Hello Guest it is May 24, 2019, 10:04:39 AM

Author Topic: Question about rear-mounted lathe QCTP  (Read 1177 times)

0 Members and 1 Guest are viewing this topic.

Question about rear-mounted lathe QCTP
« on: December 19, 2016, 02:11:38 PM »
I’m finally getting around to mounting a 2nd QCTP on the rear of my ORAC.  Merry Christmas to me!

Has anyone here used a rear mounted tool post successfully along with a front mounted one?  I’ve heard Hood mention that rear mounted tools befuddle Mach3 or was it Dolphin; I forget which.  Anyway does anyone have a method or tip on how to keep tools mounted on the back side moving the correct direction?  (Other than just plain reminding oneself which way is which and hope you get it right?)
Milton from Tennessee ya'll.

Offline RICH

*
  • *
  •  7,332 7,332
    • View Profile
Re: Question about rear-mounted lathe QCTP
« Reply #1 on: December 19, 2016, 06:50:17 PM »
Milton,
Do not mix front and rear tool posts, one or the other but not both. You have been warned! If I remember correctly the rear tool posts uses the G55 work offset.

RICH

Modified 12/20/16 : See Reply #4
« Last Edit: December 20, 2016, 02:59:25 PM by RICH »

Offline Hood

*
  •  25,816 25,816
  • Carnoustie, Scotland
    • View Profile
Re: Question about rear-mounted lathe QCTP
« Reply #2 on: December 20, 2016, 03:18:03 AM »
Always have the tools in the tool table set up as the same Tool Post. So I would imagine you have all of your present tools set as Front, so make sure you set your new tool as Front as well even though it is at the rear. Failing to do so will really screw things up.
 That then means you have to programme negative values for the rear tool in X. Bit of a PITA but afraid Mach3 does not handle mixed Front and Rear tools well at all.
What I used to do was use G51X-2 (if in Dia mode, G51X-1 if in Rad)  just prior to moving the rear tool and G50 just after, that will set the positive X moves to negative so that any code that CAM spits out will be correct for the rear tool, assuming your CAM can not be configured to output negative code for a rear tool.
 You still have to be careful with doing the G51 as if you call the G51 too early or cancel with the G50 too late then you may send your axis totally the wrong way.

Re: Question about rear-mounted lathe QCTP
« Reply #3 on: December 20, 2016, 06:18:55 AM »
OK, I'll give that a try when I get it installed after the holidays.  Thanks & Merry Christmas all!
Milton from Tennessee ya'll.

Offline RICH

*
  • *
  •  7,332 7,332
    • View Profile
Re: Question about rear-mounted lathe QCTP
« Reply #4 on: December 20, 2016, 03:01:37 PM »
A clarification...................

In the tool table there is input for "Dist Front to Rear post".
This is the distance from front to rear tool post.
The distance entered will be used to adjust G55 work offset as
related to the G54 offset.

So you may wish to explore this more and see the affects if tools are mixed.
Better yet just don't mix !
 
RICH
Re: Question about rear-mounted lathe QCTP
« Reply #5 on: December 20, 2016, 06:35:32 PM »
Thanks Rich, my plan is to begin with a parting tool on the back side, a 3 tool gang holder that locks down to both QCTP's for rigidity and my Z-axis opto probe.  When (if) those tools are successful I may set up a few more to reduce the number of tool changes on each job.  Most of the repetitive jobs I do only need a couple tools.
Milton from Tennessee ya'll.

Offline RICH

*
  • *
  •  7,332 7,332
    • View Profile
Re: Question about rear-mounted lathe QCTP
« Reply #6 on: December 21, 2016, 07:35:30 AM »
The best thing I ever did was modify the screen set to utilize probing for the following:
- Find lathe center or part location.
- Probe tools and populate the tool table
- Allow for probing and adjustment of tools ie; drills / reamers / etc.
Additionaly probing can be done to get locations or copy a part and create a dxf file manualy or automaticaly depending on the probe used.

The screen was modified to open, save, export / import, reset or bring in a master tool list.

 
The screen is done to how "I want it to work" ( don't use home switches here as I have no need for them) and use soft limits ( no switches ) to get a warning if the tool called  will exceed the travel of the carriage.Also don't use any work offsets initialy. Work affsets are used for multiple parts to be done using the same gcode and can be easily changed.
 
The tool setter is simply a 1" diameter standard accurately mounted so it can be placed in the chuck and probing can be done on 4 different
surfaces.


For tool touch off:

Just zero out the tool setter, probe with master tool and probe all the
others or just any tool and the probing routine automativcaly takes care of populating the tool table. The probing is very accurate.

 
To set up a job:

Just probe the tool setter with master tool, insert stock, probe the stock end ( or some location ). Home is used as the tool change postion and all code is based on the lathe center and end of the stock. All done with a few button clicks and NO MEASURING!.

Additionaly:

Now if you want to copy or measure a profile I use the probing to get points along the profile. This is done auto or manualy depending on the
probe used. For quick and dirty a visual indication probe is used
along with MPG's to get a few selected points and a dxf file can be created or the points put right into Acad and drawn.Don't use this much but sure does come in handy at times.

Just some things you can consider as you continue to have fun,

BTW, there is a write on how someone used gang tooling and avoided the issues with front and back tool posts.
Do a search.

RICH