-How do I set g50?
-What does g50 "tell" the machine?
-How does this work with a turret full of tools?
-If someone is experienced with this controller, I'd be very grateful for a setup walk through.
Thanks
Hello Erik,
Answering your second question first, the G50 command sets the coordinate system for each tool and specifically tells the control the distance of the tool from the position the G50 Block is executed to the X/Z Zero of the Workpiece.
The G50 Coordinate Setting system was originally designed to specify the position of the Tool where the G50 is executed, relative to the X/Z Zero of the Work and the Tool Offsets to adjust for Tool Wear. Some use the Tool Offset as a Geometry Offset (not how the system was designed); however, being able to use the Offsets in this way is machine specific as the the max size able to be registered is often limited. Following is a method for setting the Coordinate System via G50 in the manner it was designed.
Its important that the G50 command be executed from the same axis position. As the Reference Return position of each axis is the only, easily repeated position, its common for the G50 Coordinate System to be set at the Reference Return Position
To set the G50 for a particular tool, proceed as follows:
1. Reference Return each axis.
2. Display the RELATIVE POSITION page on the screen of the control
3. Set the X and Z display to Zero
4. To obtain the X G50 value:
i. Place a blank workpiece in the chuck and start the spindle in manual mode.
ii. Move the tool to be set, close to the workpiece by jog, controlled rapid, or handwheel
iii. With the tool clear of the workpiece in Z, select Handwheel Mode and move the tool in X to a diameter that will result in the workpiece being cut.
iv. Move the tool in Z to cut a journal long enough to measure.
v. Without moving the tool in X, move the tool clear off the work in Z and stop the Spindle. Measure the machined journal and note the dimension.
vi. At this point both the X and Z axis Relative Display will show negative values. Disregard the negative sign and consider the values as Absolute.
vii. Add the diameter measured in point v. above to the Absolute valued of the X value shown in the Relative display. The resulting answer is the X G50 Coordinate System Value for the tool being set and represents the distance the tip of the tool is in X, when the X axis is at Reference Return, to the X Zero (centre line) of the Workpiece.
viii. Note the value calculated in vii. above to be later written into the program.
5. To obtain the Z G50 value:
i. Start the Spindle and take a light cut on the end of the Workpiece.
ii. Without moving the tool in Z, move the tool clear of the work in X and stop the Spindle. Measure the distance from the machined face in Z to where Z Zero is on the Workpiece.
iii. As with the X axis display, the Z axis display will also be a negative value. Disregard the negative sign and consider the value as Absolute.
iv. Add the value obtained in ii. above to the Absolute valued of the Z value shown in the Relative display. The resulting answer is the Z G50 Coordinate System Value for the tool being set and represents the distance the tip of the tool is in Z, when the Z axis is at Reference Return, to the Z Zero of the Workpiece.
v. Note the value calculated in iv. above to be later written into the program.
Because the X and Z axis Relative Display was set to Zero at Reference Return, there is no need to return the Axes to the Reference Return position before setting other tools. Simply move the tool turret clear of the work, index the next tool to be set into position and repeat steps 4-ii to 4-viii and 5-i to 5-v above.
The values obtained in the above steps are used in the part program for each respective tool. For example:
Lets say that the diameter measured after cutting the journal with Tool 01 is 50.05 and the Relative Display value for X was X-253.87. The value for the X G50 is calculated as follows:
T0100 G50 X = 253.87 + 50.05
T0100 G50 X = 303.92
Lets further say that after cutting the end of the Workpiece in Z, its determined that there is 0.25mm of material between the current position of the tool in Z to Z Zero on the Workpiece and the Relative Display value for Z was X-402.53. The value for the Z G50 is calculated as follows:
T0100 G50 Z = 402.53 + 0.25
T0100 G50 Z = 402.78
The above values would be added to the part program something like the following:
(80DEG 0.8TNR OD TURNING TOOL)
(ROUGH FACE AND OD TURN)
N1 G00 G18 G40 G99
G28 U0.0
G28 W0.0
G50 X303.92 Z402.78
G50 T0100 S2500
G97 S1326 M03
G00 X60.0 Z10.0 T0101 M08
G96 S250
G01 Z1.0 F1.0
----------
----------
Program Code for Tool Goes Here
----------
----------
G00 X303.92 Z402.78 T0100 M09
M01
The above format is repeated for all other tools used in the program. N1 above is a safety start block and doesn't have to be repeated for each tool.
When using a control (such as a FS6T) using G50 to set the Coordinate System, I would generally only use the integer value of the coordinates above in the G50 Block and apply the decimal component to the Tool Offset. In this case the G50 for X and Z would be as follows:
G50 X303.0 Z402.0
and the values applied to the Tool Offset would be:
X-0.92 Z-0.78
When applying the decimal component of X for an OD Tool, it will be a negative value. For an ID Tool, the value will be positive. The Z Offset value using the decimal component will be negative for a boring bar where the leading edge of the tool is used in setting the Coordinate System.
Regards,
Bill
