why different offsets

hi everyone im new here,
have a question about offsets for cincinnati talon 210 850sx acramatic lathe. what is the difference between fixed and assignable offsets? which one do you use to touch tools off? tool probe doesnt seem to work so would be touching off the part. also how do you set Z0. with G92?
thanks

Hello Welcome to the board!

Fixed offsets are like what you would think of as a geometry offset. It tells the control where the tool tip is in relation to your absolute position. It sets your absolute coordinates system.

Come down with a facing tool and face off a piece stock and without moving the Z in MDI type G92 Z0 then hit the green button. This will set your absolute Z zero position and the "Z set" number. Then touch all other tools to this face and record the Z position in the respective spot in Z colum in the Fixed offsets table data.

Assignable offsets are a value you want to assign to a tool for a particular purpose. Let's say you want to program off the back side of a cutoff tool you could assign a Z- offset of the tool width witch would get you over to the back side and would get er done. Lol...

That make sense?

Brent

I believe this control also has shop floor programming integrated into it witch is the conversational side of the ccontrol. That is what the "tooling data" page is all about.

Do you have a manual?

Brent

thanks for the reply. that makes sense. just getting confused reading the manuel i guess. so for setting the X would i turn a bit of stock and type the position into the fixed offset? or is there something i need to do in MDI as well?

yes i have manuel

On a lathe, G50 "usually" is used for coordinate preset, not G92. G92 is normally used on mills for preset, but is a threading code for lathes. However, if it has work offsets (G54, G55, etc. like a Fanuc) I would recommend using that method instead.

It's been a long time since I messed with this control and if I remember correctly the book tells you how to set the fixed offsets using the touch probe and ours eventually got broken also and then I had to figure this out for myself.

I believe the X fixed offset is based off a 5" long OD turning tool. So if from the end to the tip of the inseet is exactly 5 inches the X fixed offset would be zero. I think? Lol...

Anyhow this is what I came up with on how to do this. It's hillbilly as hell but it worked for me. First of all I believe all the X fixed numbers except drills were negative.

Say tool number 1 is a turning tool. In your fixed X offset for tool number 1 type any number let's say X-1.234 then input. Now turn a diameter with tool number 1, then move the turret back to a safe spot where it can index without issue without moving any in the X axis. Now Measure and write down the diameter you just turned.

For argument sakes let's pretend the diameter you just measured is exactly 1 inch. Now in MDI type in T0101 M6 then hit the green button. Now on the position page read the absolute position. If the absolute position reads 1.502 and you know the diameter you just turned 1.000 exactly you need to move the fixed offset by a increment of .502 to get the absolute position to read exactly 1 inch.

Now hit the reset button then adjust the fixed offset the .502 then in MDI type T0101 M6 and see it the absolute position now reads X1.0000? If it is worse you moved it the wrong way then go the other direction with the fixed and try it again. Keep doing this until you call T0101 M6 and then the X absolute position reads what you measured the OD/ID at.

Do the same for boring tools. Indicate a boring bar pod/holder and do the same for drills.

Any of this making any sense?

Brent

rainman said:

On a lathe, G50 "usually" is used for coordinate preset, not G92. G92 is normally used on mills for preset, but is a threading code for lathes. However, if it has work offsets (G54, G55, etc. like a Fanuc) I would recommend using that method instead.

Click to expand...

Normally I'd agree but this is a old Cincinnati lathe with an Acramatic 850sx control. It does use G92 to set Z zero along with fixed offsets. Never run anything like this other than on a Cincinnati. Lol....

Brent

Oops I forgot! The very first thing you need to do is clear all wear offsets for the tools you'll be setting the fixed offsets for.

Brent

thanks for the help. ill give it a shot and see how it works.
thanks
cheers

tried running program and got error that it wasnt synced. tried to go into EDIT and it wont let me access the screen. can access other tabs. its like the program is locked. what am i missing?

keep getting errors for no colon

Yeah that goes at the start of each tool in your program. It kinda does let the control know it's ready to start.

I'll do some digging and find a old programs to post here tomorrow as kind of a sample for you to look at.

Maybe that'll get you going? Don't get frustrated this thing is a different animal then probably anything you've ever ran.

How much and what kind of lathe experience do you have?

You could post your entire program here for the group to see and then maybe someone could better help that way?

Brent

%
:10g0g60g62g98g70g40x5z12.
(msg, 20-011 5070 - revision 1 4/17/02)
(msg, z set 0.000)
(msg, ejector pin support)
(msg, run time = 0 min 0 sec)
(msg, 2" 4140 stock)
(msg, face)
g92s1000
g97s225t5m6m3
g95f.008
g0x2.4z.05m8
g96r2.4s225
(bar,h1c2d.04i.0001k.0001x2.3z0)
g1x2.2z0
g1x-.045f.006
(enc)
m50
m1


:20g0g60g62g98g70g40x5.z12.
(msg, #2 ctr drill)
g92s900
g97s500t2m6m4
g95f.006
g0x0z.1m8
g1z-.175f.002
g0z.5m9
m50
m5
m85
m0
m86


:30g0g60g62g98g70g40x5.z12.
(msg,rough front od)
g92s1200
g97s272t1m6m3
g95f.02
g0x6.z.1m8
g0x2.
G96r2.s350
g95f.009
(bar, h0c1d.080i.010k.003x1.02z.05)
g1x1.0200z.0000
g1x1.1200z-.0500
g1x1.1200z-2.3980
g1x1.4400z-2.3980
g3x1.5000z-2.4280p.03
g1x1.5000z-6.8280
g1x1.8200z-6.8280
g3x1.8800z-6.8580p.03
g1x1.8800z-7.4880
(enc)
g0x6.
M50
m5
m87
m84
m1


:40g0g60g62g98g70g40x5.z12.
(msg, #2 ctr drill)
g92s900
g97s500t2m6m4
g95f.006
g0x0z.1m8
g1z-.205f.002
g0z.5m9
m50
m5
m85
m0
m86


:50g0g60g62g98g70g40x5.z12.
(msg,finish od )
g92s1400
g97s400t3m6m3
g95f.0030
g0x6.z.1m8
g0x1.6z.06
g96r1.6s450
g1x.3f.01
g1g42z.0f.008
g1x1.0200z.0000
g1x1.1200z-.0500
g1x1.1200z-2.3980
g1x1.4400z-2.3980
g3x1.5000z-2.4280p.03
g1x1.5000z-6.8280
g1x1.8200z-6.8280
g3x1.8800z-6.8580p.03
g1x1.8800z-7.4880
g0g40x6.z.1m9
m50h0
m1


:60g0g62g98g70g40x5.z12.
(msg, 1 1/8 - 12 o.d. Thread)
g92s800
g97s300t7m6m4
g95f.030
g0x6.z.2
g0x1.125z.15m8
(thd,h0d.0080a0r1.3x1.025z0)
g33x1.025z-2.380k.083333
(enc)
g0x6.
M50
/m5
/m87
/m0
/m86
m1


:70g0g60g62g98g70g40x5.z12.
(msg, cut off )
g92s700
g97s120t09m6m3
g95f.004
g0x5.z1.m8
g0x2.z-7.348h1
g96r2.s200
g1x.20f.002
g0x4.m9
m50h0
m5
m87
m84
m2


:80g0g60g62g98g70g40x5.z12.
(msg, front stop)
g92s600
s200t6m6
g95f.004
g0x1.1z.015
m2
%

I have no effin clue as to why this editor automatically changed my copy and paste text into to lower case letters? But it did!

Here is a program of mine to look at as a sample. As you can see G92 with an S limits the max RPM as well as sets part Z zero.

Brent

Also next time you start a thread or ask a question about this control it may help to ask it on the CNC board. Sometimes it'll get more exposure to folks that could potentially help sort the problem out. It could be why Im the oonly one here? I stumbled across this post on the home page.

Brent