Hello Guest it is May 07, 2021, 06:07:44 PM

Author Topic: Program Just Stops - No errors - Help  (Read 455 times)

0 Members and 1 Guest are viewing this topic.

Program Just Stops - No errors - Help
« on: August 08, 2020, 12:13:43 AM »
G'day All,

I've recently rebuilt my CNC lathe and is exhibiting some strange behaviour. I'm using the mach motion canned cycles (I've used them before, they all work [except threading, but thats a different problem], and there have been no software updates or changes since the rebuild).

The code generates is accepted and the tool path is displayed. On pressing cycle start it prompts me for a tool change, starts the spindle, rapids over to the start point and then.... stops. The spindle keeps running, there are no error messages, it just sits there. Literally doing nothing.

The first ~20 lines of code are here, it all looks good to me:

N0 (Machine type - MachMotion Lathe Canned Cycles)
N5 (Filename: C:\Mach4Hobby\GcodeFiles\Drill Boss.tap)
N10 (Generated on 8/8/2020 at 1:48:40 PM)
N15 G00 G40 G54 G64 G80 G90.1 G99 G18 G21 (Safe Start Block)
N20 %


N25 %
N30 (Starting Gcode for Facing Cycle: FaceCycle-0)
N35 ([Xi, Zi] = [18.5, 0.0]; [Xf, Zf] = [-0.5, -0.5]; Z- Direction; OD)
N40 G50 S2750 (Spindle Speed Cap)
N45 (Roughing)
N50 G00 G40 G54 G64 G80 G90.1 G99 G18 G21 (Safe Start Block)
N55 %


N60 %
N65 T0101 (Tool Change)
N70 G99 (Feed per Revolution)
N75 G96 S80 (Constant Surface Speed)
N80 M04 (Spindle Reverse)
N85 M09
N90 G00 X18.7000 Z0.1000  (Rapid move to Clearance Height)     <--------------------------it completes this line here
N95 G01 Z-0.3000 F0.1000  (Cut in on Z-Axis)     <----- it stops on this line here. it recognises the distance to go but doesn't move
N100 G01 X-0.5000 F0.1000  (Cut in on X-Axis)
N105 G01 X-0.5000 Z0.0000 F0.1000  (Spring Pass)
N110 G00 X-0.3000 Z0.1000  (Pull out to Retreat)
N115 G00 X18.7000  (Pull out to Clearance)

I've attached a screenshot (literally a photo of my screen as I didn't want to give the computer reason to do anything stupid by opening the snipping tool while it was all enabled and working). The only difference is I tried running it again so it didn't pause for the tool change because the tool was already loaded.

Your help would be greatly appreciated. I want to make these parts...
Re: Program Just Stops - No errors - Help
« Reply #1 on: August 09, 2020, 05:06:32 AM »
So as an update, the problem still persists. I have worked out that what ever it is locks out all gcode movement. Even if I stop the program and try some MDI code it won't work (though it will work prior to running the generated code).

All I can think is there is something in the safe start blocks causing issues. I'll keep trouble shooting.

I reverted to writing code by hand today, the machine works nicely.

Offline thosj

*
  •  432 432
    • View Profile
Re: Program Just Stops - No errors - Help
« Reply #2 on: August 09, 2020, 08:23:04 AM »
Edit out the start codes one at a time to try and figure it out? Start with G18.

Tom
Re: Program Just Stops - No errors - Help
« Reply #3 on: August 10, 2020, 04:11:33 PM »
F0.1 is it not too slow?

Offline Graham Waterworth

*
  • *
  •  2,322 2,322
  • Yorkshire Dales, England
    • View Profile
Re: Program Just Stops - No errors - Help
« Reply #4 on: August 11, 2020, 08:58:27 PM »
If its inches/mm a minute yes if its per rev no
Without engineers the world stops
Re: Program Just Stops - No errors - Help
« Reply #5 on: August 11, 2020, 10:54:40 PM »
 in nc file can be per rev? its not always mm/min? or inches?

Offline thosj

*
  •  432 432
    • View Profile
Re: Program Just Stops - No errors - Help
« Reply #6 on: August 13, 2020, 07:37:50 AM »
in nc file can be per rev? its not always mm/min? or inches?

Off Topic, but G94/G95?
Re: Program Just Stops - No errors - Help
« Reply #7 on: August 13, 2020, 11:33:26 AM »
G95 as i read its use for working like taping ,when need axiss refernce to spindle
but in this file :
1. i didnt see any G95
2. its G0 move not working ,as i understand

Offline Graham Waterworth

*
  • *
  •  2,322 2,322
  • Yorkshire Dales, England
    • View Profile
Re: Program Just Stops - No errors - Help
« Reply #8 on: August 13, 2020, 08:43:54 PM »
If you change the G96 to G97 and set S80 to a realistic figure for the material and size, will the program continue?
Without engineers the world stops
Re: Program Just Stops - No errors - Help
« Reply #9 on: August 29, 2020, 07:01:01 AM »
Thanks to everyone for their replies. I've been away with work recently so haven't had a chance to troubleshoot, until today...

I found the solution! It was all my fault.

I had installed an encoder for spindle speed and single point threading; when I had the problem, the encoder was disconnected for various reasons. This resulted in Mach 4 not recognizing the spindle was moving and then not feeding because it was in feed per rev mode.   

I deactivated the spindle encoder in the configuration and it all works again, yay. I also checked that it works with the encoder installed. It does, my encoder is just having some issues at the moment so I have removed it until I get to fixing it.

Thanks everyone for their suggestions.