I have been running multi tool operations and have been either digging to deep or shallow.

I think I understand now, but Im looking for reenforcement to my though process.

The tool offset is the distance from the tip of the tool to the top z level of the table? while the machine is set to zero.

Now this is probably pretty accurate, however what im missing is the variable of the stock thickness. If I home the machine to zero and load a 1 inch thick stock on the table, do I need to change all the tool offsets or is there a stock offset I need to adjust?

I use visual mill to do this so if you have VM please let me know

From what I have learned thus far here are the formulas to work from.

Variables:
1. Stock
2. Tool

Constants:
1. Table
2. bottom of collet in spindle at Z zero home

Measurements to make for offsets:
1. The distance from the tool tip to the table
2. The distance from the top of the stock to the table

So is measuremeasurement 1 the tool offset?
and is measurement 2 the stock offset?

Am I making this more complicated than it needs to be?

I think you'll find it better if you set Z=0 to the top of your stock. The table location shouldn't be a constant, the top of the stock is.

Depends, Z Zero could be anywhere as long as all your Tools are set to the same Position your controller dose not care where this is.

You will have to find a suitable surface to set your Tools from, then you may call this
Position Zero or any other number that corresponds with your Program.

To make things easier to comprehend most People use Numbers that will relate to your Part. One example is to make Z zero the top of the Part this way all negative numbers are inside the Part and all Positive Numbers are above, much easier to read a Program with this in mind.
Often the Top of Stock will contain some Exess Material for a cleanup pass later.
For example is your Stock leaves 0.1 inch extra on top you may want to call this Position 0.1 instead of zero.
You will have to keep track of this, if one of your Tools breaks or needs to be reset after you have allready machined off the exess on top of the Part you will have to
set this Tool accordingly.

On the other Hand if you happen to use the same set of Tools for a variety of Parts
with different hight it makes a lot of sense to use the Machine Table as Z Zero.
If all your Parts are Programed this way you can machine differrent Parts without having to Set your Tools for each new Setup.
This also will not require you wory about machining off the Setup Surface on your Part.

Hope this helps
Good Luck

I think you'll find it better if you set Z=0 to the top of your stock. The table location shouldn't be a constant, the top of the stock is.

I realize this might be a common method, Ger, but it has a catch: is the top of the stock really an immutable reference point? Suppose you are machining parts from 2 different pieces of bar stock, and one bar is .005 inch thinner than the other? In actual fact, the bottom of the stock is the locating surface, not the top.

However, I do not like Z0 on the bottom either. I do like it on the nominal top of the job.

I prefer to set all tools to an unchanging reference. This would be to the table, or to a gage block sitting on the table.

Now to Replicapro's question: no, you do not have to change all your tool offsets.

What you are missing is the use of the Z value of the current work offset. You need to make one more measurement (either by calculation or on the machine) as the difference between the level you set your tools at, and the intended level of the top of the stock. This difference in your example would be Z1. in the G54 work offset register, if that is the current work offset in use.

Your CAM system merely places the call for the correct work offset that you intend to use. The actual setting of values for the work offsets takes place directly at the control during setup.

Tweaking the Z value of your work offset safely adjusts for variation in stock thickness for the whole set of tools you have defined in the machine.

Hu,
We surely don't wan't to get into Z home position. Or do we?
Regards, Walt

The Tool Length Offset is always measured from the Face of the spindle to the Tip of the Tool. This Length Offset is always constant irrespective of the Part height. Tool Length is also positive allthe time.
We measure this length for each tool & store in the Tool Length Offset Table.

We have to find out the Z-axis Co-ordinate of the Workpiece Table, when we touch the Face of the spindle to the Table. This we can measure by using a Slip Gauge or a Block with known height.

When the Spindle Face touch the Work Table surface, the Z-axis co-ordinate is say -500mm. Then the height of the part to be machined is measured, deducted from -500mm and stored in the Workpiece Offset Table (G54, G55 etc.). e.g. if the workpiece is 100mm in height, then the Z-offset of the workpiece is -400mm. We write -400mm in G54 (G55) table, under Z-axis Offset.

Here onwards, whenever we change the workpiece, we have to change the G54 (or G55) offset as described above.

Tool Length always stays constant, unless new tool is mounted.

Now, when we run the program we write it like follows:

G91 G28 Z0
G91 G28 X0 Y0
G90
M6 T10 (Call Tool & Load in the spindle)
G0 G54 G90 Z100 G43 H10 (Call Workpiece offset, Call Tool Length Offset and Move the Tool Tip 100mm above the workpiece surface, H10 is the location, where the Tool Length is stored).

Hu,
We surely don't wan't to get into Z home position. Or do we?
Regards, Walt

I don't know, Walt. What do you want to say about it? I'm listening. :D

I'm starting to see the logic behind what Smabhyan is saying, particularly in cases where the tooling might be shared amongst many machines. I haven't advanced to that point yet, that is, I would always set the offsets for the tooling on the machine I was going to use the tooling with, and my length offsets would be negative. So in my situation, the Z home position does not really come into consideration, because it is what it is, and all that matters is that it be correct and repeatable so far as the tool changer is concerned.

I sit here scratching my head about using the spindle face as a reference. I doubt that the face of every spindle is really exactly the same, so to discover some kind of uniform and universal gauge height, you still need a guage toolholder sitting in the spindle to find a common reference between all machine spindles.

I'm starting to see the logic behind what Smabhyan is saying, particularly in cases where the tooling might be shared amongst many machines...

If you have a large operation where tools are preset in a tool crib and come out with a corresponding list of tool lengths these are entered into the machine for tool offsets and then the Z work offset is taken to the reference point described in the print or program. In this type of situation there are many people involved in implementing a program and producing a part so you need to have defined procedures.

If you are the person selecting the tools, putting them in holders, setting up the machine and doing the whole thing the precise way you define tool offsets, work offsets is your choice.

If you are somewhere between then Torsten's comment: "much easier to read a Program with this in mind" comes into play. Exactly what system is used and what is "in mind" does not really matter provided everyone involved follows the same system and has the same thing in mind.

smabhyan,
I agree with much of what you are saying except for measuring from the face of the spindle for a reference point.
The reference point for measuring tool length is the gage line. The gage line is that point where the spindle taper is a certain dimension. This is where the tool comes against the taper and locks into place.
If you measured everything, set your offsets, then ground .050" off face of spindle, the tool length would not change relative to the gage line.
Twenty years ago, White Sundstrand used the face of the spindle to set home position on their horizontal machining centers. Then some busy body came in ground the taper in the spindle and then they wanted the face of the spindle ground back so the home position was right. Slowly, they became aware of the fact, the face of the spindle had nothing to do with where the gage line is located.
Maybe a step by step to set home position would help in this situation.
I usually used a test bar. The "ExCello" test bar was manufactured so it was 2.0000" in diameter and 16.0000" from the gage line to the end of the bar.
This is for a 4 axis, horizontal machine. Place the test bar in spindle. Move X axis to center of travel. Place mag base indicator on table adjust indicator to be on the side of the test bar. Move Y axis up and down to find the high spot or center of the test bar. Set a zero on the indicator and zero set Y axis. Now, move Y axis up approx 4. " to clear the indicator and rotate the table (B Axis) 180 degrees. Now bring Y axis back to the zero position. The indicator should be at zero. If not, use the resolver and or the offset in the grid to remove half of the error.
Repeat as necessary to obtain a zero zero condition.
This zero zero condition ensures the center of travel of X axis is aligned with the centerline of the spindle.
This "zero" on the indicator is located 1.000" from the center line of the spindle.
Now, move Y axis up to clear the indicator and rotate the table "B axis" to 090 degrees or so the indicator is pointed at the end of the test. Bring Y axis back to close to your set zero and increment in until the indicator goes back to zero.
The control should be at even inches at this time. For example, Z XX.0000".
Notice I did tell you the full inch dimension, I do not know the pramaters of your machine. I'm only interested in Z axis position at this time.
If the Z axis is off by some dimension adjust to remove 100% of the error.
If you want to go one step further, use a 4.0000" Jo block, and a mag base indicator. Set a zero on the top of the jo block and then move the test bar under the indicator. The highest point of the test bar (12 o clock) should make the indicator go to zero and the control should say Y XX.0000". Adjust as necessary and remove all of the error.
This procedure sets up all of the home positions for X, Y and Z axes.

This is all from memory but I believe it is right.
Why is this necessary? This is so every one, the programmer, the operator, the tool setter the inspector are talking out of the same book and making the same measurments and changes.
Maybe some one knows how to set home positions on a vertical.
I would think a test bar, known tool length and a 4.0000" jo block would be a good place to start.
Regards. Walt

PS: This takes longer to type it than it takes to do it......

Dear Walt, Hu

What you are all explaining works well.


Here the point is for precise measurment of Tool Length & Dia., a Tool Pre-setter is required (when the shop has multiple machines).

After visiting several companies as a service engineer, I have realised that any given procedure works for a shop. The important thing is, the CAD/CAM Programmer, Operator, Tool Setter etc. all speak same language (they all follow one set of methods).