I got fadal 3016, 32 MP and TS27R renishaw probe.
Somehow i learn to measure lenght of tool, but a cant measure the diameter. I read in manual about (L9101) subroutine, but it just doesnt ring a bell.:confused:


Please help

You need to get the book from Renishaw, TS27R Tool Setting Probe, part# H-2000-5018-04-C

For software routines, you need Data Sheet H-2000-2289

If you're going to play with it, don't forget to rotate the tool in reverse....between 150-800 rpm for tools .95-5.0" dia. using a surface speed of 197sfm for 1st touch. Second touch is 800rpm at .16in/min feedrate.

Dont waste your money on buying the renishaw sw.

Read the manual on L910x, it's all in there.

Thanks for answer, but can anyone tell me how to call a suroutine on fadal for tool diameter ?
I know that i need to go to UT command and use 3d option for TS probe, but i cant call program for measurment...

Right from the book....


L9101 Probe
Functions
The L9101 fixed subroutine has 10 probe functions available:
1) LOCATE TOUCH POINT
2) CENTER LOCATION AND RADIUS
3) PART ORIENTATION
4) MID-POINT AND ANGLE
5) Z DATUM LOCATION
6) TOOL BREAKAGE DETECTION
7) TOUCH/POSITION CHECK
8) COMPUTE DIAMETER
9) SET PROBE CALIBRATION
10) SET TOUCH POINT
The code L9101 is used to call a probe function, the R word R1 selects the
specific function. For example: L9101 R1+2. Selects function #2 - CENTER LOCATION AND RADIUS.
Upon completion of the L9101, the R words R1-R3 contain the results. The R words can then be used as indirect references throughout the remainder of the program.
The touch points are retained in memory until power is removed, thus making it possible to do a mid-program start after the points have been located. As in
circular motion, the G17, G18, and G19 modes determine the output of the L9101 subroutine. G17= XY, G18= ZX, and G19= YZ.

For example, use function 2 to compute the center location of 3 points. The logical X is returned in R1. When G18 is in effect, R1 contains the physical Z center location.
----------------------------
Method 2
Use the L9101 subroutine function 1 to move and store the point. Note that the program must be written in absolute terms. When using the example use the SETX command to set the X axis home approximately one inch to the right of
the object to touch.
EXAMPLE: G90 G1
M64 M66
L9101 R0+1. X-3 F25. P1
M0
X1. G0
M99 P1
The function for the L9101 subroutine is selected with the R0+1. selects function 1 of the L9101 subroutine. The function requires four items:

1) The R0 variable to select the function
2) The move to the point
3) The approach feed rate
4) The desired P variable

In the example above only the X axis will be stored because it is the only axis move in the L9101 line.
Compare this method of picking up and storing a touch point to the methods discussed previously in this section. Each method will store the points needed; selecting one method over the other is a matter of programmer’s preference.
Note that one disadvantage of using the L9101 fixed subroutine is that it must be written in absolute terms.

EXAMPLE: G90 G1
M64 M66
L9101 R0+1. X-3. Y-3. F25. P1
M0
X1. G0
M99 P1
In the example above, the X and Y axis positions will be stored because they are the axes in motion in the L9101 line.

Touch Probe - Tool
Diameter Offset

The tool diameter offset is achieved by a two step process as follows:
1) The CNC is programmed to touch the probe at two points.
2) The L9101 R1+8. code is used to perform the calculation.
EXAMPLE: After the length offset has been located, the following program is used to
establish the diameter of a 1/2" end mill.
N1 G0 G90 S500 M4 E24 X0 Y-.5 (.200+.25+.05
N2 H1 Z-.1 M65
N3 G1 G31 Y0 F5. P1
N4 G0 Z.1
N5 Y.5
N6 Z-.1
N7 G1 G31 Y0 P2
N8 L9101 R1+8. R2+.4 D1
N1: The E24 shifts the XY zero to the center and the Z zero to the top of the
stylus. The X0 moves to the center of the stylus. The Y-.5 moves to a clearance
position, calculated as follows:
1/2 the width of the stylus: .200
1/2 the approximate tool diameter: .250
Clearance: .050
N2: moves the tip of the tool .100" below the top of the stylus while spinning
the tool backwards at 500 RPM.
N3: moves to touch point 1.
N4: moves Z .100 above the stylus.
N5: moves to a clearance position in preparation for the next touch.
N6: moves Z below the top of the stylus.
N7: moves to touch point 2.
N8: performs the diameter calculation.

The stylus width is specified by R2. The D word specifies the diameter is to be stored as offset 1 in the tool table.

General Rules to
Follow: MP Series Probe
1) Start the program by selecting the probe. M64 selects the MP Series
probe, M65 selects the TS Series probe.
2) A move with the G31 must be a linear (G1) move.
3) No other codes are allowed with the G31 except G1, P# (Point Number),
and feed rates.
4) The Probe functions may only use three points for each calculation, P1, P2,
and P3.
5) The probing is to be in the absolute mode (G90).
6) CRC, Mirror Image, Rotation and Drill Cycles are not allowed during the
execution of the G31 code.

Locating the Points:
There are two procedures available to locate and store the points:
1) Using the G31 P# codes.
2) Using function 1 of the L9101 fixed subroutine.

Ok, so if i want to measure diameter i must every time to doit, manualy write program? (For each tool)

Hello again,

i know, that im a pain in the ass :)
But im from Europe and here we have almost no expert for machining on fadal. And i must lern my self. Thats the reason im asking here.

Please, if anyone know, do i need to write a program for probe touch(diameter) every time i want to measure the tool (diffrent ones)?

Check with Joseph Margraff. He is Fadal's service corrdinator in Europe. He might be able to put you in touch with some one in your local area that can help you out. You can contact him by email --- jmargraff@mag-powertrain.com

Neal

Thanks to all. I manage to mesure diameter. I write a program that fizzissist give me, transform in to the metric units and start program.
It works :)