Hardinge VMC600 W/Fanuc OM controller - setting offsets?

[Larry1958]

I am wondering if there is an easier way of setting work and tool length offsets on the lower end Fanuc OM controllers. I have no Calculate, or Measure features. The only way I can get it to work is to zero out the registers, then check machine position screen and enter those numbers into the offset registers. This is a pain in the neck, and I am sure there must be an easier way. I have had Hardinge service people hare and they are no help. Thanks in advance.

[Dave Ball]

are these repeat jobs in which you already know, or can calculate the offsets offline ?

[Larry1958]

No, mostly just 1 offs.

[Larry1958]

No presetter here either. Come on, there has to be someone here that knows this controller.

[chowquoe^]

Larry,

 

First off, I feel your pain. I have 3 of the 0M controllers. Depending on what you would like to do there are 2 options.

 

A) Positive tool lengths:

Pick an object in the machine (I use the vise fixture or what ever my work holding device is) bring the spindle face down and touch off a 3" block on that object. Goto the position page write down the Z axis machine coordinate (DO NOT MOVE 3" BLOCK). Load tool in spindle, touch the tool off the same 3" block. Position screen, machine Z axis position and subtract the two numbers. (I know more math) This will give you a positive tool length.

 

Negative tool length:

Sounds like you are doing this method above..... Bring tool down to programmed Z zero touch off and input the Z axis machine value into your tool register.

 

Option B is definitely the faster of the two and there is no math involved; however if you are using multiple workshifts this can get you in trouble if you are not careful.

 

I am currently looking at purchasing a tool tightening block, using method A above get a known tool length and modify the block so it can be used on a surface plate with a height stand to measure tools.

 

Sorry I have know magic (measure) button or a (Z input c.) answer for you. I can say again I feel your pain, I absolutely despise these controllers as far as ease of use goes.

 

"M6 (insert) T1 (eob)" what a pain in the arse.

 

Hope that helps a bit.

[Dave Ball]

Larry, Sorry to say your kinda stuck. Your options are very limited with that control. Now if you had custom macro you could write something up that would copy the machine position values into the desired work offsets which would be a little better, but since its an O control thats not likely an available option either.

[Guest CNC Apps Guy 1]

code:

---

%

O8503(AUTO TOOL SET AND CHANGE)

IF[#4120 EQ 0]GOTO1

IF[#4120 GT 0]GOTO2

IF[#4120 GT 21]GOTO1

N1#3000=1( TOOL# NOT 1-21 )

N2G0G#4006

#20=#4120

#[11000+#20]=#5023

IF[#20 GT 21]GOTO3

IF[#20 NE 21]GOTO4

N3#20=0

N4#20=#20+1

G0G91G28Z0

G90

G49

T#20M6

M30

%

---

You mean something like this???

[Larry1958]

Chow,

 

I use option A. I like to have real tool lengths for my offsets. I guess I will have to look into writing a macro program to do this.

 

CNC Apps, I looked at yours but it does not look like that will work. I need a M00 to touch off tool, then something to capture the positions and do the math from there. I also use a 3" block to set off tools and set Z work offset from face of spindle. Thanks.

[Tim Johnson]

Here's mine for an 18i;

code:

---

%

O6002(MAIN TOOL LENGTH MEASUREMENT PROGRAM)

(START PROGRAM WITH SPINDLE TIP TOUCHING TOOL LENGTH PRESETTER)

 

G65P6003A0.B40.

(A = TOOL NUMBER TO BE MEASURED -- MAKE 0 IF SPINDLE IS TOUCHING PRESETTER)

(B = NEXT TOOL -- MAKE 0 IF LAST TOOL)

IF[#101NE0]GOTO2

M00(SPINDLE CALIBRATED)

GOTO1

N2IF[#102NE0]GOTO1

G91G30Z0

G30X0Y0

N1M30

 

O6003(SPINDLE CALIBRATION)

#101=#1

#102=#2

IF[#1NE0]GOTO1

#5221=#5021

#5222=#5022-1.0598

#5223=#5023

T#2

GOTO2

N1M98P6004

N2M99

 

O6004(MEASUREMENT PROGRAM)

IF[#5223EQ0]GOTO98

G91G30Z0.

G30X0Y0

M06T#101

#103=#4120

IF[#2EQ0]GOTO1

T#102

N1G90G00X0Y0G54

M00(TOUCH TOOL TIP TO TOOL LENGTH PRESETTER)

#[#103+2000]=ABS[#5223-#5023]

IF[#102NE0]GOTO99

#5221=0

#5222=0

#5223=0

GOTO99

N98#3000=99(SPINDLE TIP NOT CALIBRATED)

N99M99

---

[Dave Ball]

yes, or this...

 

%

O9100 (Program to touch off tool lengths)

#3006=101 (TOUCH SPINDLE NOSE TO BLOCK)

#5003=0 (Set current Z position as program Zero surface)

G91 G01 Z1.5 F30. (Move away from block in Z)

G91 G28 Z0 M19 (Move to tool change position)

#101=1 (Counter for tool station number)

N1 T#101 M06 (Place current tool in spindle)

#3006=102 (TOUCH TOOL TIP TO BLOCK)

#[2000 + #101]=#5003 (Set tool length compensation offset)

G91 G01 Z1.5 F30. (Move away in Z)

G91 G28 Z0 M19 (Move to tool change position)

#101=#101 + 1 (Step tool station counter)

GOTO 1 (Return to N1)

%

[Larry1958]

Sheffer. Thanks you very much. If you have the time could you explain the code a little bit for me? I cant seem to find any #5000's in my parameters list and cant get my hands on a list for my controller. I can write basic macro - b programs but need to have the book so I can see what does what. Thanks again.

[#Rekd™]

Hi,

 

Our Daewoo has an Oi fanuc and we have a Renishaw laser on it and their macros work great.

 

John

[ToolMan184]

It seems to be it would be much easier and cost effective to do what John is saying. Get a renishaw tool setter and use their macros.

[exjay]

try this code. it works on all our fanuc controls.

change the -1.0 to suit the gauge block height(-.5 for 1/2 inch block etc)

we run it in MDI . Alter M99 to M30 to run in memory. Be sure #4120 is tool in spindle NOT tool on waiting!

 

%

0011

(TOUCH OFF TOOL TO 1 INCH GAGE BLOCK)

(IN MDI MODE ENTER M98 P11; HIT CYCLE START)

(TOOL RETRACTS TO Z HOME AND TLO INSTALLS INTO CURRENT T REGISTER)

#[2000+#4120]=#5023-1.0

G91 G28 Z0

G90

M99

[Dave Ball]

Larry, I hope this explains things. The whole cycle is a little scarry at first but if you overide the rapids and single block it you will trust it in no time.

 

quote:

---

To use this program, the setup person loads all the tools to be measured into the machine. Then, just like doing it manually, they place a block on the table to be used as a reference point in Z (the top surface of the work holding setup is commonly used). They then position the machine in X/Y so that the spindle nose (no tool in spindle) is above the block. When the program is excuted, the operator will be asked to touch the spindle nose to the block. Just as when measuring tool lengths manually, the operator will place the machine in manual mode, use jog to quickly position the spindle nose close to the block, and then cautiously touch the block using the handwheel to "measure" the spindle position. When this is done, they will place the machine back in automatic mode and press cycle start. The control will record this position in Z as the current program zero point (just like the operator does when manually presetting the Z axis display to zero) and then automatically move the machine to its tool change position. Tool number one will be placed in the spindle and the machine will stop again. The operator places the mode switch back to jog and cautiously touches the tool tip to the block. When this is done, they place the mode switch back to automatic and press cycle start. The length of tool is automatically stored in offset number one! This process is repeated for each tool until the last tool length is measured. This technique dramatically simplifies the tool length measuring process for the operator and eliminates tool offset entry mistakes.

---

[ken wong]

Press e.o.b and Z together then imput Z value will there