Hello Guest it is November 13, 2019, 03:22:49 AM

Author Topic: Turn Z part offset  (Read 4723 times)

0 Members and 1 Guest are viewing this topic.

Offline drew

*
  •  79 79
    • View Profile
Turn Z part offset
« on: September 19, 2008, 10:05:15 PM »
Since using M3 turn I have just reset my tools z axis offset to the current part's face.
What I haven't seen is if I can set my z axis offsets to a fixed point , then adjust an offset that would move all the tools to the part's face.
That offset would be the distance from my fixed point to the part's face. Have I just missed this or is it not in Mach.
Thanks Drew
If I had something important to say it would be here.

Offline DAlgie

*
  •  304 304
    • View Profile
    • Algie Composite Aircraft
Re: Turn Z part offset
« Reply #1 on: September 20, 2008, 01:29:41 AM »
Set your tool number 1 to X0 Z0 first. Put a piece of stock in the chuck and take a facing cut off it. Without moving the tool away, set the Z part offset, on the manual screen, to 0.00 and click Z offset. Next take a cut off the diameter, and without moving the X axis, you can jog back in the Z however, measure the diameter of the cut and put that amount in the X part offset box. Then click the X part offset button, it should now show the main DRO to the same diameter as the measured part. If you have a quick change toolpost you can now set all your tools using this part as your reference.
   DaveA.

Offline drew

*
  •  79 79
    • View Profile
Re: Turn Z part offset
« Reply #2 on: September 21, 2008, 07:02:43 PM »
Thanks Dave, But I know how to set tool offsets to any part. What I want to do is set the tool offsets once then only have to ajust one Z offset for all tools for parts that stick out the chuck longer or shorter lengths. Like a Work offset on my fanuc lathe.
Machine pictures at http://www.machsupport.com/forum/index.php/topic,4618.0.html
Thanks Drew
If I had something important to say it would be here.

Offline DAlgie

*
  •  304 304
    • View Profile
    • Algie Composite Aircraft
Re: Turn Z part offset
« Reply #3 on: September 21, 2008, 07:22:49 PM »
Just trying to help, but the way I described works, and will do what you want I think, unless I'm missing the big picture here somehow.

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Turn Z part offset
« Reply #4 on: September 22, 2008, 05:03:28 AM »
Yes what Dave is describing is exactly what you seem to want. One tool set as Master and all other tools offset from that tool. That means you only need to tell the machine where the zero position of the Z is and all tools will be at the same Z zero. (same for X of ccourse)

Hood

Offline drew

*
  •  79 79
    • View Profile
Re: Turn Z part offset
« Reply #5 on: September 22, 2008, 10:17:25 AM »
I dont seem to be explaning what I want to do very well. Lets say I set my tools to a part that is sticking out the chuck 2 inchs , run that part and replace it with a part that sticks out 2.75 inches. Is there an Z offset that that I can enter the 0.75 inch in to have all the tools 'see' the new face of the part ?
Thanks Drew 
If I had something important to say it would be here.

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Turn Z part offset
« Reply #6 on: September 22, 2008, 10:25:44 AM »
You could just type it into your Z DRO, eg if you had a piece that was 0.75 further  out and your Z was presently reading 2 in the DRO just type 1.25 into the DRO
 If the lengths were always the same or a few different then you could make buttons up to add or subtract from the present position and  enter it into the DRO.
Hood
Re: Turn Z part offset
« Reply #7 on: September 23, 2008, 03:31:32 AM »
You could use MDI and type G55 to get new work offset active.
In turn screens do not have work offset button to be able manualy edit work offset register like mill, but you could change active offset register using MDI.

When you start Mach it have G54 offset active and first you set your master tool X0 Z0
Next ghange G55 active and reset X0
Change back G54 active and move X to safe to avoid collisions
Make move you want to be your next location eg. Z-0,75
Change G55 active and reset Z0
Now you have two different work offset you can change in program using G54 and G55.
I think in Mach you can have 255 different work offset if you want from G54 to G59 and G59P1 to G59P254

Regards Mstcnc

Offline jimpinder

*
  •  1,233 1,233
  • Wakefield, West Yorks, UK
    • View Profile
Re: Turn Z part offset
« Reply #8 on: September 23, 2008, 06:13:18 AM »
As the last post said, it is all to do with offsets.

You do not mention a home position, and this is what you must establish first. You then home your lathe. Mach 3 then knows where it is and zero's the Machine Co-ordinates DRO's. Your home position should be established with switches (preferred) or a position to which you can return, time and time again, with absolute accuracy.

Using your selected method, create your tool table.

So you now have a home position, and the tool offset table. The tool offset table is an offset from an as yet unknown position of the lathe, and what remains to be done is  set that position.

If I want, therefore, to set an accurate offset, my X offset is 3.6267 to the lathe centre.  The Z offset varies as to how you write your program and where the Z position 0 is. It is usually, but not always, at the start face of the barstock.

If you were doing a large number of units, then I would use the HomeOff facility when homing, to zero the lathe at a position level with the face of the chuck. My offset would, therefore be how much the barstock stuck out of the chuck, or I would write my program so that it measured from the face of the chuck too, and there would not be an offset.

However you arrive at where to set the Z0 position, it depends on choice - your choice, and there are pro's and con's on either side.
Depending on the job it might vary. This is where the offset table comes in and you can enter the appropriate offset in the offset tables, using G55 to G58 and G59.7 to G59.255  - and use the offset for a particular program. Enter your x offset - usually to the centre of the lathe, then calculate your z offset from your home position.

Start up - home the table - and run the program. Provided you have accurately written the  tool changes, your machine will start up, and move to the correct position for that program and that tool.

It sounds a bit complicated but the rule is - the machine must always know where it is BEFORE you do anything.
1. Establsh a home position, either with switches (prefered) or a position to which you can return time and time again with accuracy.
2. Establish a 0,0 position from which all tools can be measured.
3. Calculate the correct offset for running the program - i.e. know the offsets from your "home" position to the 0.0 in your program






















« Last Edit: September 23, 2008, 06:25:05 AM by jimpinder »
Not me driving the engine - I'm better looking.