I have been loosing my mind trying to get Mach3 to run a lathe program as I intend it to.

Some basics-

Retrofit Hardinge CHNC1 running steppers, SmoothStepper, G203V's.
No toolchanger. Running Gang tooling on a tooling bar at 1.000" centers (Omni turn style)


I have the gang tool bar set up like this-

1st position. master tool holder. tool 1.
2nd position. NO TOOL. BLANK.
3rd position. tool number 2.
4th position. tool number 3.
5th position. tool number 4.

NOTE: 1st position is closest to operator.


I have a relatively simple file I created in BobCad ver 25 lathe that has the following-

1 spot drill op. done with tool 2, a spot drill in the 3rd bar hole.
1 through drill op. done with tool 3, a jobber length drill in the 4th bar hole.
1 roughing/finishing profile op. done with tool 1, a cutoff style tool in the 1st (master tool) bar hole.
1 cutoff op. also done with tool 1.
1 chamfer in prep for bar pull, done with tool 1 also.
1 bar pull done with a puller, tool 4, in 5th bar hole.
Loop.

I know that my locations of tools 2,3 & 4 are 1 inch apart from each other and they are tools that do not use an X offset (because they are drills and a bar puller.)
I know that tool 1 (master tool) is not on a center and is at an arbritrary place.

If my stock is .5" dia, and I want to setup the master tool, and then the others how do I go about this?

I have RTFM like 10 times and have been trying things for hours...

I suspect that this is all so much simpler than it seems. but with several diff coordinate systems, offsets, touch offs, entering cut diameters in the X axis DRO, Etc. I am so confused...

Can someone lay it out from start to finish?

Note-
I have used G52 to run this part in the past, but I think this is less than ideal on a ton of levels. for instance- wear offsets. also- I am calling a tool, but not really. more like I pretend to call a tool and just shift the part location. Seems wrong to do that.

I never use work offsets (other than the G54 ) as I have never seen a need.
My lathe screen is totally different from the standard lathe screen but here is what I do.
I home the machine then call Tool 1
I then move tool 1 in to take a light cut and just before the cut I zero the X DRO or set it to close to what I think the Dia will be.  This is so I can MDI the cut, move out on X then clear on Z and back in to X again. I then measure the Dia and on then enter that number in the (What the standard screen calls) Part Zero Coords DRO. I then press Touch X button and you should see the X DRO reflect that your tool is at that Dia. It is best to then open the tool table press apply then exit, (my Touch X and Z buttons automatically open the table for me)
Next do the same with the Z, ie  move to just negative of the end of stock and  zero the Z Dro then take a light cut, no need to touch off Z for this one.
Now jog away and call Tool 2, repeat as above for X or alternatively just use a feeler to touch off on Dia, enter the Dia in the X part zero coords DRO (remembering to add feeler thickness to  Dia, 2x feeler thickness if in Dia mode)  Then as above press Touch X, open Tool table and save. Next move Z to touch end of stock, enter  zero in the Z Part Zero DRO (or if using a feeler enter the thickness of it) and then press Touch Z, open table and apply.
Repeat for the rest of your tools, remembering to call a new tool before you set it up.

The above assumes you have accurate home switches if you are wanting to start your machine and know the tools wil be the same position as the previous day.

For doing the actual touch offs I have made up a tool for the chuck that I can take a light skim cut of with tool 1 then any other tools I want to set I just move to touch off dia and end and a LED tells me when I am there and I can then set the tools as above. Its just a bit easier than the feeler method, especially as my tools are at the rear of the work and the lathe is big so I cant really see where the tools are in relation to the work.
Hood

Just to add for drills etc you can use the same method for X by touching off the dia but you have to remember to take the half the drills Dia into your value for the X Part Zero DRO value.
Hood

Just a quick comment nateforeg,
Do exactly what Hood said and do it three times correctly (to form a habit of doing it right). The problem is one is so focused on trying
to touch off the tool that that you forget to call a different tool or click on one of the buttons, etc and
don't realise it.
RICH

If Lupe parked on the 50 yard line. Never mind I didn't understand it either when setting it up the first time. I am still vague though I do get it right eventually. IIRC don't you use the "ref" for the first or master tool and then just save for all the rest of the tools?

It can be done all sorts of ways and depends on whether you have accurate home switches or not or even none.
I tend to have Tool 1 with zero offsets and I have a Home Off value in my homing and limits page for the X which will represent the Dia that Tool 1 is when homed.
Another option is like I describe above, setting an X offset for Tool 1 which is an offset referenced to your home position.
There are many more ways but that is the easiest two ways in my mind.
Hood

Hey Nate, see if this helps http://www.cjh.com.au/Gang%20Tool%20Block%20Offsets%20for%20CNC%20Lathes%20under%20Mach3%20Control.pdf  Kind Mr. Chris Humphris did a fantastic job of documenting the process that works for him.

I'm getting close to setting tool tables up on my ORAC retro and RTFM'ing and searching on the forum still has me dazed.  I printed the sections in the manual that deal with homing & tool tables/offsets and I read it during lunch at work almost every day.  I guess I'll try wadding the pages up and eating them next.  Maybe that'll work.

DB-

Thats actually the way I have run the prog in the past. It works, but is not simple and I imagine that it should be easier to just use mach 3 tool offsets as designed.

I never could figure out why my G52 offsets ended up being ~1.9 inches away from each other per tool, when the tool block is on 1" centers. Never made any sense....

Also, I should add that I am not running limit switches.

I don't have homing/limit switches on my other little lathe and grew tired of having to constantly reset the X-axis zero point and get it to cut consistent diameters without fiddling around a lot.

I spent the nec. time to install & config opto sensors on X & Y on the ORAC and am real happy with the repeatability of referencing on the X-axis now.  It's worth the time & effort in the long run to know that it's going to cut the same dia. with the same tool each time I turn it on & re-reference it.