Sorry forgot you worked in Rad mode, have never seen the attraction to rad mode but some seem to prefer it, personally I think its much easier working in Dia.

Not understanding what you are meaning by setting the offsets in Dolphin, how are you doing that?

What normally you do is have Mach take care of offsets by having them in the tool table and the CAM basically produces code to cut at whatever radius/dia you tell it.
So what you do is have one tool as master and zero the Z on the end of the stock or maybe  set it positive by the amount you will be facing off. The tool is then placed against the OD or you can take a light cut and measure the OD and you enter half that value into the X DRO (1/2 because you are in Rad mode) That is now your master tool set, no offsets in the table but work offsets. Next you change tool with the Taabb call and then move the tool to the same as before and then the difference from the master tool is entered into the tool table for the new tools X and Z, then next tool etc.

In the end your tool table has no offsets for master but offsets for the other so no matter which tool you call if you command it to move to Z0 it will go there, same for X values commanded.

Hood

Just had another look at your CNC file and it seems like it may be in Dia mode in Dolphin, could that be your problem? I am not 100% sure if it is definitely Dia mode though as it may just be my setup here that changes it to Dia mode as that is what I have Dolphin set as default for and maybe its changed your file when I opened it.
Hood

I did have both in radius. Tried Diameter too without a lot of success. Here is a screen shot of the tool offsets in DT.

Ah Ok thats your problem then, dont enter any offsets there as you want Mach to handle the offsets in the tool table.
Hood

Hi All,

I have been following this thread for a few day now.  I gave up using Tool Tables for Gang Tooling in CNC lathes controlled by Mach3.  I now use G52 Offsets for all tools in the Gang setup.

Here is my experience and solution to the problem. 

http://www.cjh.com.au/Gang%20Tool%20Block%20Offsets%20for%20CNC%20Lathes%20under%20Mach3%20Control.pdf

Regards

Chrisjh

Chris,
 I use the tool tables in Mach for my lathe which has a front and rear turret and dont have any issues at all. There is one thing you have to make sure of and that is you have ALL tools set up as either Front or Rear in the Tooltable. Having a mixture of both is a disaster and will lead to all sorts of problems. Because my default turret is the rear I have mine all set as rear, even the ones on the front turret. That means the X axis moves positive when its moving away from the operator so any tools I have on the front turret need to be programmed with negative X values and also when entering values in the tool table you need to remember to enter the negative diameters into the DROs before sending them to the tool table. I have attached a screenshot of the DROs for entering the values and the buttons that then enter these into the tooltable (first is my screen, second is standard but both are the same DROs and Buttons). So what I would do is for example if a tool is in the rear turret I move the tool to the dia of the stock and enter that into the X Val DRO and then press Set X button ( Part Zero X button on standard) and that will put the offsets in the tooltable. Now if I have a new tool and its on the front turret if I touch off the Dia it is past the zero point of my axis so its X values are now shown as negative. I again touch off the Dia as before but this time the value entered into the DRO would be a negative value.

It works extremely well for me with my quite complicated setup and I see no reason it would not work on a gang tooled lathe as long as you remember that in the tool table  all tools need to be either Front or Rear but never a mixture. Your method obviously also works for you.

Hood

Thanks a bunch, Guys. I really like that tool setup. Looks like it works out great.

There is obviously more than one way to wrestle this mule. I have tried every different configuration possibility at this point between M3T and DT.  I am spoiled about the dro's showing me the exact values of where the tools are in relation to the spindle. I guess that is because I hand coded these before, so it is a simple matter to get my mind around that concept.

The two programs were competing against each other and cancelling or doubling offset values depending on how it was setup. Of the two modes, radius seems to allow the dro's to follow exactly along with offsets when they are programmed in DT. This doesn't happen in M3T. What happens there is it goes into machine coordinates. It just posts the opposite of your offset and then travels to 0 in the dro, which is your offset. This makes it more difficult for me to dress up the gcode as output by DT.
It does need some dressing too. It overtravels back to home too often. It doesn't allow single axis moves with each type of operation. It does for some, but not all.

Sooo.....the best for me is not tool offsets in Mach. Load them in DT instead. Keeps dro's in the actual program coordinates. That is a single system and easy to keep track of and recognize what it's doing at any given time.

These are production parts, so these offsets won't really change.
I'll always just reset them there.

I'll snap a few pictures of the gang setup now.
It is similar to what I had before, but now the drills are on one plate and have collets for changing drills.
I do use boring bars sometimes, but they go in the QCTP instead of a collet.

That is the best thing about Mach3. There are so many ways to do something with it that you are bound to find one that works for what you want to do.

Hi Hood,
I took your experienced advice ages ago and setup using one tool post only.  In my case, I selected the front tool post option, so tools that cut from the rear side have negative values of X whilst tools that cut on the operator side operate in positive values of X.

Using the Tool Table and calling individual tools works fine with Mach3. However it was not suitable for my gang setup (and I suspect most gang tool setups).  The problem I had in the gang setup was, when a tool whose centreline was located, say, 100mm from the Master Tool position was selected, the cross slide would try to travel to a position beyond the X+ limits before returning to the correct position.
 
I proved that Mach 3 Tool Table calls worked OK with a tool whose centreline displacement from the Master Tool was 40mm.  When this tool was called from the Tool Table, the initial travel from the Master Tool Position was towards the operator (positive X direction), then return to the correct position 40mm (in a negative X direction away from the operator) from the Master Tool position.  The first movement stopped just short of the X+ Limit Switch.  Any other tools greater than 40mm from the Master Tool simply tripped the limit switch on the first, unnecessary excursion.

I suspect that double movement I was witnessing has something to do with the maths algorithm within Mach3.  Because I couldn’t do anything about the algorithm, I had to seek an alternative solution.
The total Cross Slide travel between limit switches in my setup is approximately175mm so I have work within these limits.

You are correct in that there are many ways to skin a cat.  This Mach3 journey, for me, has been long and rewarding.  Still learning and trying pass on my experience in this fascinating hobby.

Leeway,
 
It was one of your YouTube videos that got me started down the gang tool setup path.  I thank you for these videos. Love the Pink Panther!! (Still in my favourites).

Here is one for you.  http://www.youtube.com/watch?v=gsw5JtYMGSI&feature=mfu_in_order&list=UL

Regards
Chrisjh

However it was not suitable for my gang setup (and I suspect most gang tool setups).  The problem I had in the gang setup was, when a tool whose centreline was located, say, 100mm from the Master Tool position was selected, the cross slide would try to travel to a position beyond the X+ limits before returning to the correct position.
Regards
Chrisjh

I do not understand this bit at all, you are saying when you called a tool it would go off before coming back? If so then were you using a toolchange position from within the m6 macro?

I can call any tool I like and the axis will never move unless commanded, the DROs will change to show the position of the tool but no motion at all until I command a move.
Hood

Hi Hood,

Attached is a diagram showing examples of how the tools move from one position to the next when called from the Tool Table.

The other drawback is that CSS was also affected because Mach3 thinks that the new Position of the tool is at a much larger diameter, so the spindle rotates at minimum speed.  That is, it appears to behave like the job is larger in diameter by a factor of the tool offset distance.

Its been quite a while since I witnessed all this so my recollection is sketchy.  I think I recall seeing the X DRO indicating the larger diameter. I suspect that this is because Mach3 thinks that the job is bigger in diameter that it really is when a tool with an X position greater than the Master Tool.

Regards

Chrisjh