Help with Fanuc O-M setup

I bought an old VMC a few months ago and am finally getting around to running some parts on it.

As background, I have run several different kinds of CNC machines, but have never run a CNC this old. It is a totally new experience for me. There are many things that, out of ignorance, I find totally absurd. Functionality and code that I am used to using that apparently do not work in the older controls. For example, in MDI typing G0 G54 X0 Y0 does nothing. Tool changes are not a simple T3M6, G90 G30 Z0.0 followed by a G91, followed by your T3M6. Or when you hit reset while running the program it does not kill the spindle, you have to go under MDI and enter an M05.

So, to the current issue at hand....

Setup the part in the vise, set my Z from the machine coordinate off the spindle face. Put that under my work coordinate. In this case I used G54. Touched my tools off the table, using the machine coordinate, and entered in the Tool Offset page. Both are negative numbers.

This as follows is what I posted, and modified, and was running.

(T3 D=0.375 CR=0. - ZMIN=-0.5791 - FLAT END MILL)
(T5 D=0.25 CR=0. - ZMIN=-0.5841 - FLAT END MILL)
N10 G90 G94 G17 G49 G40 G80
N15 G20
N20 G28 G91 Z0.
N25 G90

(2D CONTOUR2)
G0 G90 G80 G49 G40
G0 G91 G30 Z0.0
G90
N30 T3 M06
(38 ROUGHER)
N35 S3060 M03
N40 G54
N45 M08
N55 G00 X-1.0963 Y0.0015
N60 G43 Z0.6 H03
N65 G00 Z0.2
N70 G01 Z0.1 F30.
N75 Z-0.5791

When the machine gets to N60 the machine has a distance to go of -35.9746. The distance from the tip of the tool to the top of the part is about 18.6" eyeballing with a scale. My work coordinate Z is -20.478 and my tool length offset is -16.894.

I do have the manuals that came with this machine, which have done nothing but serve to make me more confused. In one section they show code like this:
G21 G90
G10 L2 P1 X--- Y--- Z---
G0 G90 G54 G40 X-- Y-- S--- M03

I tried entering this and got the same result.

In one section on tool setting they state that the tool numbers must be positive. So we tried making the tool numbers positive, that did not seem to work, as the machine traveled about 4 inches below the G30 position.

In another section I found it states G43 can only be used for Z+ numbers, G44 Z- I had never even heard of G44...

I realize now, I have been extremely spoiled in my machining career and because of it, have a very poor understanding of the basics. I have had lots of experience with conversational programming, probes, CAM software, but most of my coding is usually macros and subprograms on newer machines or modifying posts. This departure has been humbling!

If you have a huge negative work offset your tool offset should be positive. The machine crunches these numbers to go to the correct place in Z. Work offset Z, H offset and programmed position (this could include math done with variables). A easy way to set up is set the tool off a fixed point. Then measure from that point to where your program zero is and set that as your work offset. This may be a positive or negative number.

I tried a positive tool offset as I mentioned. The tool went about 4 inches below the G30 position.

My work offset is -20.478, the machine has just shy of 20" of travel in Z if I remember right, so this number does not seem out of line?

Here are two quick shots.

I loaded up the program and ran till the tool hit the G43 and started to move to the cutting plane.

First pic should be the tool offset negative second should be everything the same, tool offset positive.

Fal Grunt said:

Setup the part in the vise, set my Z from the machine coordinate off the spindle face. Put that under my work coordinate. In this case I used G54. Touched my tools off the table, using the machine coordinate, and entered in the Tool Offset page. Both are negative numbers.

Click to expand...

Hello Fal Grunt,
If the Spindle Nose is being used to set the Z Work Shift, then ALL Tool Length Offsets will be positive. You're setting your Tool Length Offsets incorrectly. You can't just touch off the tool on the table and use the Machine Coordinate value as the Offset. If the Spindle Nose is to be used to set the Z Work Shift, then the distance from the spindle nose to whatever is being used as the Reference (the Table in your example) when gaining the Tool Offset, needs to be taken into account.

Lets say that the distance from the Spindle Nose, when the Z axis is at the Z Reference Return Position, to the table is -500.0mm and the Machine Coordinate value displayed when the Tool being measured is -400.0, when its tip is touching the Table, then:

S = -500.0
T = -400.0
O = T - S
O = 100.0 (a Plus Value)
Where:
S = Distance from Spindle Nose to Table (Table being the Reference Plane used when measuring Tool Lengths)

T = Position of Tool Tip from Z Reference Return when Tool Tip is touching Table (Reference Plane)

O = Resulting Tool Offset

Fal Grunt said:

In one section on tool setting they state that the tool numbers must be positive. So we tried making the tool numbers positive, that did not seem to work, as the machine traveled about 4 inches below the G30 position.

Click to expand...

Where the tool is relative to the Z G30 (Second Reference Return Position) means virtually nothing, unless the Z G30 Position is taken into account when calculating the Z Work Shift and Tool Lengths

Fal Grunt said:

In another section I found it states G43 can only be used for Z+ numbers, G44 Z- I had never even heard of G44...

Click to expand...

I doubt that it actually said that. What it would have actually said is that G43 will apply the Offset in a Plus Direction and G44 in a Minus direction. Meaning that if the Offset Value is a Plus Value, G43 will apply the Offset in a Plus Direction and if its a Minus Offset Value, G43 will still apply it in a Plus direction, but because the Offset Value is Negative, then the net result is a negative movement. Its exactly the same as adding a Negative Number in an equation. A better way of looking at the use of G44 is that it Subtracts the Offset Value, rather than Adds it as is the case with G43. G44 is generally seldom used and there is no real need for its use over G43.

Regards,

Bill

Bill,

Thanks for the post and explanation. I ran a Deckel 5 axis for about 8 months that we manually set tools on (my only real experience doing that). However, I am a little confused, as we always set the tools from the table, and the work coordinate from the piece being machined? We only measured a tool if we built a new one, only changing the Work coordinate from piece to piece. I feel like I am over complicating this...

So, for reference to make sure I am doing this right.

I need to bring down the spindle nose to the table.
Record the machine position. (S)
Bring my tool down to the table
Record the machine position (T)
Subtract S from T

My comment about the G30 may have been misleading. I meant only to provide it as a reference as to where the tool wound up at the time of the move.

Concerning G43/G44, I think your explanation is much more understandable. After I get this up and running I will try to find the section. It is very likely, as you stated, I misunderstood what it meant.

Now that I type this up, part of it is coming back to me.

Fal Grunt said:

Bill,

So, for reference to make sure I am doing this right.

I need to bring down the spindle nose to the table.
Record the machine position. (S)
Bring my tool down to the table
Record the machine position (T)
Subtract S from T

Click to expand...

Hello Fal Grunt,
That's correct if the Spindle Mose is to be used to set the Z Work Shift. Of course, you won't get the Spindle Nose to touch the table. Use Gauge Blocks, or whatever measuring device that's available, in conjunction with moving the Spindle down towards the table as far as it can go, to be able to determine the distance from the Spindle to Table when the Spindle is at Machine Reference Return. You only need to get this dimension the once and use it whenever setting tool lengths. Also, it need not be the Table Surface that is used as the Reference Plane. It can be anything that represents a constant Reference each time a tool is being set; a manual Tool Setting devices incorporating a Dial Indicator for example. Whatever device is used, the Spindle (S) value in the equation will be the distance from the Spindle Nose to the Setting Device when the Spindle is at Machine Reference Position.

The result of setting the Tool in the way described, is a tool length Offset that is eqial to the distance from Tool Tip to the Gauge Line of the Tool Holder's Taper (Spindle Nose).

Regards,

Bill

Ok Bill,

I am closer, but not quite there yet.

Followed your procedure, made a little tool setter, got my tooling numbers.



T3 & T5 are my tooling numbers. The other tooling offsets are the previous owners.

After setting up my tooling numbers, I rechecked my G54 Z setting just to verify.

Ran the program. I get down to my part in the vise, and I have 8" "distance to go", but the tip of the tool is only about 1.75" from the top of the part.

Fal Grunt said:

Ok Bill,

I am closer, but not quite there yet.

Followed your procedure, made a little tool setter, got my tooling numbers.

View attachment 209166

T3 & T5 are my tooling numbers. The other tooling offsets are the previous owners.

After setting up my tooling numbers, I rechecked my G54 Z setting just to verify.

Ran the program. I get down to my part in the vise, and I have 8" "distance to go", but the tip of the tool is only about 1.75" from the top of the part.

Click to expand...

Hello Fal Grunt,
If you refer to my first Post, I stated that the ALL tool offsets will be Plus values if the Spindle Nose is used to set the Z Work Shift.

Lets say that the distance from the Spindle Nose to the Z Zero of the Work Piece is -200.0mm, and registered in G54. Lets further say that a Tool Length of Zero is set in Offset Number 3. If the Z axis, with no tool in the Spindle and the Drive Dogs removed, was sent to Z Zero with:

G43 Z0.0 H03

then the Spindle Nose would settle at Z Zero on the Work-piece (discounting the Drive Dogs on the Spindle Nose).

Still with no tool in the Spindle, but now with a Minus Value of, say, -100.0mm in Offset 03, would the Spindle not want to bury itself in the Work-piece by 100.0mm if the above program snippet were run? If you were to place the tool in the Spindle that had a tool length of 100.0mm from Tip to Gauge Line and run the above program snippet with the same -100.0 Offset, would the Tool Tip not want to bury itself to the extent of -200.0?

So how is a Minus Tool Offset ever going to work if the Z Work Shift and Tool Length setting are all calculated using the Spindle Nose as the Reference?

It would work, using your Minus Tool Length Offsets, if you used G44 instead of G43; counter intuitive in my opinion.

Regards,

Bill

Your a great teacher and I am a horrible student!

Made chips!

Thank you very much sir!

So, can you hazard a guess as to what on earth the previous owner was doing? I am really confused now!

Fal Grunt said:

Your a great teacher and I am a horrible student!

Made chips!

Thank you very much sir!

So, can you hazard a guess as to what on earth the previous owner was doing? I am really confused now!

Click to expand...

Hello Fal Grunt,
There are numerous methods of setting Tool Offsets. One is the measured Air Gap between the Tool Tip and the Setting Device. In this method, ALL tool Offsets will be Minus values. Another method is to use a Master Tool as the Reference. In this case, its possible to have both Plus and Minus valued Offsets. When using the Spindle Nose as the Reference, in essence, the Spindle becomes the Master Tool that has a Tool Length of Zero. Accordingly, all tools placed in the Spindle must be longer than the Zero Tool Length of the Spindle and therefore, will have Positive Values.

Regards,

Bill

re the tool change in mdi
with my Om NTC in mdi you have to command a zero return in a line before the M6 command
during startup in setting tool offsets if I forget and command a M6 to load the tools into the pots without the machine being sent back to Z0 the tool change won't happen.
As mentioned above,many different ways to set tool lengths.
Evan if your working by yourself on this machine, make cheat sheets to repeat the process.
Nothing worse than setting tools to a + when they should have been set to a -

One good thing about Fanuc controls
That big red button will stop the machine

Mike

I consider the master-tool method safer (not necessarily better) than the spindle-nose method, because offset mistakes would not lead to serious accidents.

mjk said:

Nothing worse than setting tools to a + when they should have been set to a -

Mike

Click to expand...

Hello Mike,
There is one thing; setting tools to a Minus when they should have been a Positive. The inverse will send the Z axis into + Over-travel; not the end of the world. But when an Offset is set to Minus when it should have been a Positive is when things get interesting. The occurrence of what I described in Post #9 is a real possibility.

Regards,

Bill

The use of MEASUR soft key on newer controls obviates such problems.
The control calculates the distance with appropriate sign.

As mentioned above many different ways.
I happen to use G44 for tool to surface values
Much of my work is based on fixtures that drop into the 2 vices that live on the table
Not having to enter the - sign made sense when I started using it
Consistency in your particular shop is the key
New hires knowing the shop standard very important

G43 and G44 have opposite effects. Using both would be risky. We are human beings, not computers.
Moreover, G43 is more logical, as regards positive/negative signs of the offset values.
With G43, a positive offset would shift the origin (Z0) in the positive Z-direction.
This has already been explained by Bill in post#9.
In my opinion, use of G44 should be banned.

Out of curiosity I set a tool with a G44 value to a (-) minus value and it alarmed out in the (+) positive Z direction

As with other commands that are controversial (G28 or G92) they a have there place

As for G44 it was initially chosen when I did a lot of manual programming and saving the - keystroke made sense. Switching the shop now would not be wise

Only G92 is controversial. Rest are fine.