Hello Guest it is October 14, 2019, 02:45:10 AM

Author Topic: Feed rate after tool change problem  (Read 7898 times)

0 Members and 1 Guest are viewing this topic.

Re: Feed rate after tool change problem
« Reply #10 on: September 23, 2008, 08:29:00 AM »
I guess I'm the one that does not understand.

Why is the move to safe height move at rapid speed and the move back down at the feed rate of F1. There is no gcode moves in there.

Why does the Z move down at all in fact? If the z moves to safe height after a tool change that's fine. Shouldn't it wait for an move instruction at safe height? The next instruction in my code after the tool change is the spindle on. There are no moves yet the Z moves down on it's own.

If the current operation is by design then that is fine with me and I'll just have to change the Mach Post in Sheetcam to set a higher initial feed rate that I can deal with.

This whole question came about from Les of Sheetcam. Sheetcam jams the F1 in there. When I told Les I had to change the F1 to a higher rate, he said it was not necessary which led to the thinking that Mach was doing something weird.



Offline Hood

*
  •  25,855 25,855
  • Carnoustie, Scotland
    • View Profile
Re: Feed rate after tool change problem
« Reply #11 on: September 23, 2008, 12:15:13 PM »
OK what is happening is your toolchange is calling the M6 macro, the M6 tells the axis to move to your toolchange position and wait for the Start button and then move back to the position it was at previously at a G1 feedrate. If you actually look whats happening is your axis starts at Zero, it rapids to the  Toolchange position, it then feeds back to zero then the next line is a rapid to 0.6, not a very good idea LOL.
 You could edit the macro so that it only goes to the safe Z, you could edit the post processor to do similar or always do a certain Z move before a change or whatever you wanted.
 I have not looked at the standard M6 macro for a while but will do so later on and see exactly whats in there and could probably edit it to take out the return to previous position if you want that? Just in the door so it will be in a while.

Hood
Re: Feed rate after tool change problem
« Reply #12 on: September 23, 2008, 03:44:27 PM »
Hood,

The M6(start) macro has this in it:

  tool = GetSelectedTool()

  SetCurrentTool( tool )

The M6(end) macro is empty.

I'm assuming that the M6(start) macro does no movement and just updates the screen.

I did some more playing around with this and found that the tool offset has something to do with it. I don't do much with tools settings in mach in fact, the tool table is all zeros. By playing with safe height and tool offset I see now what is happening. Upon hitting the M6, Mach updates the screen as per the macro and waits for a continue. Upon hitting start the z rises to safe height rapid speed and then immediately moves to the tool height as set in the tool table at feed rate. It then continues on as expected.

If this is normal behavior by design then so be it. I can live with it. I just don't understand why. In my situation with no tool changer I have to manually fit tools and zero them. Once fitted and zeroed I am happy to see the move to safe height for protection. The move to the offset height is a wasted move.

Ted

Offline Hood

*
  •  25,855 25,855
  • Carnoustie, Scotland
    • View Profile
Re: Feed rate after tool change problem
« Reply #13 on: September 23, 2008, 03:53:23 PM »
OK how do you go about a tool change, ie do you jog up, put the new tool in, jog down to sufrface and zero the DRO?
Hood
Re: Feed rate after tool change problem
« Reply #14 on: September 23, 2008, 07:07:18 PM »
Yup, that's exactly it.

I'm not always worried about the exact height as long as I'm no lower then the surface height. I'm mainly cutting through a 0.060" surface on most of my jobs. I setup most of the jobs to cut 0.200" deep so I have plenty of leeway. On jobs where z precision is required, I touch off a gauge block connected to the probe input. I have a little macro that does that for me.


I guess if the Mach behavior is normal by design I'll let Les at Sheetcam know about it.

Thanks,

Ted

Offline Hood

*
  •  25,855 25,855
  • Carnoustie, Scotland
    • View Profile
Re: Feed rate after tool change problem
« Reply #15 on: September 23, 2008, 07:18:17 PM »
Nothing is really normal, just depends on your code and also whats in your macros.
 You said M6 End is empty so really I am not sure why your axis is moving way up then down again. You sure its definitely empty? You are looking in the correct profiles macro folder?
Hood
Re: Feed rate after tool change problem
« Reply #16 on: September 23, 2008, 08:10:01 PM »
Ha, I lied.

M6 end has the following code:

REM The default script here moves the tool back to m6start if any movement has occured during the tool change..

x = GetToolChangeStart( 0 )
y = GetToolChangeStart( 1 )
z = GetToolChangeStart( 2 )
a = GetToolChangeStart( 3 )
b = GetToolChangeStart( 4 )
c = GetToolChangeStart( 5 )
if(IsSafeZ() = 1) Then
   SafeZ = GetSafeZ()
   if  SafeZ  > z then StraightTraverse x, y,SafeZ, a, b, c
      StraightFeed  x, y,  z  , a, b, c
else
Code"G00 X" & x & "Y" & y
end if

If I'm reading this correctly, If Safe Z higher then the current Z then will do a rapid move to Safe Z. Then we will do a feed move to the original position.

If Safe Z is not higher (already above or higher then Safe Z) we will do a rapid move to the original x,y.

This explains what I'm seeing.

I must have looked at an old profile's macros when I saw the empty M6 end. Sorry about that.

Thanks for your help. I'll pass this info to Les.

Ted

Offline Hood

*
  •  25,855 25,855
  • Carnoustie, Scotland
    • View Profile
Re: Feed rate after tool change problem
« Reply #17 on: September 23, 2008, 08:14:37 PM »
If you REM all that out it should be fine the way your Post Processor is writing the code. Only thing is you will have to watch it doesnt get overwritten by an upgrade. Easiest way to solve that problem is have a custom profile and the macros for that profile wont get overwritted during an upgrade.
Hood

Offline Kristin D

*
  •  203 203
  • Take that you LazyCam, next stop the glue factory!
    • View Profile
Re: Feed rate after tool change problem
« Reply #18 on: September 23, 2008, 09:15:59 PM »
Hood,

I can't see REM'ng everything out of M6end but I am sure something could be modified to prevent this.

Kristin
Re: Feed rate after tool change problem
« Reply #19 on: September 23, 2008, 10:07:32 PM »
I think I'll stick to modifying the post in Sheetcam to set the initial feed rate to something I can live with instead of the F1 Les has provided.

I don't mind the extra moves I just can't wait forever at F1 speed.

This way I don't have to worry about Mach upgrades.

Thanks for your help.

Ted