[SSMrob]

All,

Been having some issues.. Got the tool change to work pretty well, however..

It seems as if after the G27 moves the Z axis to home position and all other toolchange related items are performed, I am having trouble getting it back to my WCS.

I am assuming that this is because G27 switches the machine from WCS to MCS to perform the Z origin to ready the machine for the tool change, and then does *not* automatically switch it back after the tool change is performed?

So, it looks like I would have to give it a G54 command to switch it back to the WCS?

Now, my next question is, after the tool change is performed, do I need to first move the Z axis downward using a MCS value simply to get it off of the MCS Z origin *before* switching to WCS1 (G54)?

Haven't really messed around much with the toolchanger until recently, and the documentation is *terrible* for tool changes! It doesn't say anything about the machine going to MCS mode during the G27 command, nor do the examples show the use of G54 after the G27 command.

Im thinking its as easy as invoking G27, performing tool change (M06 T05), G00 down in Z to some negative direction to get it off the origin switch, switch from MCS to WCS1 (G54), then invoke tool length compensation (H5) and continue with the program?

If you utilize G92 to set your part origin, does it automatically use this offset and save it to WCS1? Or is there another command to set the current coordinates of the tool to one of the WCS registers?

Thanks in advance!

[txcncman]

Not familiar with the specifics on your control. Most Fanucs I have worked with use syntax similar to the following:

G00 G91 G28 Z0.
T01 M06
G00 G90 G54 X0. Y0. S2000 M03
G00 G43 Z1. M08

[fordav11]

G27 goes home to an exact position in the WCS then checks it to make sure it is at the zero return position. So your machine is not switching to MCS.
G27 is kind of pointless. Most people don't care if the machine thinks it is there or not. They just want it there regardless. So use....
G91 G28 Z0
G90

On the older controls like yours to set the WCS requires a G92 X Y Z
G54-G59 is an option on the early controls. Does your 3-series have it? If you do you should have a screen for setting it showing G54 to G59.
If not then you must use G92 to set your XYZ position. Then use G43 Hxx to read the tool length offset. You don't need an intermediate move to get it off the zero return position.

Also if you do have G54-G59 the machine powers on in G54 mode by default so you are never in MCS unless you program it. You may have some parameters not set correctly causing it to cancel the WCS or something? You would need to check your parameter manual.
The early Fanuc manuals have the parameters in the back of the operator manual so maybe yours is the same.

[SSMrob]

G27 goes home to an exact position in the WCS then checks it to make sure it is at the zero return position. So your machine is not switching to MCS.
G27 is kind of pointless. Most people don't care if the machine thinks it is there or not. They just want it there regardless. So use....
G91 G28 Z0
G90

On the older controls like yours to set the WCS requires a G92 X Y Z
G54-G59 is an option on the early controls. Does your 3-series have it? If you do you should have a screen for setting it showing G54 to G59.
If not then you must use G92 to set your XYZ position. Then use G43 Hxx to read the tool length offset. You don't need an intermediate move to get it off the zero return position.

Also if you do have G54-G59 the machine powers on in G54 mode by default so you are never in MCS unless you program it. You may have some parameters not set correctly causing it to cancel the WCS or something? You would need to check your parameter manual.
The early Fanuc manuals have the parameters in the back of the operator manual so maybe yours is the same.

Well, this old piece wants G27 or else lol.. It needs that origin light to come on, or no tool change. And if you send it to Z0.0, it still will not allow it to toolchange. As a matter of fact, if you hit the soft reset button for any reason, the Z axis needs to be rezeroed, or it will hang on a toolchange the next time.. Ugh...

The machine DOES NOT have G54-G59, so it looks like everytime I do a tool change, I need to either calculate what the difference from the toolchange position Z and the workpiece, then either use G92 Z0.0 once it gets to the offset.

So, ok, here is what I have.. In the position, I have machine (in metric).. That never changes... I have Absolute (this is tied to G92 and/or gets reset in Z when you perform a toolchange/origin), AND, last but not least, I have Relative (this is the one you can zero by pressing axis button (x,y,or z) and hitting CAN.

So, from what I found, it must be G90 G27 Z0.0 Txx M06 or it just doesn't work... Actually got G28 to work too, dunno what the difference is really?

Now, the big question is, how do I get it to use the relative position for the program after a toolchange? Z rel is 10.7 (which is correct to run my program) and Z abs is -2.72.. It seems to be defaulting to the abs ie machine value.. Is there an easy way to do this?

Thanks again, I almost have this working...

[txcncman]

What about cancel tool offset and use G53 Z0.?

[SSMrob]

What about cancel tool offset and use G53 Z0.?

Eh, just found out my machine doesn't recognize G53.. Oh what fun this is! Esp. since it says in one manual it *does*, just like it also says it recognizes G54 So far, I have gotten G27 *and* G28 to work to allow a toolchange.


Now, my biggest problem is once you perform a toolchange, any G92 value you had is toast. Z automatically zeros out..

So, I switch to metric G20, I G00 to the abs coord value of my zero (in this case, -251.55mm), I then switch to G21 (inches), and then initiate my tool offset (Hxx).. I have to switch to inches because the offset values were done in inches.

Here is what I have so far, and the offsets now seem to work.. Just want to be able to switch tools and get the thing back to the same workpiece origin that it is at before the toolchange.. Getting really close...

G90 (abs)
G21 (switch to metric)
G28 Z0.0 T01 M06
G00 Z-252.705 (puts me at the Z zero for the part)
G20 (switch back to inches, because thats what the L offsets are in)
G92 Z0.0 (reset the zero, because it would have been -252.705)
G00 G43 Z0.0 H01 (adopts the offset value in H01)
G92 Z0.0 (sets zero to include the H value)
G00 Z3.0 (moves tool up 3 inches)
M30 (stop)

Let me know if this sucks lol..

[SSMrob]

Ok, screw this lol..

The machine *will* offset the tool length correctly, *however*, it will ignore any subsequent G92 once a tool length offset compensation is in effect. I *can* perform a G92 only *if* I give it a G49 *first*. However, then, the tool automatically moves upwards (all my tool offsets are in the negative) which screws up my plans..

So, looks like I have give up on the tool offset G44/43 Hxx and just perform it manually using G92.. What a crock, but, it doesn't seem to want to do it otherwise.. If the Hxx is any non-zero integer, then it doesn't work.

Ugh, gotta love these old machines, so much mystery, so many bad manuals contradicting other manuals.

Well, it is a 3m and from what the Fanuc tech told me, there was a LOT of bad ideas in this particular Fanuc controller, and alot of things that changed over time so its hard to tell what you have even by the serial number.

[fordav11]

as far as I know operation and programming-wise 3T/M is just the same as 6T/M. I worked a 3T for a couple of years (Wasino LJ-4 with 3T-D). It was the same except it had FAPT where the 6T didn't.

the correct format is to use G43 H then at the end after you finish with that tool give it a G49 to cancel the tool length then G28 to Z0 (home)
if you follow the right programming procedures it will work as expected.

you set the G92 X0 Y0 as usual and the Z is the distance from the spindle face to the work Z0. the tool lengths are set from the same face to the top of the job.
if you set it right and program it right it should work.

but in case it doesn't use a G92 XYZ on each tool. that's the same thing as setting one G92 Z and offsetting the tool lengths with G43.
you just need to put each tool in, zero the Z position in relative then move the tool to your Z0 top of job then whatever Z reads put that in the Z for the G92.
if you do it this way you need to have a G92 XYZ at the beginning of each machining section when changing tools and for *each* tool but you don't need to use G43.

also, it's a *****REALLY REALLY BAD IDEA***** to switch inch/metric in the program. Use one or the other. If offsets are set in one, re-set them so they match one system. Otherwise one day you'll mess up and your machine will try to drill to China.....

[SSMrob]

Originally I had the g49 on the second line. As far as switching from inches to metric and back again, only way I can get an accurate return to zero every time since the machine is in metric when you use the machine coordinates and it doesnt have g54/59, which you must use for repeatability, plus I am using a dripfeed ROM which seems to be causing the machine to hang on g92 only when a nonzero int is present for the current h offset value. When I had the base roms I didn't have this issue.


I guess I could redo/convert all my offsets to metric also. Not a big deal really but still have to do a g20/21 switch at some point.

Guess my progging will all be going to metric soon lol.

[fordav11]

why not just change one parameter and use inch system?
it can be set on the same page where the IO channel is set.
does your machine have a screen or just 8 RED LED display?

[SSMrob]

I will try that, but, from what I gather, the machine is always natively in MM, and thats what it switches to when you perform an origin ie G27 or G28. I will give it a try and see what happens.

[indymx6]

You ever get this figured out?

[SSMrob]

Yep, just a bit tricky... Had to use G92 in the middle of the tool change to set the zero, then, G92 again to set the offset.

Don't know why I needed to go G92 again, I tried to move it to an arbitrary zero point while in G21, G92 and set zero, then, switch to inches (g20), then, G92 again to set the tool offset manually.

U still want this RF30? I put it up on Craigslist just to try to avoid ship cuz its going to be a pita.. Still gonna cost ya about $800-900 to the door to get it to you.. I put all the tooling and whatnot that going with it in pics.. Take a look when you get the chance...

[indymx6]

I definitely still want it. I'll have to do some checking on shipping.