Today I am trying to load, understand and use the tool table on my lathe. I have a 6 position turret tool changer
   I loaded 3 tools, a .375 Drill as the Master Tool, a left hand turning tool as #4 and a small boring bar as tool 6. No reason for this arrangement other than using the longest tool as the Master and starting somewhere.
I went thru the procedure as closely as I could like chapter 7 states in the manual. Though looking back thru my tool table editor the only thing I see is the tool number and name. It sounds like I missed something to set and or save the offsets on tools 4 & 6 and the master tool has no offset (at least that is the way I understood it). The tool offests numbers really confuse me for some reason.
   When calling for tool 1 in the MDi line I just say T1 00 or T4 00. So far I have never followed the tool number with any positive number (though it is my understanding there are 256 offsets available, why I dont know but that is another day). I see some refer to it as T101 (tool 1 offset 1?) I am supposing T1001 would be tool 10 offset 1? Anyway I am guessing upon start up each day or job beginning you home your machine, in my case I do have limit/home switches on both axis' farthest from the chuck. I would think I would physically touch tool 1(Master) to the Z face and touch part 0. At this point all other tools in the turret are a known distance from the master, correct? How do I call out tool 4 to touch the face of Z on the same part? If I simply type in T4 00 in the MDI line the tool changes fine but no G##  I typed in would command a move. Seems really odd to me. I am really just trying to verify that i could touch a part and visualize the concept. Smids book is a little over my head so far. Any tips or help would be great!  

The following should help you out. Just understand that no switches are being used and that it is written for a tool holder but the basics are the same.
If you want more detail about homing and the tool table then have a look at Appendix "F" in the LazyTurn manual which can be found in Members Docs.
Surely others will chime in as they use a turret.

RICH
 

I dont use the standard lathe screenset so my methods are likely different but heres a few pointers.
First you need to understand that the tool table is really an offset table in Turn and you actually only have 99 offset numbers even though the tooltable shows 254.
The reason you only have 99 is because of the way tools are called in Turn, TXXYY where X is the tool number or slot of turret and YY is the offset for that tool. For instance if you called T0101 or T0201 it would use the offset number you have in 01 in the tool table. That is not practical really unless you had two identical tools in two different slots and had them set exactly the same (almost impossible) So as you can see you can only have a 2 digit tool number and a 2 digit offset number thus the max of 99 offsets available.
Not read Richs manual but likely it covers the setting of tools but if you dont follow shout back and I am sure you will get more help.
Hood

Feel free to ask questions on anything in Appendix "F" or better yet just tell me that something is not clear.
In the quickie i don't go into any detail where the appendix does.  The problem with automating the turning of a part is that one needs to understand
setup, the coordinate system, the Gcodes, and how they all relate to one another. That is a lot of info and it's very easy to get confused.

RICH

 

Rich, Confusion is a good word to use in this arena. There is an incredible amount to learn and having a strong mathematical background would have been nice too. When I started to read the first page of the link you gave me, 1 of the first screens was to check the persistent tool offset. I was sure this forgotten unfortunately all were checked. Anyway I went thru the process of loading a few tools however since my machine does have limit/home switches I modified it a little bit. I already have my toolchange occurring at a predetermined spot so I also used that for my zero world location (the location where the tool 0 was being set up). I then proceeded thru the 3 tools. Then I touched Z of my part (scrap in the spindle with a face and diameter) with my Master tool (1) and pressed part zero with 0 in the dro. I then homed the machine and entered T100 the correct tool was loaded (actually just verified as it was already in the right postion. I then entered G54 Z0 X0 F2. Tool 1 proceeded to part x0 Y0 perfectly though there are a few questions (I get a totally different feedrate depending on the tool chosen even though F2 was requested). On to other misunderstandings. I then pressed home all again. Machine homed fine. I then entered T400, (here is where I believe my first error was, no offset) tool 4 moved into the correct location in the turret and it appeared to be in the correct location in X but Z was the same distance away as the master tool was. I then had an epiphany (after I had shut everything down and was laying in bed) that because I didnt ask for any offset, it didnt give me any. My thought now is that had I specified T404 it would have gone to the correct location or T401 still not sure of which one but I will try them both this morning. Thank you both as always for your input. It is  privilege to be able to receive the professional advice I get here.

So I tried T401 and T404 trying to see if there was a difference in how far it was away from the part I zeroed on using the master tool. I am missing something as all of the tools are the same distance away as the tool 1 (in Z). Though tool 1 hits Z0 X0 perfectly but my offsets from that tool must be wrong (easy to understand how that could have happened). I would have expected the error in X (due to the battle between radius and diameter) but not the Z. What amazes me the most is how you can write the manual so well and in an orderly manner (btw, this doesnt mean I understand it but that is my fault). I cant even conceptualize most of it. As you can see, order is not my strong suit.

Ok heres is what I would do if I didnt have home switches.
Move tool 1 and take a cut and measure the Dia and set that for the X DRO, next take a facing cut and set the Z DRO as zero. Now call a new tool, say tool 2. Move so the tool touches off the dia of the stock you have just cut, enter the size that it is into the X DRO for the Part Zero then press the Part Zero X button, you should now see that the actual X DRO has changed to that diameter. Do the same for the Z, move the tool until it touches the end of the stock, enter 0 into the Part Zero DRO for Z and press Part Zero button.
Repeat these steps for each tool, once you have done all tools you are best to open the tool table and apply. When you look in the tool table you should see offsets for X and Z for all tools you have set up except Tool 1, it should not have any offsets. That means each tool is set with reference to Tool 1.

Then to test just MDI each tool and you should see the X and Z DROs change to show the relative position of each tool.

I think I have the right buttons and DROs, reason I am not 100% certain is I have my own screenset and I have named the buttons differently.
Hood

Is there any reason why everyone keeps suggesting what to do "if I didnt have home switches"? I do have limit switches at the positive ends of travel in both axis and they are extremely repeatable according to my indicator. They are both used as home switches also and use different pins in Mach. Otherwise I will follow the advice as all my attempts above have not yielded me the results I was anticipating.

My appologies, skimmed through and thought you said you didnt have but see now you do.
Ok then what to do is have your X  home position as your "Master Tool", when you home set X DRO to  zero and then call Tool1 and do as mentioned above taking a cut and measuring the dia of that cut and enter that for the Part Zero DRO for X and press the X Part Zero  button. That will set an offset for tool 1 on the X in relation to your X Home switch. Z I wouldnt bother with as you set the Z DRO each time you put in a new piece of stock so if you leave Tool 1 Offset for Z in tool table as 0 then all other tools will be offset in relation to that. So face and set Z DRO sero then move on to setting the other tools as described.
Hood

Hood, A few more questions if you dont mind. Can I use the tool change location as the master tool home ? (this is off of the limit/home switch on both axis by approx 1/4" and set in my tool change macro). In your example the master tool is 0. All other tools are offset from that? If I use all 6 holders in my turret, should I label and call the offset by the same number as the tool number? ie T101, T202, T303 etc? as they all have different lengths and distances from the changer? If I asked for tool 4 as in T401, tool 4 would load but would be using the offsets of tool 1, wouldnt it? Which if it was my longest tool for example (a long drill bit, longer than any other tool in the turret) but tool 4 was a left hand turning tool, wouldnt I end up with the turning tool the length of the drill bit (or the drill bit minus the turning tools projection in Z) away from the piece/stock? Damn, I cant even ask the question coherently.