[Dave1]

Anyone,
I have a question on canceling offsets. I changed the parameter to apply the tool offsets by shifting the coordinate system instead of tool movement. When/if I use wear offsets they do not cancel and I end up with an overtravel alarm. Any remedies? Thoughts?
Thanks,
Dave

[bborb]

Does your tool callout use 4 digits?

T0202 (Tool station2, offset 2)
G0X1.Z1.
machine code
machine code
G0G40Z1.T0200 (cancels tool offset)
M01

Does the above code look familiar? Make sense?
What does your code look like?

[L. Sakthivel]

Try P 13.3 to 1 for Tool Geometry compensation is cancelled by position No. 0 &
P 14.1 to 1 forTool Geometry compensation is cancelled when the Reset state entered.

[Dave1]

Try P 13.3 to 1 for Tool Geometry compensation is cancelled by position No. 0 &
P 14.1 to 1 forTool Geometry compensation is cancelled when the Reset state entered.

P 14.1 is currently set to 0,,,,, P 13.3 is already set to 1
I will give it a try, thanks.

Bborb,
My code looks like what you've posted and I've tried T0000 with no luck


Dave

[bborb]

Parm 13 bit 1 A tool geometry compensation number is specified using the least significant/most significant digit of a T code.

[Dave1]

Parm 13 bit 1 A tool geometry compensation number is specified using the least significant/most significant digit of a T code.

Parameters are as follows,
013> 01101100
014> 00000100

It should work as it is (I think) when I cancel and change tools I write,
(blah, blah, code)
G00 Z.5 (some arbitrary clearance point)
T0200
G0 G28 U0 W0 (machine reference point)
M30
Then I get an over-travel alarm but only when using wear comp, if wear comp is at zero then all is well. Machine uses G50 work coordinates, not G54-G59

Dave

[bborb]

Did this machine cancel the offset the way you liked BEFORE you changed parameter 0013 bit 2 ?

Can you try this? (below)
G0G28U0.W0.T0200 (cancelling in a motion command)

Also, param 13 bit 3 (which you have as a 1) says Tool geometry compensation is not cancelled/is cancelled by position number 0

so T0000 should work (I think)

G0G28U0.W0.T0000
M30

[Dave1]

Ooops, I goofed. The parameters listed above are what was originally in the machine, It originally applied and canceled the offsets (wear included) by moving the axis. (Which I didn't like at all) So, parameter 013 has been changed only by shifting the coordinate system (new value> <013> 01101000 I was reading the original parameter list (I made a backup before anything got changed)
I'm sorry for the screwup(nuts)

According to the book, 013 bit 3 is enabled with (1) thus canceling the offset with an offset call of 0, if bit 3 was set to 0 then the offset would be active until the next tool and tool offset call (that's the way I would understand it anyway) Correct???

Parameter 014 bit 1 currently (0), the book says' (1) cancels the tool geometry offset vector by resetting ( I wish there was more of an explanation about this, seems confusing as to what is actually going on)

Dave

[bborb]

My literature says "position" zero and your literature says "offset" zero.
So.....T0000... that's a "T" and 4 zeroes, should work. At least its worth a try.
Tool zero offset zero.

G28U0.W0.T0000
M30

[Dave1]

Here's what I've noticed, the wear is applied by an axis movement, not by coordinate shifting. When you call a tool, I.E T0606 and that tool has some wear applied to it, the axis moves and apply's the value before any positioning command has been issued????
Is there a way to change it so the axis does not physically move? I'm new to Fanuc and their way of thinking, don't know why you'd want any physical movement from the offsets/wear?!?!?
Dave

[L. Sakthivel]

Geometrical offset is common to the whole Program, Tool wear offsets are changing according to Tool, so if we are entering the wear offset system shift the axis position according to the tool calling, it willnot reflect in the axis movement display. Because One program contains so many tool callings.

[Dave1]

Geometrical offset is common to the whole Program, Tool wear offsets are changing according to Tool, so if we are entering the wear offset system shift the axis position according to the tool calling, it willnot reflect in the axis movement display. Because One program contains so many tool callings.

Yes, but, why the motion then, why did they not have it shift the work coordinates like geometry offsets?? While I realize the wear offsets in most cases are small, (.0005, .001-.005 max?) maybe they (Fanuc) didn't think it would be a problem?? Next time I run it I'll try the wear offsets again and see what happens.
Dave

[cacrawfo]

Dave,
The early Fanuc stuff is just like that, and I have found that you just need to adjust your programming style to match it.

Here is how I program on my lathe with 6T:

(program starting info, set for inch, etc.)

N01 (CNMG 432 turn and face)
G28 U0 W0 (home axis for G50 setting)
G50 X10.5655 Z13.3554 (set coordinates)
T0100 (Indexes turret to station 1, no wear offset called, no movement of axis))
G97 S400 M03 (Set speed, start spindle)
G00 X1.6 Z0 T0101 M08 (rapid to part, call wear offset, turn on coolant)

-Machine part-

G00 X1.6 Z.1 T0 M09 (rapid safe distance off part, cancel wear offset, turn off coolant)


By indexing the tool seperately from instating the wear offset, you can instate the wear offset in a movement command. The movement and wear offset are calculated together, and the final position includes the wear amount. This way, there is no "jumping" as there is if you call the wear offset while sitting on the home switches.
Carl C

[Dave1]

Carl,
Thanks, that is the answer I was looking for. It is what it is then and there is no magic parameter change to stop it from doing "The Jump". I can certainly program it the way you mentioned although, my cad/cam post will need to be changed to call the tool in the first position move. BTW, I don't ever put the G50 coordinates in the program, I use the work shift feature instead. I end the program with,
G00 X3.0 Z1.0 M08 (arbitrary clearance point)
T0000 or T0600 (whatever tool was used)
G28 U0 W0
M30

Thanks again,
Dave

[cacrawfo]

Dave,
My 6T control does not have the capability to change how the wear offsets are called in, but your control may. I do not have geometry or work offsets, so I have to set the G50 at each tool change. I am getting used to it, many times I use the same tools, so after I measure with my first tool, I can subtract the difference and offset the Z of the other tools the same amount.

Cheers!
CarlC

[Dave1]

Can't thank everyone enough for the info on the Fanuc's. I've been trying some of them the last couple weeks and all is well. Also, I've been finding out some more info on the Fanuc since then. I will share
From what I've been able to find out, When using the G50 work coordinate style system you use the wear offsets. When using the built in work shift or G54-59 system you use geometry offsets. From what I've seen or understand they were not meant to be used together (geometry and wear offsets) My manual does a poor job of explaining this but it's all good.
Also found out how to make the control count when using a bar puller. The code is as follows,
M98P0208000 This will call program 8000 and repeat it 20 times
My machine manual and even the 75 dollar Fanuc manual fails to point this out, but in Fanucs defense, I haven't read all 8 bazillion pages yet so it may actually be in there somewhere.

Just a bit of info I've run into,,,,,, hope someone else can use it.
Dave

[cacrawfo]

Dave,
I believe I spoke too soon, I did not know that your control has geometry offsets... So your control has a page with Geometry and Wear offsets, and also a work coordinate shift? In that case, you will not need G50's at all!


With this type of offseting, changes between jobs are a breeze! When you call a tool, such as T0202, you are calling the tool change with the first 2 numbers, and the offsets with the second 2. So, T0202 would index the turret, and call both the 02 geometry and wear offset. You could also call T0212, which would index tool 2, but call offset 12.....more on this later.

The work shift is a Z-shift that will allow you to move your Z-zero point without having to re-touch all your tools. It is usually used like this: pick a "main" tool, usually a CNMG turn and face tool that you use for a lot of jobs. Set its geometry Z offset to zero. Touch it off and set your X geometry offset, and take a cut to establich your z zero. Now set your work shift to zero as well. You can now touch off all your remaining tools to the part, and enter the coresponding geometry offset values. Now if you run another part with a different amount hanging out of the chuck, all you have to do is touch your main CNMG tool and set the work shift to that Z value. All your other tools will be offset that amount. So if you think about it, all your geometry offset values will be the tools distance from your main CNMG tool.

You usually have more offsets than you do spaces in the turret, and you can call any offset with any tool. There are times you may want to use more than one offset with one tool. I suggest using the turret number for the main offset, and 10+ for the additional offset. For example, T0404, and T0414. I use this when I use my cutoff tool to do light facing. I find that it is hard to control the length of the part, as the cutoff tool will deflect differently on the front and rear of the part. Instead of modifying the whole program, I use one offset for the face of the part, and a slightly different offset for the back of the part. That way I can modify the wear offset a little for the back to make the length correct. Some people do the same thing for precise grooving, so that they can easily control the width of the groove from outside the program.

Hope this helps!
Carl C

[Dave1]

Carl,
Yup, you nailed it, that's exactly the way I've been doing it. The only time I ran into problems was when I used wear with the geometry offsets. But, I tried it the way you suggested and it worked fine, it eliminated the "jump" so to speak. One thing nice about the control when using geometry offsets is if you change them incrementally the control will add or subtract for you, which is a nice feature. I.E if you want to change the diameter by .001 I type in U.001 and it will update. Not all controls will do this. the Takisawa only has 19 geometry offsets for a 12 station turret though, there probably is a parameter that opens this up but for now it's not needed.
My other lathe (EMCO MAIER) uses G54-G59 offsets and I program the Z offset the same way. I.E. Picking a main tool. This lathe has 99 tool offsets. I've used 15 so far.
When I got the lathe I was a little leary about programming the Fanuc, never did that before but once I started doing it it was easy, after all, they are all basically the same, it's just setting up that is different at times.
I also like the measure function on the lathe, makes setting up a breeze. First tool, take a test cut and type MZ 0, first tool is established, second tool I use a sticky note and touch off and type MZ.003 and so on. To set X I take a cut, measure and type in the diameter,,,, MX .995 and it's good to go, they sure made that easy and fast,,,, I love it!!
Dave