Nice to see that the forum is updated

Unfortunately the Mach3Turn tool offsets are still making me crazy. I have searched for movies on Youtube but still I can`t get it done. I suppose there are already a lot of topics about it but I can`t find them.

I am using a tool changer turret  and Mach3 is showing me the correct tool numbers (most of the times). The macro for the tool changer needs some more attention but I don`t think it has something to do with the offset problem.

When I try to set up the offsets in the tool table I am using Tool number one as the master tool. I zero the dro and for the upcoming numbers/tools I use the part button. Still it doesnt work. For example, when I try to set my offsets for tool number 2, the offsets are writen in the offset box for tool number 1. I don`t think that is correct.

Is there somebody who can give me a link from a good video or a topic that explains it well?

There are a few different ways to touch off the tools to populate the tool table.
I would strongly recomend that you use probing for touching off the tools.
To each their owne...........

The master tool concept is used. I use tool #1 as the master tool and it has no offset values and is not used to machine with. Tool #1 and tool #0 both have no tool offset.Understand that all the tools relate to the master tool and all the tools relate to each other! Tool # 0 offset is zero and can't be changed in the table. SO using tool "0" you can move to a reference location anywhere and touch off to a surface, and define that point  in Machine Coordinates as zero. Don't have any work offset / G52 / G92  offsets in affect when doing this. You are using  Machine Coordinates as a way to measure the touch off distance difference between the different tools. You should be  be in radius mode/absolute modes as all the offset values in the tool table are in terms of radii.

When doing the above once, the master tool has been touched off, you simply move the controlled point anywhere, change the tool, and touch off to the reference surface, continuing on until all the tools have been touched off. Said differently , a point you are at is a location which is defined as zero, any movement away from that point is tracked constantly, you move back with a different length tool and the dro shows the difference in length of a different tool when it touches the zero point.

FWIW, I can probe 20 tools and populate the tool table in 15 to 20 minutes and accuracy / repeatability is +- 0.0002".

RICH

How are you sensing the tool position?  I have a tool setter which is a bar with an accurately known diameter that is mounted in the lathe taper.  I have a touch sensor that detects when the tool touches this, controlled by a macro run from an "offsets" screen.  The macro can move the tool in both X and Z.  Tool 1 is in effect a master tool but can also be a real turning tool.  To use the macro, I just enter the tool number in a DRO, job the tool to within 2 mm of the X or Z position, and click on a button.  The macro moves the tool slowly until it touches, takes 3 touch measurements, calculates the offset, and writes it to the tool table.  IIRC one button for the X offset and one for the Z, as the start positions are slightly different.  You also have to enter the setter diameter, which you make negative for boring tools and put the tool behind the setter.  Happy to let you have a copy of the macros and screen (if I knew how to do that!).  Also I home the X axis at the start of every turning session to a known machine zero - that's why I can use tool 1 as a real tool.

John,
I use probing for touching off  "ALL"  tools and use a simple tool setter.  Find that it is the most accurate and repeatable of all the methods. I do not double probe the touch off but rather probe at  a slow rate eliminating the over travel. I use a few macro's but the button scripting takes care of what is needed to be done.
 
By "ALL" tools I am meaning things like reamers, drills, whatever and a few buttons provide for any changes required. To touch off any lathe tool you need 4 surfaces / references when probing.

I use the master tool concept such that tool one is used to define all the other tools. It is not used for machining and it is just a piece of 1/2 round carbide and the sides are parrel and the face  is perpendicular to the sides. Once the tool table is populated any tool can become the master tool. If tool #1 is broke and needs to be replaced then you can use say tool 10 to replace tool #1 with the proper offset.

My tool setter is home made and cheap! Simply it is a piece of ground round with a 1" micrometer standard on the end of it. The mike standard is mounted on the end of the round, centered and the flat surfaces parrel to the round.

I just put electrical tape on the round so i can probe to any of the mike standards four surfaces.
Now you say .....tape on the ground round and he is accurately finding offsets.....I hear it now...give me a break, Rich!
It matters not what is holding the tool setter, you must center it using an indicator 0.0001". The tool setter just provides a common reference X Z plane for the tool  to touch off. You need that to have "0" runout in the X direction and the plane can be slightly above or below lathe center. My three jaw creates a small runout on the tool setter, so it's easy to center the setter on lathe center.

BTW, I don't use home swiches, always start by using the tool setter to find lathe X center via probing. Then manually define a  home and tool change location and both are at the same location (KISS). Then define the G54 Work offset. I use a quick change and probably the most number of tools used in one machining operating was around 8 tools or so.
 
RICH

I did a couple of videos showing two methods of basic set up of tools in Turn, they are

Without home switches

https://www.youtube.com/watch?v=mWnfioI3G0E

and with home switches

https://www.youtube.com/watch?v=Kla1sZ8IF6k

Thanks for the anwsers, I was a few weeks on vacation so because of that my late respons.

My tool setup, already have shortened the tools. For touching off the tools I am using a 45mm bar.



I use my machine zero point for T0. I want to use T1 master tool just as my tool number one, possible or not?

For touching off the tools I just bring the tool to position and click on touch X or Z. Still the values doesnt make any sense after I have done that.



Just tried to touch off T1 and T2





Probably I am still doing something wrong but it is getting super annoying. Is it because T1 is not allowed to use as usable tool?

I have sent you a PM.

Tweakie.