Trouble with offset concept

[bbulich]

Having a little trouble grasping a few concepts and it seems anything I read is practically in a foreign language.

I am primarily using my cnc lathe as of now with the help of mach 3 wizards doing simple turning, facing and grooving functions. I am having trouble understanding the difference between the main DRO on the top left of mach 3 and the DRO that says work coordinates. I

I understand the concept of putting a piece of stock in the chuck, taking off a thin slice and measuring the diameter to get your x-axis coordinates and the farthest face of the chuck is the z-0. But I am not sure which coordinates these are. Couldnt one find the exact center of the x axis and set that to zero, then you could just measure the stock diameter without taking a cut.

If someone has a good reference where these concepts are explained plainly, that would be much appreciated. I feel once I get a grasp on setting the coordinates correctly and tool offsets, things will make more sense. I appreciate any help

 

[bryan_machine]

A more direct answer to your question might be this reference:
CNC programming handbook, 3rd edition
Peter Smid
CNC Programming Handbook, Third Edition: Peter Smid: 9780831133474: Amazon.com: Books


I'm not famaliar with mach 3, but the following ideas are likely to be helpful.

First, many machines have multiple work coordinate systems. Any WCS will define "where 0 is". When you touch off a part, you are defining zero for one of those coordinate systems. That definition will be expressed in terms of some machine coordinate system.

Second, at least some machines will have the ability to display an "absolute" position - which could be relative to an arbitrary place, though it's often relative to the limits of travel of the machine. (Don't confuse this with absolute versus relative moves. With an absolute move "g1 x5" means "go to X=5" while a relative move "g1 x5" would mean "add 5 to what X is now and then go there.")

I suppose mach might also display the distance to go for a move (centroids do that.)

In practice I at least don't look at machine coordinates very much, look at work coordinates all the time.

 

[Tonytn36]

There are TWO offsets you are typically dealing with on a CNC.
1. Work Offsets
2. Tool Offsets

On a lathe, the typical (but not always) work offset is based on the distance to the center of the spindle and the face of the spindle (behind the chuck) - FROM A FIXED POSITION ON THE TOOL SLIDE. As Bryan noted, this is typically tied to machine travels (but not always). A work offset moves the Z to either the face of the chuck or to the end of the workpiece. It can also move X, but there is rarely a need in a lathe application. Yes, you can (and should) set up work offset X as center of the spindle. But.......there is a problem with that....if you aren't using Tool Offsets....

Tool offsets are the relative distance in X, Z of the theoretical tool tip from a fixed reference point on the tool holder (ex: Turret Face, center of boring pocket for a typical lathe tool turret.)

If you have a presetter (or tool probe) for your lathe tools to determine where the tool tip is relative to this fixed reference point, all is good with setting X work offset at center of the spindle. Every tool has a different dimension and thus the tool offset is added to the work offsets to get actual slide position. If you do not have a method of determining the tool offset (presetter or tool probe) then the absolute method of always having X at center of the spindle and Z at face of spindle for work offset cannot be used as you do not know where the tool tip is in space. When you cannot set the tool offsets, then you must use the touch-off method of setting X and Z.

 

[bryan_machine]

"When you cannot set the tool offsets, then you must use the touch-off method of setting X and Z" <= for *each* tool....

You can think of it as 3 levels of address, over 2 levels of math.

; assume there's a tool library and it says that T5 has tool offsets of X=1 and Z=1 - just for illustration.
T5 D5 H5 G43 ; or something similar - tells machine "use tool offset 5" and load tool 5. (May be an M6 required)
G1 X4 Z4 ; says move (assume absolute mode on lathe)
; the move is to move the TIP of the TOOL to X=4 Z=4

That move involves 2 adds for each axis.
First, subtract the tool offset (which might be negative) to the target location based on the work coordinate system.
So "G1 X4 Z4" becomes "G1 X3 Z3"

Then, add the result of the previous step (which might be negative) to offset of the work coordinate system relative to the machine coordinate system.
The result is pair of numbers that directly drive the tool slide in X and Y in direct hardware terms.

You (OP) don't need to stress about the translation, what you need to do is find a pattern of work that sets tool offsets and work offsets in a way that works on your machine.

 

[bbulich]

okay, that makes since, but in order to do any of the above, I first need to set tool offsets with a tool probe or presetter? Is there a good thread on using ofthese, as I have not done this before. It makes sense that there should be some kind of gauge that helps find the exact center of the spindle.

 

[Garwood]

Machine reference point (origin, ZRN, whatever)

Part origin

Work offset(s)

Tool offsets

That's it, nothing else, no tool setter probe thing necessary.

The machine's reference point is where the machine considers zero. The work offset is the distance in X and Z from this point in space to the part origin.

The function of the work offset is to tell the control where 0,0 is on the part so the numbers in the program make sense.

The part origin is 0,0 on the print.

Tool offsets tell the control the tool length differences.

If that seems too complicated at first think of it like this-

None of that shit is necessary. You can program any CNC machine without any work offsets or tool offsets. You can write the entire program from the machine's reference point or start the machine at the part origin point. You could put the tool offsets in the program using an actual movement to comp for the tool differences.

This is how really old shit used to work- No offsets, or atleast minimal.

Folks realized it's a lot simpler to put that info in the control and not in the program because putting all that shit in the program means you have to redo the program any time you change the littlest thing.

 

[CarbideBob]

All of this is still so confusing.
So the machine has some zero where it found it's switches when I turned it on.
I get to set a new XYZ system putting zero where I want.
Zero in my world is offset from the machine's brain dead stupid zero , ...ah I see, offset, the machine knows nothing, I know were my part is.
Must be some code to tell it to think in my world. Probably very bad if it starts thinking in it's own zero instead of mine.

And then Tony tells me I need to set my new zero at the chuck or end of part.
Why can't I set my zero halfway down the part on the side of the groove I'm cutting?
Seems like it is my zero and if I want to put it 1320 feet from the finish line I should be able to do so.

Now on diameters seems like I should be able to shift so that my short tool make a zero dia part.
But when I change to a long tool, machine goes to the same place and, oh my gawd, mini diameter comes out.
Looks like I need a new offset for tool length.
Two in/out part diameter(X) offsets? How do I keep my first, which is my part in the world in front of me, and handle the second?
A whole new set of offsets just to keep track of how long my tools are?

WTF, now I have to tell the stupid thing where the end of my part is, some silly work coordinate system, (My XYZ to the world which you would think it would know)
Now added on top some tool length offset thing where everyone with the brains God gave a rock knows longer tools cut deeper.

All this computer power and the darn thing is stupid.
It's a conspiracy, I'm telling ya. All designed to make things harder than they should be.
(To the OP, a bit of fun here, but yes it's a bit crazy at first)
Bob

 

[bryan_machine]

(OK, Bob added to his post and now I see he's pointing the oddness of all this.)

Indeed, no matter what I do, I cannot cut a negative diameter!

bbulich - Keep in mind that it's just the controller doing a bunch of adds (or subtracts), and it does indeed do it mindlessly (and YOU have to get the +- sign right) But given that fact, and the point that the machine itself can be used to measure tools, all you really need to do is find out the easiest/best way to get the right numbers into your controller.

 

[CarbideBob]

(OK, Bob added to his post and now I see he's pointing the oddness of all this.)

Indeed, no matter what I do, I cannot cut a negative diameter!

On one, don't type too quick behind me, I'm a bit slow ........
On two, of course you can, but once you accept this you have to go live in an alternate universe and we don't get to chat with you anymore.
(Think about that next time your part disappears into thin air)

Offsets all seem so straightforward until you try to explain them to somebody else.
Then you see their eyes glaze over and you know you have lost them.
So many ways to play with these numbers. I like to stretch people and put the zero way outside of the machine envelope.
What if your zero was in Houston and you are sitting in Flint? Ok, now put zero where Santa sits.
How about you have a 10 mile long tool and the next one is 10 thou. long?
Big gaps people get, inside the machine, little numbers.
Silly, yes, but it seems to work for me.

Bob