Hello Guest it is August 08, 2020, 02:18:24 AM

Author Topic: Mach 3 lathe home input  (Read 1605 times)

0 Members and 1 Guest are viewing this topic.

Offline RICH

*
  • *
  •  7,411 7,411
    • View Profile
Re: Mach 3 lathe home input
« Reply #10 on: March 04, 2018, 08:41:52 AM »
John,
Yes they are correct and what I use.

RICH
Re: Mach 3 lathe home input
« Reply #11 on: March 04, 2018, 08:49:09 AM »
Thanks Rich!
Re: Mach 3 lathe home input
« Reply #12 on: March 08, 2018, 04:27:36 PM »
OK, well I'm making progress but in fits and starts!  My probe hardware is operating, I have modified the "tool table" screen of the standard turn screen set to add some buttons to activate the probe and written some probe macros as button scripts.  I'm getting some very puzzling results, so I was wondering if I could just check a couple of points with you please Rich?

1. In a few places I have seen references to an M40 macro and that it needs to be activated to open a point file for the vars - on the other hand all the working probe macros I use on my mill don't use it.  So am I correct to ignore M40?

2. I'm trying to operate only in machine coordinates for this exercise, but I read somewhere that G31 operates in work coordinates - is this correct?  I'm getting some very anomalous behavior which I can only think is because there is some offset coming in that I don't understand.  

I'm sure there's more I don't understand but I don't know it yet!

Thanks, John.

Offline RICH

*
  • *
  •  7,411 7,411
    • View Profile
Re: Mach 3 lathe home input
« Reply #13 on: March 09, 2018, 06:02:23 AM »
Suggest you consider the followong:
1. Understand the master tool concept for populating the tool table.
    The master tool is used to set a reference point and all the other tools offsets are based        
   on the master tool.  All the tools are related to each other.
2. Understand the difference between Machine, Part, and Program Coordinates.
    Machine Coordinates are absolute values and X values are in terms of radii. Tool offsets      
   in the  lathe tool table are in terms of radii.
3. Know how Work Offsets offsets are created. Mach defaults to G54. For a rear toolpost
    the offset is G55.
4. Know how to set machine coordinates and work offstes to zero values.
5. Understand how G31 works. Then you decide how you want to use it.
6. Understand tip direction as it relates to tool touch off. Most gcode  from CAM are              
    pre-compensated. In probing of lathe tools you will need a four surface tool setter
     and even with that you will still need the ability to adjust the probed offset values for            
     some types of tools.  
7. Consider using a different screen set for the lathe.
    Have a look at this one and modify to suite your needs.
    http://www.machsupport.com/forum/index.php/topic,13548.msg88932.html#msg88932
    

I don't use the M40 macro but rather get the variable value created by G31 and directly set the current tools X or Z offset value.
 If you are collecting points that is a different story.
G31 works in Machine Cooordinates.

RICH
Re: Mach 3 lathe home input
« Reply #14 on: March 09, 2018, 07:24:44 AM »
Just an update - I think I've made a step forward, by defining my own DRO to which to write the probed value rather than trying to re-use the OEMDros 175 and 176; and also working in radius mode for the purpose of probing.  Essentially what I want to do initially is to be able to make tool offset measurements and manually populate the tool table until I understand how it all works!  Thanks for your advice above Rich.  Just a few comments...

1.  As far as I can tell from the documentation the Master Tool (No. 1) is assumed to have zero X and Z offsets.  When the work is mounted in the lathe you touch off end and periphery using the master, possibly turning a short section to get a concentric diameter first.  When you enter that diameter as an X coord for Tool 1 (when set to that diameter) then every other tool if put in the holder instead and selected would turn to the same diameter; and equivalently for Z.  What I'd like to do is to start by homing the machine as I have a pretty repeatable X home switch (<10 microns as far as I can tell), then use the offsets for all tools including Tool 1 to avoid the touching/turning step.

2.  I think I've got the coordinate systems straight and realised that radius mode is key for measuring offsets.

3.  I think I'm right in saying that for the lathe, only the Z offset is relevant?

4.  Documentation is a bit hazy on this but "Zero World" buttons zero the m/c coords?  For the work offsets you select work coordinates and zero the DRO?

5.  I'm fairly familiar with G31 as I've been probing on my mill for some time.

6.  Once I've made a test bar I will have in effect a 4 surface tool setter.  I'm finding the limits to the concentricity of the MT4 to MT2 adaptors for my Myford at the moment, so once the probing routines are working I have to make a test bar with a 4MT short taper on the end.

7.  I'll look again at that screen set - once I understand better what I'm doing!

Thanks again for all your help Rich.

Cheers, John.

Offline RICH

*
  • *
  •  7,411 7,411
    • View Profile
Re: Mach 3 lathe home input
« Reply #15 on: March 09, 2018, 11:28:57 PM »
Use MC's to measure but start measuring with MC's =0. So if you probe with a tool and have the probed value / variable put into DRO 108 or109 then that value is the offset from the master tool which will be put into the tool table and no need to populate it manualy. KISS / just a thought!

COMMENTS ON YOUR REPLY #14:
I don't use switches since they add no value for the way I work. Frankly I keep it simple
by having MC zero, home, and tool change location all set to MC's=0,0.   KISS!

1. Tool 0 has no offsets and you cannot change them. Tool 1 would be the master and it has no offsets but you can change them. Tool 0 comes in handy if you want to move around and not do something stupid to screw up the tool table or what ever.

3. No, both the X and Z tool offset is relative. I think you are thinking of work offsets and that would be basicly true since the lathe center is X = 0 and the Z value varies depending on where the end of the stock is located along the lathe bed. Usualy  lathe gcode is based on X and Z=0 and that is the end of the stock.

4. Zero world will zero the MC and also delete / set work offset to zero value.
  
5. Hmm....what is your probing feed rate and min travel distance you allow for when     probing ?

6. You need (4) surfaces to probe lathe tools easily, else a PITA. Also you will need to provide for easily probing  / changing a tools offset. ie; probe tip, drill , reamer. whatever!
A 1" standard for checking a micrometer mounted on a ground shaft is cheap, easy and
very accurate tool setter.

Have fun......,
RICH
« Last Edit: March 10, 2018, 07:17:06 AM by RICH »