What's new
What's new

Setting work zero & tool offsets on lathe

brentanthony

Plastic
Joined
Jul 31, 2012
Location
youngstown, ohio
Hi, i have a mori seiki sl-3 lathe with the universal control (1979) i have always run cnc mills (vmc & hmc) but never a lathe. I do not understand where to set my work zero, is it 0,0 off the center front face of the chuck, or the 0,0 off the center end of the piece that im holding in the chuck? If its from the 0,0 off the center front face of the chuck do i ever have to change it?

Tool offsets: I have 8 tools on the turret. Do i set them off the skin face of the part or off my work zero position? Im very confused with this. From what i read before, you set one tool, and then set the others based off that first tool ?

ultimatly i have to turn very close tolorances within .002-.005

Any wise help would be greatful. Thank you all for your previous responses. This is my go to place when i dont understand something in the shop.

-brent
 

wheelieking71

Diamond
Joined
Jan 2, 2013
Location
Gilbert, AZ
where is your programmed origin? normally that would be zero. but, there are several ways to accomplish the same thing as you have already pointed out.
 

pmtool

Cast Iron
Joined
Jul 10, 2011
Location
Portland, OR
Well typically you can choose any location to touch everything off to and then input a work shift to move the zero to the front of your part. X is always the centerline. I have a 2 inch touch off light so I would touch all tools off to 2 inches off the spindle nose or some other constant on the machine.



Normally you touch of a tool and take a test cut and then make an adjustment to your offsets. Your touch off will rarely be perfect.

I have never used your very old style control, but this is how I would do it on Fanuc lathes.
 

brentanthony

Plastic
Joined
Jul 31, 2012
Location
youngstown, ohio
where is your programmed origin? normally that would be zero. but, there are several ways to accomplish the same thing as you have already pointed out.

thats what i dont know, where should i make the program zero? what is the normal way to go about a simple lathe program, say were turning a 4" od piece X 8", i hold 2" in the chuck and plan to part it off at 5" long.
 

Garwood

Diamond
Joined
Oct 10, 2009
Location
Oregon
Does your 1979 control have work offsets?

My old 5T controlled lathe uses G50 lines to set program zero for every tool. The work offsets are in the program.

I use the part origin for the program zero in the machine. I'll touch off on the chuck or jaws and move away the proper amount then zero the tool and send it home.
 

wheelieking71

Diamond
Joined
Jan 2, 2013
Location
Gilbert, AZ
thats what i dont know, where should i make the program zero? what is the normal way to go about a simple lathe program, say were turning a 4" od piece X 8", i hold 2" in the chuck and plan to part it off at 5" long.

OHH, that is a totally different question all together. "zero" can be wherever you want it. typically it is the outermost finished face of the part. (farthest from chuck) what you need to do is pick a technique, and stick with it. like pmtool mentioned, X is always center of spindle rotation. if i were training you, Z "0" would be the outermost finished face. all tools would be touched there. and all work shift offsets would be 0.0! I would make sure you had a good grasp on that, before getting you started on "work shifts". but, since it sounds like you do have prior CNC experience, I feel you are "over thinking" the whole deal. take a step back, and realize that it is very simple. Z"0" = finished face, X "0" = center of rotation.
 

Heinz R. Putz

Stainless
Joined
Mar 16, 2006
Location
Columbus, Ohio
A 79 Mori is set up with the G50 line as the first block in the program.
N1 G50 X10.0 Z12.0 S2500 means the the tip of the tool sits at these dimensions and the max RPM is 2500.
Its a little tough to explain in detail with words, its pretty easy if you are in front of the machine.
Do you have a front or rear turret?
Early Mori lathes were set up with minus values for rear turrets, so it could be G50 X-10.0 and all X dimensions are minus.
I have all this on my lathe setup DVD if you really get stuck. Look them over on doccnc.com
I am in Columbus, if you need to talk. 614-888-8466
Heinz.
 

angelw

Diamond
Joined
Sep 10, 2010
Location
Victoria Australia
thats what i dont know, where should i make the program zero? what is the normal way to go about a simple lathe program, say were turning a 4" od piece X 8", i hold 2" in the chuck and plan to part it off at 5" long.

Hi Brent,
Being a 1979 vintage and a Mori the control will be either a Fanuc 6TA of a Meldas control; but most likely the Fanuc control. Its always useful to state this information when asking questions relating to operation procedures.

As has been stated by others in this Thread, the Coordinate System is established by using the G50 Address. When using G50, its very important to always execute this command with the machine slides at a particular physical location. Via G50 the control is told how far the tool is from the X and Z Zero of the Workpiece.

Determining where the X Zero of the Workpiece will be is simple. Logically it will be the cerntre of the work, which corresponds to the centre line of the machine. Accordingly, if a G50 of a tool has already been established and the tool remains in the machine, then it will have the same X G50 for all work machined. The Z G50 can be anywhere along the workpiece, but for convenience is normally set at either end of the workpiece. Okuma controls of that time didn't require a decimal point included in the program for Integer values, that is, 60mm could be written as 60 and the control would interpret the input as 60mm. Later model Fanuc controls could be set to what Fanuc refer to as Pocket Calculator Mode via parameter so that a decimal point is not required for Integer values in the program, but by default this is not the case and this mode was not available with the Series 6T control. Being aware of this is quite important when considering where the Z zero should be set as will become more clear from the following.

When positioning the tool ready for the machining operation, its always a good idea to go to an X coordinate slightly larger than the blank Workpiece and clear by a margin in the Z axis. So lets say that the Workpiece Diameter is 100.0mm and the Tail Stock end of the work is used as Z Zero. In this case you might have an approach block as follows:

G00 X102.000 Z10.000 T0101 M08

The above block will position the tool outside the diameter of the work and clear of the work in Z by 10.0mm less whatever material is left on the workpiece in Z to allow clean up. I use a Z coordinate like Z5.0 or Z10.0 because during program prove-out, 5 or 10mm is more recognizable from 1.0mm than say 2.0 if the following block is used

G00 X102.000 Z1.000 T0101 M08

If the decimal point had been accidentally omitted from Z coordinate as shown in the following block:

G00 X102.000 Z10 T0101 M08

then the Fanuc 6T control would interpret the coordinate as Z0.010mm (0.00039"). When this block is executed, the tool would position outside the Workpiece Diameter and at Z0.010. Although in the wrong Z position, a prang has been avoided as the tool is outside the Workpiece Diameter. If the Chuck End of the Workpiece was used as the Z Zero, and the length of the Work from Z Zero is 100.0mm then the approach block to give the same standoff as G00 X102.000 Z10.000 T0101 M08, would be as follows:

G00 X102.000 Z110.000 T0101 M08

If the decimal point was omitted in the Z coordinate then Z110 would be interpreted as Z0.110. When using the Chuck End of the Workpiece as Z Zero, Z Zero will be past the front surface of whatever is holding the Workpiece; chuck jaws etc. Accordingly, notwithstanding that the example approach block puts the tool outside the Workpiece Diameter, the approach position in Z if the decimal is omitted, will be past the front surface of the work holding device, and a crash will ensue. Obviously this error would probably be picked up when doing an initial program prove-out, and the crash avoided. This type of crash normally results when a decimal point is omitted during a manual edit at the control on a well proven program.

As far as setting the Coordinate System for each tool using G50, the following may prove helpful.

1. As mentioned earlier, the G50 must be executed from the same, known, slide position in X and Z. The easiest position to find at any time is the Reference Return position for each slide, or an incremental distance away from the Reference Return position. Therefore, the following safety block should be included for each tool if the Reference Return position is used.

G28 U0.0 W0.0
G50 X??.??? Z??.???

With most chucking lathes, using the Reference Return in both X and Z as shown in the above example is acceptable; there is no huge travel in either X or Z for the slides to make to get the tool close to the Workpiece. In relatively long machine having a Tail Stock, you could use the following:

/G28 U0.0 W0.0
/G00 U-100.000 W-500.000
G50 X??.??? Z??.???

Using the above format, block delete is turned off when initially running the machine, and when having to repeat the operation of a particular tool if the program is stopped mid operation, when therefore, the position of the tool is lost. Once the program is up and running, the Block Delete switch is turned on so as to avoid the Reference Return and Incremental Shift move. Each and every tool would have the above included in it's code as shown following:

(1ST TOOL)
N1 G00 G21 G40 G99
/G28 U0.0 W0.0
/G00 U-100.000 W-500.000
G50 X200.000 Z100.000
G50 T0100 S3000
G96 S250 M03
G00 X102.000 Z10.000 M08
---------
---------
---------
G00 X200.000 Z100.000 T0100 M09
M01
(2ND TOOL)
/N2 G28 U0.0 W0.0
/G00 U-100.000 W-500.000
G50 X220.000 Z80.000
G50 T0200 S3000
G96 S250 M03
G00 X50.000 Z10.000 T0202 M08
---------
---------
---------
G00 X220.000 Z80.000 T0200 M09
M01
(3RD TOOL)
/N3 G28 U0.0 W0.0
/G00 U-100.000 W-500.000
G50 X180.000 Z90.000
G50 T0300 S3000
G96 S250 M03
G00 X40.000 Z10.000 T0303 M08
---------
---------
---------
G00 X180.000 Z90.000 T0300 M09
M30
%

Using the format above, if at any time the position of the tool is lost, stopping the program due to a broken insert for example, its a simple exercise of:
i. Press Reset in Edit Mode.

ii. Position the Cursor at the Sequence Number of the focus tool.

iii. Turn Block Delete Off

iv. Select Auto Mode and Press Cycle Start.

V. Once the G28 and the Incremental Shift Blocks have been executed, Block Delete is turned back on. If the operator omits to turn the Block Delete back on, no harm will be done, as the control will just execute a Reference Return and Incremental Shift for subsequent tools.

Some machines were equipped with a second Reference Return, G30. In this case, the Incremental Shift could be omitted and included in the parameter for the G30 position. In this case the program would be as follows, with no Block Delete required:

(1ST TOOL)
N1 G00 G21 G40 G99
G30 U0.0 W0.0
G50 X200.000 Z100.000
G50 T0100 S3000
G96 S250 M03
G00 X102.000 Z10.000 M08
---------
---------
---------
G00 X200.000 Z100.000 T0100 M09
M01
(2ND TOOL)
N2 G30 U0.0 W0.0
G50 X220.000 Z80.000
G50 T0200 S3000
G96 S250 M03
G00 X50.000 Z10.000 T0202 M08
---------
---------
---------
G00 X220.000 Z80.000 T0200 M09
M01
etc.

2. To determine the G50 for each tool, one method is as follows:
i. Perform a Reference Return for both the X and Z slide.
On very early Mori Seiki with 2000C controls, Reference Return for X and Z were two dial indicator attached to the machine as part of its assembly. Reference Return was executed by positioning the slides manually using these dial indicators.

ii. Set the Relative Position display to X0.0 Z0.0

iii. To get the X G50, with a piece of material mounted in the machine, start the spindle and take a light cleanup cut with the tool being set.

iv. Clear the tool of the material in the Z axis without moving the tool in X and stop the spindle.

v. Measure the diameter just machined and add it to the X value of the Relative X display. If the X Reference Return position is in a Positive direction from the Workpiece and as the Relative X display was set to Zero at Reference Return, the value displayed for X after taking the clean up cut will be a Negative value. When adding the measured diameter of the cut diameter, ignore the minus sign of the position display. For example, if the measured diameter was 50.051mm and the Position Display was X-150.987, then the calculation would be:

150.987 + 50.051 = 210.038

201.038 is the diameter the tool is at when at the reference return position and is the X G50 for that tool if executed at that location. Note this value down for use in the program.

vi. Start the spindle and take a clean up cut on the end of the Workpiece.

vii. Clear the tool of the Workpiece in the X axis without moving the tool in Z.

viii. Stop the spindle and determine by measurement the amount of material between the machined surface and where Z Zero on the Workpiece is.

ix. Again ignore the minus sign of the Relative Display and add the value found in viii to it. For example, if 0.54mm remained on the end of the
Workpiece, and the Relative Z display was Z-200.945 then the calculation would be:

200.945 + 0.54 = 201.485

The position of the tool when at Z Reference Return will be Z 201.485, and therefore, the Z G50 for the focus tool will be Z201.485. Note this value for use in the program.

3. Repeat the steps of point 2 above for all other tool that have to be set.

4. Particularly if Metric Mode is being used, I use the integer component of the X Z G50 found in step 2 above and apply the decimal component to the Offset for that tool.

Regards,

Bill
 
Last edited:

PROBE

Hot Rolled
Joined
Jan 23, 2003
Location
Tel Aviv, Israel
Hi Brent,
Being a 1979 vintage and a Mori the control will be either a Fanuc 6TA of a Meldas control; but most likely the Fanuc control. Its always useful to state this information when asking questions relating to operation procedures.

As has been stated by others in this Thread, the Coordinate System is established by using the G50 Address. When using G50, its very important to always execute this command with the machine slides at a particular physical location. Via G50 the control is told how far the tool is from the X and Z Zero of the Workpiece.

Determining where the X Zero of the Workpiece will be is simple. Logically it will be the cerntre of the work, which corresponds to the centre line of the machine. Accordingly, if a G50 of a tool has already been established and the tool remains in the machine, then it will have the same X G50 for all work machined. The Z G50 can be anywhere along the workpiece, but for convenience is normally set at either end of the workpiece. Okuma controls of that time didn't require a decimal point included in the program for Integer values, that is, 60mm could be written as 60 and the control would interpret the input as 60mm. Later model Fanuc controls could be set to what Fanuc refer to as Pocket Calculator Mode via parameter so that a decimal point is not required for Integer values in the program, but by default this is not the case and this mode was not available with the Series 6T control. Being aware of this is quite important when considering where the Z zero should be set as will become more clear from the following.

When positioning the tool ready for the machining operation, its always a good idea to go to an X coordinate slightly larger than the blank Workpiece and clear by a margin in the Z axis. So lets say that the Workpiece Diameter is 100.0mm and the Tail Stock end of the work is used as Z Zero. In this case you might have an approach block as follows:

G00 X102.000 Z10.000 T0101 M08

The above block will position the tool outside the diameter of the work and clear of the work in Z by 10.0mm less whatever material is left on the workpiece in Z to allow clean up. I use a Z coordinate like Z5.0 or Z10.0 because during program prove-out, 5 or 10mm is more recognizable from 1.0mm than say 2.0 if the following block is used

G00 X102.000 Z1.000 T0101 M08

If the decimal point had been accidentally omitted from Z coordinate as shown in the following block:

G00 X102.000 Z10 T0101 M08

then the Fanuc 6T control would interpret the coordinate as Z0.010mm (0.00039"). When this block is executed, the tool would position outside the Workpiece Diameter and at Z0.010. Although in the wrong Z position, a prang has been avoided as the tool is outside the Workpiece Diameter. If the Chuck End of the Workpiece was used as the Z Zero, and the length of the Work from Z Zero is 100.0mm then the approach block to give the same standoff as G00 X102.000 Z10.000 T0101 M08, would be as follows:

G00 X102.000 Z110.000 T0101 M08

If the decimal point was omitted in the Z coordinate then Z110 would be interpreted as Z0.110. When using the Chuck End of the Workpiece as Z Zero, Z Zero will be past the front surface of whatever is holding the Workpiece; chuck jaws etc. According, notwithstanding that the example approach block puts the tool outside the Workpiece Diameter, the approach position in Z if the decimal is omitted, will be past the front surface of the work holding device, and a crash will ensue. Obviously this error would probably be picked up when doing an initial program prove-out, and the crash avoided. This type of crash normally results when a decimal point is omitted during a manual edit at the control on a well proven program.

As far as setting the Coordinate System for each tool using G50, the following may prove helpful.

1. As mentioned earlier, the G50 must be executed from the same, known, slide position in X and Z. The easiest position to find at any time is the Reference Return position for each slide, or an incremental distance away from the Reference Return position. Therefore, the following safety block should be included for each tool if the Reference Return position is used.

G28 U0.0 W0.0
G50 X??.??? Z??.???

With most chucking lathes, using the Reference Return in both X and Z as shown in the above example is acceptable; there is no huge travel in either X or Z for the slides to make to get the tool close to the Workpiece. In relatively long machine having a Tail Stock, you could use the following:

/G28 U0.0 W0.0
/G00 U-100.000 W-500.000
G50 X??.??? Z??.???

Using the above format, block delete is turned off when initially running the machine, and when having to repeat the operation of a particular tool if the program is stopped mid operation, when therefore, the position of the tool is lost. Once the program is up and running, the Block Delete switch is turned on so as to avoid the Reference Return and Incremental Shift move. Each and every tool would have the above included in it's code as shown following:

(1ST TOOL)
N1 G00 G21 G40 G99
/G28 U0.0 W0.0
/G00 U-100.000 W-500.000
G50 X200.000 Z100.000
G50 T0100 S3000
G96 S250 M03
G00 X102.000 Z10.000 M08
---------
---------
---------
G00 X200.000 Z100.000 T0100 M09
M01
(2ND TOOL)
/N2 G28 U0.0 W0.0
/G00 U-100.000 W-500.000
G50 X220.000 Z80.000
G50 T0200 S3000
G96 S250 M03
G00 X50.000 Z10.000 T0202 M08
---------
---------
---------
G00 X220.000 Z80.000 T0200 M09
M01
(3RD TOOL)
/N3 G28 U0.0 W0.0
/G00 U-100.000 W-500.000
G50 X180.000 Z90.000
G50 T0300 S3000
G96 S250 M03
G00 X40.000 Z10.000 T0303 M08
---------
---------
---------
G00 X180.000 Z90.000 T0300 M09
M30
%

Using the format above, if at any time the position of the tool is lost, stopping the program due to a broken insert for example, its a simple exercise of:
i. Press Reset in Edit Mode.

ii. Position the Cursor at the Sequence Number of the focus tool.

iii. Turn Block Delete Off

iv. Select Auto Mode and Press Cycle Start.

V. Once the G28 and the Incremental Shift Blocks have been executed, Block Delete is turned back on. If the operator omits to turn the Block Delete back on, no harm will be done, as the control will just execute a Reference Return and Incremental Shift for subsequent tools.

Some machines were equipped with a second Reference Return, G30. In this case, the Incremental Shift could be omitted and included in the parameter for the G30 position. In this case the program would be as follows, with no Block Delete required:

(1ST TOOL)
N1 G00 G21 G40 G99
G30 U0.0 W0.0
G50 X200.000 Z100.000
G50 T0100 S3000
G96 S250 M03
G00 X102.000 Z10.000 M08
---------
---------
---------
G00 X200.000 Z100.000 T0100 M09
M01
(2ND TOOL)
N2 G30 U0.0 W0.0
G50 X220.000 Z80.000
G50 T0200 S3000
G96 S250 M03
G00 X50.000 Z10.000 T0202 M08
---------
---------
---------
G00 X220.000 Z80.000 T0200 M09
M01
etc.

2. To determine the G50 for each tool, one method is as follows:
i. Perform a Reference Return for both the X and Z slide.
On very early Mori Seiki with 2000C controls, Reference Return for X and Z were two dial indicator attache to the machine as part of their assembly. Reference Return was executed by positioning the slides manually using these dial indicators.

ii. Set the Relative Position display to X0.0 Z0.0

iii. To get the X G50, with a piece of material mounted in the machine, start the spindle and take a light cleanup cut with the tool being set.

iv. Clear the tool of the material in the Z axis without moving the tool in X and stop the spindle.

v. Measure the diameter just machined and add it to the X value of the Relative X display. If the X Reference Return position is in a Positive direction from the Workpiece and as the Relative X display was set to Zero at Reference Return, the value displayed for X after taking the clean up cut will be a Negative value. When adding the measured diameter of the cut diameter, ignore the minus sign of the position display. For example, if the measured diameter was 50.051mm and the Position Display was X-150.987, then the calculation would be:

150.987 + 50.051 = 210.038

201.038 is the diameter the tool is at when at the reference return position and is the X G50 for that tool if executed at that location. Note this value down for use in the program.

vi. Start the spindle and take a clean up cut on the end of the Workpiece.

vii. Clear the tool of the Workpiece in the X axis without moving the tool in Z.

viii. Stop the spindle and determine by measurement the amount of material between the machined surface and where Z Zero on the Workpiece is.

ix. Again ignore the minus sign of the Relative Display and add the value found in viii to it. For example, if 0.54mm remained on the end of the
Workpiece, and the Relative Z display was Z-200.945 then the calculation would be:

200.945 + 0.54 = 201.485

The position of the tool when at Z Reference Return will be Z 201.485, and therefore, the Z G50 for the focus tool will be Z201.485. Note this value for use in the program.

3. Repeat the steps of point 2 above for all other tool that have to be set.

4. Particularly if Metric Mode is being used, I use the integer component of the X Z G50 found in step 2 above and apply the decimal component to the Offset for that tool.

Regards,

Bill


Bill,
Briliant explanation, as usual. Hip hip.
 

brentanthony

Plastic
Joined
Jul 31, 2012
Location
youngstown, ohio
Hi Brent,


Regards,

Bill

Bill, Thank you! You are an absolute BEAST FOUNTAIN OF INFORMATION!!!!! the control is actually a yasnac 2000g (universal interface) im going to implement everything you have mentioned to get her going ! now with a better grasp on things, GARWOOD pointed out that there are no work offsets for this vintage model. Turns out hes right. it must all be programed from the g50 command... there is an existing program stored in the nc memory along with tool offsets (havnt changed anything since i got the machine) which is as followed :

G50 X-6.0154 Z6.0000 S1300. M08
T101 M41
G96 S700 M03
G00 X-4.3 Z0.0
G01 X.5 F.8
G00 X-3.972 W.5
G01 Z-.7 F.110
G00 Z.5 U-.5
G00 X-3.769 Z.5
G01 Z-.125 F.110
G00 Z.5 U-.5
-------
------
-----

so the first line of that code is the work offset through g50? oddly enough the tool offsets are T101: X .8 Z0.0

btw what is the T101 M41 command?
 

angelw

Diamond
Joined
Sep 10, 2010
Location
Victoria Australia
Bill, Thank you! You are an absolute BEAST FOUNTAIN OF INFORMATION!!!!! the control is actually a yasnac 2000g (universal interface) im going to implement everything you have mentioned to get her going ! now with a better grasp on things, GARWOOD pointed out that there are no work offsets for this vintage model. Turns out hes right. it must all be programed from the g50 command... there is an existing program stored in the nc memory along with tool offsets (havnt changed anything since i got the machine) which is as followed :

G50 X-6.0154 Z6.0000 S1300. M08
T101 M41
G96 S700 M03
G00 X-4.3 Z0.0
G01 X.5 F.8
G00 X-3.972 W.5
G01 Z-.7 F.110
G00 Z.5 U-.5
G00 X-3.769 Z.5
G01 Z-.125 F.110
G00 Z.5 U-.5
-------
------
-----

so the first line of that code is the work offset through g50? oddly enough the tool offsets are T101: X .8 Z0.0

btw what is the T101 M41 command?

Hi Brent,
The Yasnac and Fanuc controls are/were extremely similar; many say the Yasnac was a re-badged Fanuc but there were/are many subtle differences.

With the corresponding Fanuc Series 6T control, if you were to call the new tool and its offset combined, as in your example listing, there would be movement of both the X and Z slide equal to the stored Tool Offset for each while the index was in progress; the Yasnac control will be the same. This is only a small point I suppose, particularly if the offsets are kept to very small values by using a fairly accurate G50. However, you indicate the use of a 0.8" offset in your last Post which is a significant amount of movement. You may note in the examples I listed in my previous Post that I've shown the Tool being called without a Tool Offset and then the Offset applied during the approach move. In my opinion, this is the better method as the Offset move is assimilated in the move and is unseen.

The Fanuc controls used to get hung up when the following conditions applied:
1. Tool and Tool Offset were called together, but without a move command.
2. G01 mode was current.
3. The spindle was stopped and the control was in Feed Per Revolution Mode.

I've not experimented with the Yasnac control to see if the same occurred, but because of the two control's similarities I suspect that the same would apply.

Another point that's quite important, is to make sure that the Tool Offset is cancelled when the slides are returned to the Tool Change Position. If this is not done, and a Reference Return command is not included before the execution of the G50 Coordinate System Set, then there would be a gradual shift of the G50 position equal to the accumulation of the uncancelled Offsets. In your example, there is no Reference Return in the program before the G50 is executed. Accordingly, if the return to the Tool Change position was made by the following block

G00 X-6.0154 Z6.0000 M09

then a shift in the G50 for the next tool called would occur. To avoid this, the command block should be G00 X-6.0154 Z6.0000 T0100 M09 when returning the slides to the Tool Change position.

btw what is the T101 M41 command
The T101 is a combination call of the Tool and its Offset. The M41 is to call a Gear Range.

Regards,

Bill
 

Nick Mueller

Titanium
Joined
Jun 12, 2006
Location
Munich / Germany
That offset and work zero stuff initially is a bit confusing.
And, there are a few ways to do it. Without going into too much detail:
Tool offsets can be in two ways:
* Either relative to one distinct tool (tool #1)
* or relative to some point in the lathe. I'm using the second method, because I do have a tool setter in my lathe. No matter which way, as soon as you switch between tools, the control can (and does) calculate the distance between the previous tool's tip and the current tool by subtracting the offsets in X and Z. After that, the control will make a compensating move (at least if you order to go to the same place the previous tool was in).

Until now, that was not good enough for turning any parts (unless you want to make some confusing math that certainly will end with a tool stuck in the chuck).
What you have next, is the work offset. In most cases G54. Now this offset also has an offset value of X and Z, like the tool's offset. The control adds both offsets for G54 and for the tool and that both in X and Z to get the final commanded position.
Now it is getting to make sense! The offset in X for G54 is always a value that sets the tool to the centerline. The important point to understand is, that the X-value for G54 is always the same. Differences in tool length are compensated by the tool offset.
So whatever you do, the X-value for G54 will never be touched. Consider it as a machine constant. Well, there are cases, but ...
On the other hand, the Z-offset for G54 is the one that is constantly changed with every setup. Normally, the Z-zero is the face of the part, facing the tailstock. All work thus has negative Z-values (except while facing, boring, drilling, tapping etc.).
If you chuck some work, the first thing normally is to set the G54 Z-value to the face by touching it with a tool. That tool # has to be known -and properly offset- to the control, or it will calculate a wrong Z-offset when you actually start cutting.

Hope that cleared some of your confusion. You'll learn the details later while using the basics.


Nick
 

angelw

Diamond
Joined
Sep 10, 2010
Location
Victoria Australia
That offset and work zero stuff initially is a bit confusing.
And, there are a few ways to do it. Without going into too much detail:
Tool offsets can be in two ways:
* Either relative to one distinct tool (tool #1)
* or relative to some point in the lathe. I'm using the second method, because I do have a tool setter in my lathe. No matter which way, as soon as you switch between tools, the control can (and does) calculate the distance between the previous tool's tip and the current tool by subtracting the offsets in X and Z. After that, the control will make a compensating move (at least if you order to go to the same place the previous tool was in).

Until now, that was not good enough for turning any parts (unless you want to make some confusing math that certainly will end with a tool stuck in the chuck).
What you have next, is the work offset. In most cases G54. Now this offset also has an offset value of X and Z, like the tool's offset. The control adds both offsets for G54 and for the tool and that both in X and Z to get the final commanded position.
Now it is getting to make sense! The offset in X for G54 is always a value that sets the tool to the centerline. The important point to understand is, that the X-value for G54 is always the same. Differences in tool length are compensated by the tool offset.
So whatever you do, the X-value for G54 will never be touched. Consider it as a machine constant. Well, there are cases, but ...
On the other hand, the Z-offset for G54 is the one that is constantly changed with every setup. Normally, the Z-zero is the face of the part, facing the tailstock. All work thus has negative Z-values (except while facing, boring, drilling, tapping etc.).
If you chuck some work, the first thing normally is to set the G54 Z-value to the face by touching it with a tool. That tool # has to be known -and properly offset- to the control, or it will calculate a wrong Z-offset when you actually start cutting.

Hope that cleared some of your confusion. You'll learn the details later while using the basics.


Nick

Hi Nick,
You're absolutely correct when the control being considered has Work Shift and Geometry Offset programming available, but with the control the OP is inquiring about, this is not the case. Some try and program such controls the same way that a machine with Geometry and Work Shift would be, by applying large offsets (the geometry of the tool) in what was designed to be a Tool Wear Offset. This would work to some extent on some machines, because on the majority of machines with these old controls that used G50 and G92 to set the Coordinate System, the maximum allowable offsets was quite small, as the Tool Offset was designed as a Tool Wear Offset only.

Gang tooling configured machines tended to allow large Tool Offsets to be set, and these machines where frequently programmed with one G50 execution at the beginning of the program to accommodate the shift in the Z Zero from workpiece to workpiece if the tail stock end of the work was used as Z Zero. However, there is no getting around the fact that the slides have to be at an exact, particular position when this G50 Coordinate Set command was executed. With a control that uses Work Shift Offsets, the slides could be at any safe slide location to start from, and the control knows the program position of the tool via its internal calculation based on the Work Shift and Tool Geometry Offsets.

Regards,

Bill
 
Last edited:

Garwood

Diamond
Joined
Oct 10, 2009
Location
Oregon
That offset and work zero stuff initially is a bit confusing.
And, there are a few ways to do it. Without going into too much detail:
Tool offsets can be in two ways:
* Either relative to one distinct tool (tool #1)
* or relative to some point in the lathe. I'm using the second method, because I do have a tool setter in my lathe. No matter which way, as soon as you switch between tools, the control can (and does) calculate the distance between the previous tool's tip and the current tool by subtracting the offsets in X and Z. After that, the control will make a compensating move (at least if you order to go to the same place the previous tool was in).

Until now, that was not good enough for turning any parts (unless you want to make some confusing math that certainly will end with a tool stuck in the chuck).
What you have next, is the work offset. In most cases G54. Now this offset also has an offset value of X and Z, like the tool's offset. The control adds both offsets for G54 and for the tool and that both in X and Z to get the final commanded position.
Now it is getting to make sense! The offset in X for G54 is always a value that sets the tool to the centerline. The important point to understand is, that the X-value for G54 is always the same. Differences in tool length are compensated by the tool offset.
So whatever you do, the X-value for G54 will never be touched. Consider it as a machine constant. Well, there are cases, but ...
On the other hand, the Z-offset for G54 is the one that is constantly changed with every setup. Normally, the Z-zero is the face of the part, facing the tailstock. All work thus has negative Z-values (except while facing, boring, drilling, tapping etc.).
If you chuck some work, the first thing normally is to set the G54 Z-value to the face by touching it with a tool. That tool # has to be known -and properly offset- to the control, or it will calculate a wrong Z-offset when you actually start cutting.

Hope that cleared some of your confusion. You'll learn the details later while using the basics.


Nick

Nick, It's been pointed out that his control does not have work offsets. G54 does not exist in his machine.
 

Nick Mueller

Titanium
Joined
Jun 12, 2006
Location
Munich / Germany
G54 does not exist in his machine.

I should have read the thread post by post. :leaving:
I just saw that the explanations kept coming and I thought that what the OP is missing is a bigger picture of all.

Sorry, I'll shut up. Have no clue what to do without G54.
Nick
 

ramires

Plastic
Joined
Mar 17, 2014
Location
California
Hi
Can some one help to explain the difference using G54 and using work shift? I am using vertical Lathe with Fanuc O-T I also want to mention I am new on this forum and new at this trade.

I love how much information is here.
Javier
 

Yingxi

Plastic
Joined
Aug 14, 2016
Hi Nick,
You're absolutely correct when the control being considered has Work Shift and Geometry Offset programming available

Bill

Hello, Bill.
I really want to know how to use both work shift and geometry offset on fanuc 0i-TD lathe. I understand Nick's method, but I don't know how to operate in details. For example, how can I obtain these G54 work offset values?

Your help is greatly appreciated. Thank you very much.

Yingxi
 








 
Top