Hello Guest it is April 20, 2021, 01:02:57 AM

Author Topic: Problem in Turning after Threading  (Read 5131 times)

0 Members and 1 Guest are viewing this topic.

Problem in Turning after Threading
« on: March 23, 2009, 07:38:56 AM »
 Dear All

I have designed 3-axis milling and also lathe both are working very nicely using Mach3. Now after a number trails of turning taken in lathe i observed one problem i.e. if i run G76 for threading, it works very nicely. but after that if run simple truning then it is not working correctly. e.g. my code is G01 z-20 F50. then z axis should move with the feedrate of 50mm/minute. instead of that it moves 2000mm/minute which is my rapid speed.
this problem remains as it is till i shut down mach3 and restart it. after restarting if i run simple turning job then it works perfactly. but again if i run G76 thread command then threading is Ok but after that it is not recongnizing G01 code and it always consider G00 and executes all command with G00 even if i mention G01. i have not use G32. and threading file is made from the simple threading wizard given in Mach.  kindly give the suggession on this.

thanks

sanlee

Offline Hood

*
  •  25,838 25,838
  • Carnoustie, Scotland
    • View Profile
Re: Problem in Turning after Threading
« Reply #1 on: March 23, 2009, 07:43:35 AM »
Sounds like the feed is still in G95 (feed per rev), personally I think turning should be done in G95 but its up to the operator. anyway what to do is after the threading move put a G94 in your code and that will shift it back to Feed per min mode.
Hood
Re: Problem in Turning after Threading
« Reply #2 on: March 23, 2009, 08:57:12 AM »
Thanks Hood

after writing G94 it works perfactly. But one more thing i want to know that is it possible to write G94 in some of the macro which is written for G76, so that operator need not remember to write every time G94 after threading code is over.

thanks again

sanlee

Offline Hood

*
  •  25,838 25,838
  • Carnoustie, Scotland
    • View Profile
Re: Problem in Turning after Threading
« Reply #3 on: March 23, 2009, 09:06:26 AM »
Write it into your post processor so the code is added automatically, actually I thought it did revert automatically, but possibly not,  however that may depend if you have a G94 in your preamble at the start of the code, if I get a chance I will try it out.
The norm for lathe work is to do all turning  in G95  as that means no matter what your spindle speed is the feed will be correct.
Hood

Offline Hood

*
  •  25,838 25,838
  • Carnoustie, Scotland
    • View Profile
Re: Problem in Turning after Threading
« Reply #4 on: March 23, 2009, 09:23:28 AM »
OK just tested it here and it does revert back to G94 if the preamble has a G94 in it and you should always have a preample on any code you do to set the parameters up so that you are not taken by surprise if the normal mode has been changed by some previous code you have run.
Hood
Re: Problem in Turning after Threading
« Reply #5 on: March 23, 2009, 10:00:22 AM »
thanks hood

wel! i undserstood now. and now it revert back to G94 if the preamble has G94. Even one more thing i have tried and it works very nicely. i.e. i have written Code "G94" in M1076.m1s macro at the last line. so now there is no need to have G94 at preamble.

Thanks lot

sanlee

Offline Hood

*
  •  25,838 25,838
  • Carnoustie, Scotland
    • View Profile
Re: Problem in Turning after Threading
« Reply #6 on: March 23, 2009, 10:08:50 AM »
You should really make it a habit of having a preamble and you should have it with the parameters that you consider your norm. If you hand code then its a simple thing to get into the habit of adding, if you use CAM then its even easier as you just get the Post Processor to add it and you never need to think of it again :)
 If you rely on the G94 at the end of your M76 macro then it will at some point in time bite you in the arse, for example you may upgrade the revision of Mach and it may overwrite the m1076 macro, you will maybe not realise and next code you run it shoots off at 50mm/rev instead of 50mm/min.

Hood
Re: Problem in Turning after Threading
« Reply #7 on: March 24, 2009, 12:13:36 AM »
Ya Hood

you are absolutely right. instead of writing in M1076 i should make a practice to write in preamble. i will definately follow this. thanks again

sanlee