Hello Guest it is January 19, 2020, 02:48:55 PM

Author Topic: In the Mach3Turn, how to get the lenght offset?  (Read 4682 times)

0 Members and 1 Guest are viewing this topic.

In the Mach3Turn, how to get the lenght offset?
« on: December 29, 2008, 07:44:29 PM »
Hi all,
    In the Mach3Turn, how to get the lenght offset number?
    In the code "T0102 M6",
    Tool = GetSelectedTool()    'Tool=1
    but the lenght offset number howto get??

thanks!
Edison

Edison

Offline DAlgie

*
  •  304 304
    • View Profile
    • Algie Composite Aircraft
Re: In the Mach3Turn, how to get the lenght offset?
« Reply #1 on: December 30, 2008, 01:25:10 AM »
In turn you set the tools on the tool offset page. There is no length really, just an X and a Z offset. Set tool 1 as your base tool, usually a roughing tool. In the part offset DRO set Z as 0.00, fit a piece of stock in the chuck and take a manual jog cut off the diameter, measure this and put that diameter in the part offset DRO for X. Remove this tool and fit the next one, I use T0202 as a profiling/ finishing tool. Click on the tool display number box and change that to tool 2, make sure you hit enter to accept it.  Jog this up to the material and just touch the OD of the material. Without moving the axis, go to the tool setting page and click the X Touch button, this will set the offset of that tool in the tool register. Do the same for the Z offset, touch the side of the tool on the end of the stock, etc. Generally you use 'T0101, T0202, which would be tool one, offset one, tool two, offset two. Don't mix them up by using T0102, etc or you are sure to end up with a crash. Mach turn really does have an excellent tool setting setup, much better than a lot of the high dollar Fanucs, etc.
   DaveA.
Re: In the Mach3Turn, how to get the lenght offset?
« Reply #2 on: December 30, 2008, 01:54:12 AM »
HI,DaveA,
    I used the AutoTool Change, in the macro how to  get offset number? As "T0101 M6" get the number "1".
    Or you has same idea to deal with the offset problem?
Thanks!!
Edison
« Last Edit: December 30, 2008, 01:57:14 AM by Edison »
Edison

Offline jimpinder

*
  •  1,233 1,233
  • Wakefield, West Yorks, UK
    • View Profile
Re: In the Mach3Turn, how to get the lenght offset?
« Reply #3 on: December 30, 2008, 04:34:53 AM »
In "Turn" you do not use M6 to get the offsets.

The "T" command is of two parts   eg. T0101 (unlike "Mill" which is T +tool number)

The first 2 digits are the tool number from your tool table, the second two digits are the offests (also from the table) . Therefore you could have say tool 6 with offset 2. Don't ask me why, I don't know, but I assume this means that on an auto tool setter, you can select a tool number, and if all the offsets are the same, you can just use the same offset.

As Dave says, it works very well, I have a drill post mounted on my cross slide, for centre drilling - the x offset is common at 3.6267 inches. The other offset varies with the length of the drill, which I have set so that it arrives 0.05 inches from the work piece. The only difficulty is making sure there is nothing in the way, so after the T0404 or whatever, I do seperate G0Z0 and G0X0 to move it into position.

Reading your posts again - are you asking where to put the offsets - the answer is to enter your tools in the tool table, with the offsets.
It helps, of course, if you have a quick change fitting or similar, so all your offsets are fixed, once set.

You should be able to locate your X0Z0 position on your lathe, which is usually X0 - lathe centre and Z0 face of the workpiece (or perhaps the chuck face, which I use, because it is a permanent fixture). Set your most used tool to that position and then set the DRO's to zero. Enter this first tool with zero's as the offsets. Set your other tools to the same position and note the offsets on the DRO's and enter them into the table.

If you now choose a tool, using T0303 (or whatever) then G0X0Z0  should move all the tools to the same position.

If you have "home" switches fitted. You home the machine. A G54 offset  then brings the machine to your normal X0 Z0 position, and your tool table takes care of the offset for all the tools. You can then write your GCode programs from the same "position" every time.

Jim







Not me driving the engine - I'm better looking.

Online Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: In the Mach3Turn, how to get the lenght offset?
« Reply #4 on: December 30, 2008, 05:51:32 AM »
Jim the reason you can have different offsets is on a lathe you normally haver a turret or toolpost which is automatic and as such you have limited positions available. Because the setup of tools in these are usually fairly accurate it means you can have all sorts of tools ready to pop into a slot and thus can call tool slot 2 with offset 2 or you could place another tool in that slot for a different job and you have the offset already set so you call tool2 offset 12.
 On my turret I have 6 slots and on the toolpost I have 4 so thats 10 in total, I have tools for each slot  and that is T0101, T0202.......T1010 I then have other tools that fit in these same slots so for instance I may have T0616, T0626, T0636 etc etc, that way the tool changer will rotate to the correct position and the correct offsets for that tool are applied.
 In Turn the T01,T02 etc dont have any reference to/in  the tooltable as the table is purely offset numbers.

Hood
 

Online Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: In the Mach3Turn, how to get the lenght offset?
« Reply #5 on: December 30, 2008, 05:53:01 AM »
Edison, are you asking how too get the tool that is already in position for your macro? If so then it is
GetCurrentTool()

Hood
« Last Edit: December 30, 2008, 10:10:41 AM by Hood »

Offline jimpinder

*
  •  1,233 1,233
  • Wakefield, West Yorks, UK
    • View Profile
Re: In the Mach3Turn, how to get the lenght offset?
« Reply #6 on: December 30, 2008, 09:58:42 AM »
I though that was the reason - I shall get an auto tool changer (eventually)
Not me driving the engine - I'm better looking.
Re: In the Mach3Turn, how to get the lenght offset?
« Reply #7 on: December 31, 2008, 01:42:58 AM »
Thank you for help, the problem was finally resolved.
In the origina, lathe where we do not need to control his tool offset, it can according to the code "T0102",
auto-correction tool on the 2nd offset. The M6 macro as like as two peas with the milling.
Edison
Re: In the Mach3Turn, how to get the lenght offset?
« Reply #8 on: December 31, 2008, 01:50:19 AM »
In order to help more people, I post my  auto tool changer code, hope you can help!



'** File Name:    M6Start.m1s
'** Created By:   Edison_Pan
'** Created date: 2008-12-1
'** Version: 1.0
'** Descriptions: First version

Option Explicit

'Declaraciones
Const   MaxToolNum = 4   'Max number of tools for the changer
Const   CCWTime    = 3
Const   ChangTime  = 10

Const   T1  = Input1
Const   T2  = Input2
Const   T3  = Input3
Const   T4  = Input4

Const   CW  = Output5
Const   CCW = Output6


Dim OldTool,Tool,NewTool
Dim Tim

OldTool = GetOEMDRO (1111)
Tool = GetSelectedTool()

If OldTool = Tool Then
Message ("Selected Tool already loaded")
Exit Sub
End If
While Tool > MaxToolNum
Tool = Question ("Tool Error, Tool number to large Enter new tool number")
Wend

Call StartTool
SetTimer(1)
While NewTool <> Tool
   Call CheckPins
   While IsMoving()
   Sleep(10)
   Wend
   Tim=GetTimer(1)
   If Tim > ChangTime Then
       DoOEMButton(156)
       DoOEMButton(1021)
       Message ("Tool Error,time out")
   Exit Sub
   End If
Wend

Call StopTool
Call SetUserDRO (1200, NewTool)
SetCurrentTool(NewTool)
'Code "G43 H" & NewTool       




'Subroutines
Sub StartTool
   ActivateSignal(CW)
      While IsMoving()
        Sleep(10)
      Wend
End Sub


Sub CheckPins
   If IsActive(T1) Then
      NewTool = 1
      End If
   If IsActive(T2) Then
      NewTool = 2
      End If
   If IsActive(T3) Then
      NewTool = 3
      End If
   If IsActive(T4) Then
      NewTool = 4
      End If
End Sub


Sub Stoptool
   DeActivateSignal(CW)'Stop the toolchange
      While IsMoving()
     Sleep(5)
      Wend
      Sleep(1000)
   ActivateSignal(CCW) 'Lock tool
      Code "G4 P" & CCWTime    'Lock time
      While IsMoving()
     Sleep(5)
      Wend
   DeActivateSignal(CCW)'Turn off the Lock
      While IsMoving()
     Sleep(5)
      Wend
End Sub         
Edison