Need Help!- Setting tools offset on Fanuc 21i

[jdgromi]

Hello!

I don't understand how to do this. I have read the book of my lathe ROMI 17 and I can setting my first tool like rought tool, x = 0 axe and y= 0 the face of my chuck. For my treading tool and the others I am not able to setting the offset. How can I do that? What is the way to do the good setting?

Best reagrds Jean-Denis

[stevo1]

This will all depend on were your machine home is set up. If your Y0 is the face of the chuck as you had said you can touch your tool on the chuck face and subtract the reference distance(distance from machine orgin to spindle face) from machine position. Now with that offset instated if you program Y0 the tool tip should want to travel to the chuck face. You then need to just have the part height put in your work coordinate.

For the X if your home position is the center of the chuck you touch your tool off on a known diameter. Subract the machine position from the known diameter.

Stevo

[dcoupar]

If your machine is not equipped with a tool setter, you turn a diameter, then move Z away (don't move X) and stop the spindle. Measure the diameter you just turned. In the Geometry Offset page, move the cursor to the X for the tool you just set, and press X, type in the diameter, and press the MEASUR soft key. Now move Z to the face of the part, take a facing cut, decide how much stock is left on the face (i.e., 0.01), press Z, type in 0.01, and press the MEASUR soft key. Repeat for the remaining tools.

[jdgromi]

Many Thanks

Stevo1 and dcoupar.
I have done as you have written to me and the result is very good. But the thread cutter, in the first pass, is too far away from the piece, 0,030 R.
Must I correct my offset setting or my 2 lines of bloc?
N150 G76 P010060 Q00 R00 ;
N160 G76 X,505 Z1,020 P1182 Q300 F,0909 ;
Thread 5/8 - 11 NC.

Best Regards
Jean-Denis

[dcoupar]

The first pass comes from the minor diameter (X,505) + 2 * height of thread (P1182) - 2 * depth of 1st pass (Q300). I would guess your 1st pass is at X0.6814, right? I think your P should be about half of what you have in there for a 5/8-11 (the Machinery's Handbook shows 0.0492 for a 11 pitch UN thread). Also your Q may be a twice what you want, too.

[timlkallam]

G76 P010060 Q0050 R.001 ;
N160 G76 X.493 Z1.020 P0557 Q0100 F.0909

The thread height P in the second line is a radius not dia.

To find the thread height mutiply the thread lead by .61343
(.0909 x .61343= .0557

[timlkallam]

Tool seting fanuc 21

To set work shift
move the tool to to your zero point( touch off tool 1 in program)
press off set key
press right arrow soft key TWICE( the soft keys are under the screen
there are no markings on them)
on the bottom of the screen you will see (w shift) press the soft key under it you should now be in the workshift page.
Upper left hand corner of of work shift screen the is x and z
highlight the Z press 0 input ( change the number to 0)
on the bottom right of the screen there is a number z xxxxx(relative)
enter that number as a NEGATIVE number in the upper left (where you just changed it to zero )
Now that bottom right number should read zero and your workshift is set.


To set tool length offsets
index to second tool in program(example tool 2)
touch off tool
go to the geomertry screen highlight z in tool 2
push off set Measure key (this is not the same key as off set key)
press Z0
push measure (soft key under screen)

To set diameter offsets
Take a cut with the tool you want to set ,(ex tool 2 )move the tool off the work buy moving z axis.
stop spindle
measure workpiece
go to geomerty screen Highlight x tool 2
press offset measure key (this is not the same key as off set key)

type x and the diameter size (example X1.625)
press measure (soft key under screen)

[jdgromi]

Now I understand the tools setting. It's great.

My question is about cutting thread.
The result of my 5/8-11NC is:

G76 P010060 Q00 R00 ;
G76 X.495 Z1.020 P650 Q187 F.0909;

How can I find the X value?
"timlkallam", you have find x,493. How can you find it?

Romi suggest to me for finding the Q value:
P(F x ,65)/ sq(nb of pass) or P/square root(nb of pass: 12).

It seem to have many way to find the result for this bloc. Which one are given the good result in the first try?

Best regards Jean-Denis