it's parked in it's usual spot.

In the document setup tab, I do not have the check box selected where you pick another tool change location... I was under the impression that with that un-checked, it would use the reference position.

I'm using a Fanuc post for an Oi that was provided to me by gibbs.

TIA for any help guys! I will call them on monday but it's bugging the hell out of me.

PS: Think my turret is knocked out of alignment from that little drill removal session? The machine didn't alarm out or anything, don't think it was too bad. Chuck was only going 300 rpm too, thankfully- glad I don't have any pieces of HSS embedded in my face.

[trevj1]

Me. I'd check the tool change position box, set a safe position, and run (at a positively safe distance) it to see if that was all it needed.

Try just posting the output with the changes, and having a look to see the difference.

I'm getting to know my way around Gibbs a bit better, and my main bugaboo is that the process dialog boxes insist on remembering details from the 'last' job. <sigh> Getting used to checking those carefully!

Can't help you with the alignment possibles. I'd be measuring, not guessing.

Cheers
Trev

[peter.blais]

Ya, I decided I had better RTFM... It does in fact require that- I wish there was a way to just set it to go home. Now i'm trying to run it in the air a ways back, and of course I don't have enough travel to do that without over-traveling on some of the longer tools, since it always tries to go back 4" or whatever. Move the air machine work forward enough to clear in the back, and I'm within striking range of the chuck again... *sigh*

It looks like one could leave it unchecked, and add a line of code before each tool change which would G28 it home, but i'll leave that for another day. I think I'd rather have my guys not do that anyways, if they forget it we'll get a repeat.

We bought this lathe for making itsy bitsy stuff- like .75" diameter by a quarter inch long- of course the first part i need- spindle liners - is a lot bigger. LOL

I'm gonna check the turret on monday, I suspect that no harm was done, other then ego / confidence haha.

[trevj1]

Racking my memory here... Check the settings for clearance distances. There is one that makes the tool retract before anything else happens, and it was my bane for a while on our milling machine with it's limited travel, as it always wanted to retract before starting anything, so it overtravel alarmed out. Cannot recall where that was though. I seem to recall thinking it was not in a very good spot. Books! Gotta hit-em. Sorry I couldn't be more helpful.

Possibly in the "Documents" page?

Cheers
Trev

[peter.blais]

FWIW- guys- I got them to give me a post which just sends it home as the default toolchange location.

I think you could enter it per tool if you really wanted, but I have a wee lathe with fast rapids, so I don't care.

Thanks guys-

[rhundl]

I always check the box for tool change position and just use x10 and z10. But it sounds like you got it figured out. Also run the option stop on your machine for proving out your programs, its a simple way to catch those little mishaps before they happen. Once you know everythings clear then turn it off

[glenthemann]

This is why you run through a program for the first time in single block as well as dry run..

You should have been able to see with your own eyes that the drill did not have enough room.

I always keep my tool calls on their own block.

You can never, imo, rely on any cam software to provide you with 100% fool proof code such that you can simply upload the program and hit go.

Be more careful, single block is your friend. Use your eyes. Sending the entire turret home after each tool is a good way to double your program time for no reason.

Heres a tip, say you want to set T0202 which comes after T0101. Call T0101 in MDI and then manually index the turret to T0202, jog T0202 to a position you feel is safe, the position screen will show you the current location that T0101 would be in. This is now your retract position for T0101. Retract T0101 to this position before T0202 is called and you end up with T0202 right close to your part without any interference.
This makes things a little sketchy if youre gonna be constantly changing tools, ie. to a different drill with longer flutes, etc. You just need to set things within your personal comfort range. Personally Ill index within .05-.1" of the part.

[jeffliu2]

Heres a tip, say you want to set T0202 which comes after T0101. Call T0101 in MDI and then manually index the turret to T0202, jog T0202 to a position you feel is safe, the position screen will show you the current location that T0101 would be in. This is now your retract position for T0101. Retract T0101 to this position before T0202 is called and you end up with T0202 right close to your part without any interference.

That's good idea!

[Joemachine]

I saw a slick trick from a clever mechanic to check or set turret alignment. He chucked on a large diameter, facing it off all the way to center. Then mounting a magnetic indicator on the turret, he moved the turret on it's x axis while probing the OPPOSITE side of the disk that the tool went across. It showed twice the error of misalignment.

Joe

[Rockyluc2000]

Here's A neet trick. Read the manuals. I am not an expert by any means. but as an operator for twenty years i have realized some things over the years. And first off Glentheman is correct. Any new program or Job you setup and run, single block and Dry run our your biggest friends. I would also Like you to try something and watch what happens. Send the Axis's to the home postition and call up T0101 and watch the absolute position page and then call up T0100 or T0202 and look at the absolute position page. these numbers should change depending on the tool offset that is called upon at that time. My point here is there is a way to get the machine to a true Safe index positition without taking the offsets into the equation. There are also other factors that can play a role in the safe index positition. So what i am trying to say here is you should always be looking for a way to send the machine to a machine position (Safe Index) without Tool offsets , Work coordinates, workshifts getting involved