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
