Help with Fanuc O-MD control

[within a thou]

I have a VMC with a Fanuc O-MD controller. When running a program the tool length offset (H value) is added to my actual Z position (for example if I am programmed at G90 Z-1. and my H value for the tool is -1.5 on the actual position page it shows a z value of Z-2.5) and I know it is a parameter setting to turn this off. I am just not sure which bit I need to change. Any and all help is greatly appreciated.

[Josh T™]

Check to see what postion screen you are in. You should have 3: Machine / Absolute / Relative

 

Absolute will show you what you want to see.

[crazy^millman]

Are you on the right fixture offset? Do you have a general Z offet on the workoffest page?

[Todd Mann from Fastech]

Are you using a tool setter? We use a tool setter and the length from the spindle nose to the tip of the tool is in the tool length offset as a positive number. In "G54" we touch the nose of the spindle off the top of the part if thats where "Z" datum is and everthing works fine.

[within a thou]

Yes I am in Absolute this parameter is bit 5 of parameter 018 on other fanuc series controllers I just don;t have the proper parameter book.

 

No I am not using a tool setter I have a reference tool with a H value of 0.0 I touch that off where I want it then in my G54 offset page I type the actual machine position in reference to home. then when I set a tool after that it is the difference of the length of my cutting tool to my standard and that difference in length becomes my H value

[Dan_AKA_ROY]

Fanuc Series 0-MD here...

 

I never bother using a reference tool myself. I just touch off bits to be used using a 123 block and add or subtract the difference from the stock thickness and input it in the corresponding tool offset number. If a stock mikes out to 2.525", I touched the tip of the bits off to the 2" side of 123 block and subtract .525" then input this value. Its super fast touching off bits this way for me so I've always stuck to this way.

 

As for using a reference tool...

 

1. Touch off ref tool to your stock.

 

2. Press function key (POS) until the current position display screen with relative coordinates is displayed.

 

3. Reset the relative coordinate for the Z-axis to 0 (press CAN key)

 

4. Press function key (MENU OFFSET) until the tool compensation key is displayed.

 

5. Use manual operation to move the tool to be measured until it touches the same specified position. The difference between the length of the ref tool and the tool to be measured is displayed in the relative coordinates on the screen.

 

6. Move the cursor to the compensation number for the target tool (the cursor can be moved in the same way as for setting tool comp values).

 

7. While holding down the (EOB) key, key in address Z. If either X or Y key is depressed instead of Z key, the X or Y axis coordinate value is input as a tool length comp value.

 

8. Press the (INPUT) key. The Z axis relative coordinate is input and displayed as a tool length offset value.

 

^ Thats from the FANUC Series 0 Operator's Manual...

[Dan_AKA_ROY]

3. Reset the relative coordinate for the Z-axis to 0 (press CAN key)

 

^ Manual says see section 11.1.2 for explanation...

 

1. Press function key (POS)

 

2. Press soft key (REL).

 

(So, pressing the CAN key resets the relative value to 0).

[doyleg]

within a thou, check parameter # 18 bit 5 (6th from the right) it should be a 1.

[within a thou]

yes ROY I am doing that now but my actual machine parameter data bit is set wrong depending on how it is set the tool length offset is aded in my absolute position Z display or you can set it so it doesn;t add it to my actual G90 position. I just don;t know which data bit I need to change to make the display to not include my compensation value

[doyleg]

also check parameter 28 bit 0 , it should be a 1

[within a thou]

Now the book says I should use 018 and my control shows 0018 is this the right paramter or am I on the wrong page

[within a thou]

my parameter are set as follows

 

bit 18 00000100

bit 28 10001101

 

and it hasn't changed anything

[within a thou]

and Millman yes I have a value in my G54 Z offset. Everything works it just does not display the proper Z value on the screen it is still adding the offset to my Z even after changing both of those bits

[Dan_AKA_ROY]

Oh, OK.

 

:Gilda Radner voice: "Nevermind."

 

---------------------------------------

 

Remember to turn power off before a changed parameter can take effect...

 

I found this...

 

Selection of tool length offset

 

Select tool length offset A, B, or C by setting bit 6 of parameter 003 and bit 3 of parameter No. 119.

 

- Not sure if that helps, but I tried. Hope you get it working the way you want.

[within a thou]

even after repowering it is still the same. ROY ya that doesn;t apply to this but that is the answer o my next problem lol I am just tryin to prioritise this mess. I just started with this company they were running this machine so back arsewards I am trying to get us up to speed. Not only do I not get to see where my actual Z is at If I marry My H and D values (G43 H1 and G41 D1) it adds both offsets and applys the sum of both of them to both my length and diameter offset. Also when I run off DNC my control is completely blank luckily I am the programmer and not the guy in front of it

[doyleg]

parameter # 18 = 00100000

or 00100100. the 2nd bit (3rd from right is for adjusting feed magnification in one of the axis'. not sure which one. so you can leave it at 1 if you don't have any probs with it.

[doyleg]

remember your bits to the parameters are read from right to left. bit "0" is on the right, bit "7" is on left.

[Charlie Pierson]

Parameter 18, bit 5

[within a thou]

doyleg you the man now I feel dumb I was reading it backwards thank you and everyone else who chipped in now on to my next problem lol

[doyleg]

cool - if you have other probs or want to set your machine another way - other than proprietory info from fanuc, like memory expansion and the such - i do have the parameter book but it doesn't show any of the parameters that is the proprietary info.

[within a thou]

quote:

---

Remember to turn power off before a changed parameter can take effect...

 

I found this...

 

Selection of tool length offset

 

Select tool length offset A, B, or C by setting bit 6 of parameter 003 and bit 3 of parameter No. 119.

---

Right now my machine is set up it If my offset page is set up as follows

 

H1 -1. D1-1.5

 

When I program

 

G43 H1

 

it adds them together and gives me a H value of the sum of both (in this case Z-2.5)

 

This is also true when I use G41 it shifts my diameter by 2.5 and not the 1.5 I want it to.

 

Now what I want to o is set the machine up so I can use the same H# and D# and have it so they don;t compound.

 

Right now I currently have to use 2 seperate numbers the control doesn;t recognise the difference between my Length offset page and my wear offset page and reads them both as one number

 

Does the book have the combination of Bit 6 parameter 003 and bit 3 parameter 019 to allow me to do this?

[Guest CNC Apps Guy 1]

Right now the machine is set for Tool Offset "A" (1 Column)H one number D another number not used as H anywhere.

 

Tool Offset "B" is H&D same number with no wear (2 columns).

 

Tool Offset "C" is H&D same number in addtion to wear values for H&D (4 Columns).

 

That is an option (read you're going to have to pony up some $$$ to Fanuc) to have the same H&D. NO gettin' around that.

[within a thou]

Thanks again I have a 24 carriage ATC guess I will just create a standard of adding 30 to my D value so there is no interference and my operators know whats going on.

 

My other 2 problems are when I run off DNC the program does not display on the controller is this a add on or is there a way to get this program on my screen? Makes it hard when all you can see is distance to go and current codes being executed.

 

The last problem is when I use G83 my tool starts feeding from .100 above the previous peck depth which is way to far away. I would like to change it to .04

[within a thou]

2 coloums would be more then sophiciant (I need to learn how to spell) can that be created without the extra ponies?

[crazy^millman]

quote:

---

The last problem is when I use G83 my tool starts feeding from .100 above the previous peck depth which is way to far away. I would like to change it to .04

---

There is a parameter for that look the book for the canned cycles and read carefully and it will tell you what one to adjust.

 

No book here when working from home so can not be of much help.