Hello Guest it is November 13, 2019, 11:59:39 AM

Author Topic: Cannot do G1with zero feed rate?  (Read 7026 times)

0 Members and 1 Guest are viewing this topic.

Cannot do G1with zero feed rate?
« on: March 30, 2013, 12:36:36 AM »
VERY long story....I'll make it short.
One of our forum friends spend a huge amount of time with me and managed to get my machine setup after all this time(nearly 2 years).I had almost given up but now I'm thankfull I didn't. After Mr. Chaos finished helping me I loaded some G-code and the part didn't display correctly. Inches to mm issues. So we changed the G20 to G21 and off it went... Cut my first part!!!! YAY!! :) :)
Yesterday speaking with my programming friend he realized somehow the machine must be setup to millimiters which I could have sworn we had set for inches. Lo and behold...fired it up today and sure enough! Damn millimiters!
No biggie, I changed the native units back to good old inches, adjusted the motor tunings and looks fine but I am having a couple of weird things happening. Probably easy fixes but I don't know where to look.
If I'm on the MDI tab and type in an Axis coordinate (like X 1) I get this error "Cannot do G1with zero feed rate" and other times I get this "R ijk words all missing for arcline 15" every time without any G-code loaded.

Thanks for any input
Re: Cannot do G1with zero feed rate?
« Reply #1 on: March 30, 2013, 01:03:22 AM »
No telling what modals are set on startup.  Try typing "G1 X1 F10", instead of just "X1".  Normally, you'd want the Mach3 startup string (in Config->GeneralConfig) to define the initial configuration, including G20 or G21, G0 or G1, set the Feedrate to some reasonable value, like F10, etc.

Regards,
Ray L.
Regards,
Ray L.
Re: Cannot do G1with zero feed rate?
« Reply #2 on: March 30, 2013, 01:33:59 AM »
Ray,
I typed G1 X1 F10 and it worked.Don't know why. But now I can type any coordinate (like X1,Y3,whatever) and it goes there!

Thank you!
Re: Cannot do G1with zero feed rate?
« Reply #3 on: March 30, 2013, 01:45:19 AM »
When you just type "X1", it will be interpreted as whatever the last modal command was.  If the last modal was G0, then it will do "G0 X1".  If the last modal was G1, it will do "G1 X1".  If the last modal was G2, it will do "G2 X1", which is not a valid command.  If you use the Init string to force the modal to a known state, then you'll know what it is, and behavior will be predictable.

Regards,
Ray L.
Regards,
Ray L.

Offline RICH

*
  • *
  •  7,370 7,370
    • View Profile
Re: Cannot do G1with zero feed rate?
« Reply #4 on: March 30, 2013, 08:07:16 AM »
You can create an initialization macro such that mach will always stsrt-up in a preferred state.
Have a look at Appendix "C", page 57, in the Threading on The Lathe write up which can be found in Member's Doc's.

RICH

Offline Chaoticone

*
  • *
  •  5,628 5,628
  • Precision Chaos
    • View Profile
Re: Cannot do G1with zero feed rate?
« Reply #5 on: March 30, 2013, 10:42:56 AM »
Great you cut your first part Peter!

Quote
I changed the native units back to good old inches, adjusted the motor tunings and looks fine

You should not change the native units at any time Peter.  This changes your steps per., motor tuning, tool table, work offsets, etc.  For example, if have a tool that is 3 inches long and .5 inches diameter when you change your native units that tool would now be seen as 3mm long and .5 mm diameter.  This is not the proper way and can create quite a mess.  If you work mostly in inches, the native units for the profile needs to be inches.  If you ever need to work in MMs as your units just create another profile and make it's native units MMs.

You don't have to change your native units to execute code generated to run in MMs or Inches. As Ray pointed out, you will do this with a G20 for inches or G21 for MMs.  Gcode is only units.  A G20 G0 X5.0 will move your machine 5 inches.  A G21 G0 X5.0 will move it 5 MMs no matter what your native units are set to and assuming your steps per are accurate.  Did you ever get any numbers on your ball screws to use to set your steps per? Have a look at this link and you will understand why you need the specs on the screws I think.  Screws with 5mm lead or .200" lead are very common and close to one another.  A 5mm lead converts to 0.1968498" per revolution where the .200" is exactly .200.  Sounds close right?  Now, the .200" lead will take 5 turns to move 1 inch.  The 5mm lead will take 5.08001 turns to move 1 inch so at 5 turns of a 5mm screw you will have moved .98424 inches.  That's out by .01576" per inch and this will be cumulative so multiply that by your travel.  If you command a 20 inch move that move would only go 19.6848".  That's out by .3152 inches or just over 5/16 of an inch in just 20 inches.  Over 40 inches that would double to just over 5/8 of an inch. I could cut closer with a band saw.

http://www.machsupport.com/forum/index.php/topic,12512.msg81001.html#msg81001

Brett  
;D If you could see the things I have in my head, you would be laughing too. ;D

My guard dog is not what you need to worry about!
Re: Cannot do G1with zero feed rate?
« Reply #6 on: April 02, 2013, 07:32:28 PM »
Thanks Brett and everyone else with your input. Its all good now. As far is this concern....LOL