1. Configuring LinuxCNC
  3. Advanced Configuration
  5. Back tool turret layer and G76 (threading) problem

Back tool turret layer and G76 (threading) problem

More
25 Jul 2014 20:25 - 25 Jul 2014 20:53 #49124 by aike
Back tool turret layer and G76 (threading) problem was created by aike
Hi!
Usualy lathe has front turret layer and the moving in G76 (threading cycle) cycle begins from X max to X min (in the deep of workspace).
But I have back turret layer, and when I use G76 command, the drive line moving hit tool in the metal.
I need to swap drive line from positive to negative, but don't know how to do this.
The link in vodeo:

I hope you will see it yourself.
Last edit: 25 Jul 2014 20:53 by aike. Reason: add video

Please Log in or Create an account to join the conversation.

More
25 Jul 2014 21:33 #49128 by cradek
Replied by cradek on topic Back tool turret layer and G76 (threading) problem
linuxcnc.org/docs/html/gcode/gcode.html#...G76-Threading-Canned

The docs say you can make I negative to swap the direction. Does that work?

Please Log in or Create an account to join the conversation.

More
25 Jul 2014 21:37 #49129 by aike
Replied by aike on topic Back tool turret layer and G76 (threading) problem
Negative for internal thread, but I have external thread.

Please Log in or Create an account to join the conversation.

More
25 Jul 2014 23:13 - 25 Jul 2014 23:14 #49132 by ArcEye
Replied by ArcEye on topic Back tool turret layer and G76 (threading) problem
Hi

A hairy old subject

See this for instance
sourceforge.net/p/emc/mailman/emc-develo...aHrw@mail.gmail.com/

I use a slant bed lathe, so I have this set in my ~/.axis.rc
##This entry in ~/.axis.rc will change the plot around so that the X axis moves downwards towards zero 

## lathe rotation of axes for slantbed lathe
if lathe:
    bind_axis("Down", "Up", 0)
    def set_view_y(event=None):
	widgets.view_z.configure(relief="link")
        widgets.view_z2.configure(relief="link")
	widgets.view_x.configure(relief="link")
        widgets.view_y.configure(relief="sunken")
	widgets.view_p.configure(relief="link")
        vars.view_type.set(4)
	o.reset()
        glRotatef(90, 1, 0, 0)
	glRotatef(90, 0, 1, 0)
        o.set_eyepoint(5.)
	o.perspective = False
        o.lat = -90
	o.lon = 0
        o.tkRedraw()
						  
    TclCommands.set_view_y = commands.set_view_y = set_view_y
    root_window.bind("v", commands.set_view_y)
    root_window.after_idle(commands.set_view_y)
#

Because I home above the spindle and touch off from that it works fine

The only 'simple' way I have found to change from front tool to back tool ( or vice versa in my case as I have a gang tooling plate below the centre line)
is to change the home position for the X axis, but that depends upon how much carraige movement you have.

Trying to rotate about the Z axis with G10 L2 is supposed to work as is GEOMETRY = -XZ but I just made my head hurt trying :laugh:

good luck
Last edit: 25 Jul 2014 23:14 by ArcEye.

Please Log in or Create an account to join the conversation.

More
26 Jul 2014 00:33 #49137 by andypugh
Replied by andypugh on topic Back tool turret layer and G76 (threading) problem

Hi!
Usualy lathe has front turret layer and the moving in G76 (threading cycle) cycle begins from X max to X min (in the deep of workspace).
But I have back turret layer, and when I use G76 command, the drive line moving hit tool in the metal..


I can't see how the turret position has any effect on the threading cycle.
If X+ is "more diameter" then the physical location of the toolpost is irrelevant. (though Axis probably won't display the geometry well)

It is possible that you are misunderstanding G76. I know I do any time I program it by hand.

Please Log in or Create an account to join the conversation.

More
26 Jul 2014 03:05 - 26 Jul 2014 03:07 #49144 by aike
Replied by aike on topic Back tool turret layer and G76 (threading) problem

Hi!
Usualy lathe has front turret layer and the moving in G76 (threading cycle) cycle begins from X max to X min (in the deep of workspace).
But I have back turret layer, and when I use G76 command, the drive line moving hit tool in the metal..


I can't see how the turret position has any effect on the threading cycle.
If X+ is "more diameter" then the physical location of the toolpost is irrelevant. (though Axis probably won't display the geometry well)

It is possible that you are misunderstanding G76. I know I do any time I program it by hand.

The problem is in "spare moving".
1. There is drive line.
2. I start the treading cycle.
3. "I" parameter positive for external thread and negative for internal. But in my case, I parameter TOLD THE CNC TO MOVE IN METAL AND NOT IN SPEAR SPACE! So as material is from other side of tool as in Fig 14.3 in "LinuxCNC User Manual".
The moving is from top to bottom (Fig 14.3) in my case and not from bottom to top as shown in Fig 14.3.
Attachments:
Last edit: 26 Jul 2014 03:07 by aike.

Please Log in or Create an account to join the conversation.

More
26 Jul 2014 03:21 #49147 by andypugh
Replied by andypugh on topic Back tool turret layer and G76 (threading) problem

3. "I" parameter positive for external thread and negative for internal. But in my case, I parameter TOLD THE CNC TO MOVE IN METAL AND NOT IN SPEAR SPACE! So as material is from other side of tool as in Fig 14.3 in "LinuxCNC User Manual".
The moving is from top to bottom (Fig 14.3) in my case and not from bottom to top as shown in Fig 14.3.


In that diagram bigger-X is down.

Which way is "bigger X" in your case?

It's all just numbers, the controller has no idea what is on the ends of the wires.

I am sure that the problem you have is not because of the rear-toolpost.

You can prove it by manual MDI. Imagine a 6mm thread. You would move to X7 Z0 and then use I=1 and K=1
First pass is made at X = I + increment = 5.9
Then it moves to the start X (7)
Then it returns to Z = 0, and repeats.

As long as "bigger X numbers" == "further away from the work" everything works just the same for rear toolpost as front toolpost.

Of course, if you are using negative X numbers for the rear toolpost, what I just said isn't true. But there is no reason to do that unless you have a front toolpost too.

Please Log in or Create an account to join the conversation.

More
25 Aug 2014 03:45 #50237 by joekline9
Replied by joekline9 on topic Back tool turret layer and G76 (threading) problem
I use front and back tools. I don't do anything with the axis.rc file.

I use G10 L2 R0 and G10 L2 R180 to rotate the coordinate system around the Z axis.
The same g76 parameters are used whether front or back.
The tools display correct but you need different orientation & angles for the back tools.

Tool Defs:
P is Tool No. I & J are angles, Q is orientation.

G10 L1 P4 R.002 I120 J60 Q6 (Front tool)
G10 L1 P7 R.002 I-120 J-60 Q8 (Back tool)

See:
Lathe-g76-Front-Back.ngc

I hope this helps.
Attachments:
The following user(s) said Thank You: aike

Please Log in or Create an account to join the conversation.

  1. Configuring LinuxCNC
  3. Advanced Configuration
  5. Back tool turret layer and G76 (threading) problem
Time to create page: 0.115 seconds
Powered by Kunena Forum