Hello Guest it is October 23, 2021, 04:21:20 AM

Author Topic: Why would Mach ignore G01 & do G00 instead?  (Read 2458 times)

0 Members and 1 Guest are viewing this topic.

Why would Mach ignore G01 & do G00 instead?
« on: July 13, 2013, 03:23:49 PM »
Had a great day with  mach threading & parting off until it jammed my parting tool straight into the work wide open.  G01's were interpreted as G00's until I restarted Mach.  Happened 4 times and I think it happens only after running a "Simple Threading" wizard.

v.057, PP
Milton from Tennessee ya'll.

Offline Hood

*
  •  25,838 25,838
  • Carnoustie, Scotland
    • View Profile
Re: Why would Mach ignore G01 & do G00 instead?
« Reply #1 on: July 13, 2013, 05:44:16 PM »
Could it be you normally have your code in Feed Per Min  mode and thus your feedrates are for Feed Per Minute  but when threading it is changed to Feed Per Rev. In other words if you have  Mach in G94 and command a feedrate of 250mm/min(10 IPM ) you then do your thread but then you dont change back to G94 then your feerate will now be 250mm per rev (10 inch per rev) and will look suspiciously like a rapid :)

Always a good idea to programme a lathe as feed per rev anyway, in my opinion, it has many advantages.

Hood
Re: Why would Mach ignore G01 & do G00 instead?
« Reply #2 on: July 13, 2013, 10:51:48 PM »
Ahh OK thanks, that makes sense.  Gotta learn about G94 & feed per rev now.  Sigh, is there no end to the learning needed to do this stuff?  (Answer: no, of course not!)

I was so proud to get 4 tools accurately electronically tucked away into the tool table.  I switched tools around several times with repeatable & expected results, parted off 5/8" steel stock with authority, cut my 1st CNC threads in steel with good results.  Wow, (methinks) I got this stuff now!!  Then BANG!...my best & sharpest homemade parting tool destroyed in an instant.

At least my 1st threads came out pretty well considering the tool was a cheap brazed carbide cutter and the steel was hardware store 5/8 CRS rod.  The only thing I had lying around near 5/8" to check a thread with was a 16x1.5 mm die so I chose that.  My lathe is set up in inches so I just did the conversion math and let 'er rip.  It came out great & the die screwed right on with hardly any slop.  The threads faces look a bit gnarly but I think that'll get better when I can afford "real" inserts and holder.

The 3/4 hp DC motor with KBCC-125R speed control with tach generator feedback did a great job of holding the speed steady enough to cut good threads...I'm happy with that!
Milton from Tennessee ya'll.

Offline Hood

*
  •  25,838 25,838
  • Carnoustie, Scotland
    • View Profile
Re: Why would Mach ignore G01 & do G00 instead?
« Reply #3 on: July 14, 2013, 03:54:13 AM »
G95 is Feed Per Rev, G94 Feed Per Min

As said G95 has many advantages in a lathe, for example alter your spindle speed via code and your chipload will stay constant where if you programmed in G94 you would also have to alter your code with a new feedrate to keep chipload to what it was previously.


I have G95 in my initialisation string so that my lathes always default to G95 and of course my code always  has (or should have ;) ) a G95 in it just to be doubly sure, not sure if the wizards will put in a G95 as I rarely use them. Another good thing about programming in G95 is your feedrates are small, typically for me,  0.35mm for roughing and 0.15mm for finish. Now if for some reason the lathe is put into G94 mode and my code doesnt have G95 in it then no big deal, the feed will be extremely slow and I will notice it and realise. If using G94 feedrates normally and for some reason G95 becomes active then the axis suddenly moves at rapid speeds or near to them and I will still realise whats wrong but its too late by then ;D


G95 for lathe work is  a good habit to get into ;)
Hood
Re: Why would Mach ignore G01 & do G00 instead?
« Reply #4 on: July 14, 2013, 07:58:05 AM »
Thanks for the sage advice Hood, that makes perfect sense.

Have I said lately how much I (and every other noobie Mach user I'm sure) appreciate your (and all the other gurus here) patience & willingness to teach us this stuff? ;D  I don't know how you do all the work you do and still find the time to fix our problems too!
Milton from Tennessee ya'll.