[HalfRhoVSquared]

Not at shop so can't see machine but do I have to set work offset for every tool individually? So if I have 10 tools I have to go set the tool offset for each one and then have to set the work offset for each one? ( so have to set 20 things)

If so this doesn't make common sense because you should be able to go set all your tool offsets and then only have to set one work offset and it should remember all the other tool offsets and figure out where the tips of all the tools are relative to the work offset of the one tool that you had selected Whenever you set the work offset with that tool.

In short I want a simple and fast way to set the tool offsets with my 3.000 gauge and then my xyz work zero with my Heimer which is Tool 1.

I've looked all over for a video on this on YouTube etc but can't find anything for this old control.

[the_gentlegiant]

Not at shop so can't see machine but do I have to set work offset for every tool individually? So if I have 10 tools I have to go set the tool offset for each one and then have to set the work offset for each one? ( so have to set 20 things)

If so this doesn't make common sense because you should be able to go set all your tool offsets and then only have to set one work offset and it should remember all the other tool offsets and figure out where the tips of all the tools are relative to the work offset of the one tool that you had selected Whenever you set the work offset with that tool.

In short I want a simple and fast way to set the tool offsets with my 3.000 gauge and then my xyz work zero with my Heimer which is Tool 1.

I've looked all over for a video on this on YouTube etc but can't find anything for this old control.

Yes you set your offset for each tool. Read my last post carefully and you'll see I said nothing more or different then that. This tool setting all depends on how you're going to run your machine. If you're going to leave many or most of your tools loaded in the machine and change out only a few, you want to use what might be described as a Master System. In a system like that you have to have a repeatable place you can go to to measure your tools no matter what you have loaded vise or fixture wise on the table. Your 3" block sitting on the table is an example of that. If you plan on tearing down after each job (like I do, which isn't very common, but I have twenty year old tools that look like new.) you would instead use your 3" block on top of the actual work piece. This way you won't have to set any numbers in your "Shift" or G54-G59 Z areas, as all tool offsets will be referenced to the stock surface. Meaning stock surface is your current reference. CORRECTION: You will have to account for the 3"block. Otherwise your tools will al run 3" high above the part.

When measuring tools with your block you're entering the info (possibly using EOB / Z / Input) into the tool offset screen and looking at Z only. When using your Heimer and probing for part reference, you're looking for X and Y values to enter into the Work Coordinate areas of the control like G54-G59 and not worrying about the Z just yet.

As part of your Master System, you should also have a Z offset set or written down that you obtained off the same 3" block for your Heimer. Treat it as a another tool so to speak. Then at the beginning of each job, you measure the top of the stock with your Heimer, and enter the difference between that number (Machine Coordinate Screen Z value) and the previously measured height of the Heimer on the 3" block, (obtained again on the Machine coordinate screen Z value) into your G45 Z area, and any other Work Coordinate that you're using. If you're using all 6 offsets (G54-G59) it's simpler to enter the calculated Z offset height into the "Shift" register which should be right next to G54 somewhere. Anything entered there affects all Work Coordinates. You can even use the "Shift" register to correct things in X and Y also. Say you realized that shoot... I want to move all the programming 0.005" away from the fixed jaw in all the vises you have loaded. You could enter Y-0.005 in the Shift and it would move all your offsets (G54-G59) without having to change all of them individually.

To simplify. 3" block on table.

1) Measure all tools on block. Only needs to be done once. Look at Machine Coordinate screen and enter that Z value you find there into the corresponding area of the Offset screen. T1 into T1 (H1), T2 into T2(H2) and so on. Maybe put your Heimer offset in the highest number offset you have for safe keeping. Again you may be able to use EOB / Z / Input to enter your values instead of typing them in. (See earlier post)

2) Place 3" block on your work piece Z zero surface and measure its Z height with the Heimer. Take the number you find in the Machine Coordinate Z area and add or subtract that from what you have previously set/measured for you Heimer. More then likely you'll be looking for a positive number, because it's very likely that when you're measuring on top of your work piece you're higher up then when you measured on the table. But not always.

3) That number you now have that is staring at you from the calculator screen is the number you either put into the Z area of the "Shift" or Global Work Coordinate area, or... enter it into the Z area of any and all Work Coordinate Z areas you're using on the job. Again Work Coordinates refers to G54-G59.

Tools measured once. Work height measured for each new job and calculated difference enter as in 3) above.

Last paragraph deleted. See below.

[the_gentlegiant]

In closing. Keep in mind what I said in the first post about accounting for the 3" block. Until you get used to things, it's probably better to read the numbers on the screen directly and not account for the 3". As long as you do the same thing like using the 3" block for all measurements, you should be good.

I started new here to correct the above which is incorrect. You do need to account for the 3" block. Only in the sense that you don't use it when measuring the stock surface you want to use for your reference plain. Measure directly on the stock or part surface if possible. You can use your Heimer for this, or any tool for that matter. It will be easy to see if you want to enter a positive or negative number. Slide your 3" block up to your work piece. If the block is lower then your work you will enter a positive Z number. If the block is higher then your work you will be entering a negative Z number.

Basically all you are you're doing is telling the control what the Z height difference is between the master tool reference plain (3" block on table) and the actual part surface plain. That's what the control needs to know for every new job you put on the table.

Even if you break a tool in the middle of a job. As long as you measure the replacement tool on the 3" block as you did with all your other tools and enter its new value that you find on the Machine Position page, that new tool will go right back to machining at the correct height without changing any other numbers.

That statement tells why using the Machine Position (Coordinate) screen for all measurements is so important. Those numbers under every circumstance are always the machine's position relative to the machine's Home Position set by the Machine Tool Builder. They are untouchable. This is what makes them so safe to use. Unlike Actual and Relative Position screens which can in many circumstances become meaningless due to numbers entered elsewhere. Honestly in all my years of machining I've hardly ever looked at Actual and Relative positions anyway. Unless I'm bored and want something to watch just for the hell of it.

Hope this makes sense for you and helps you get going.