Machsupport Forum

Mach Discussion => General Mach Discussion => Topic started by: panaceabeachbum on September 16, 2008, 09:45:01 AM

Title: problems after g76 in turn
Post by: panaceabeachbum on September 16, 2008, 09:45:01 AM
After I run the thread cycle, g76 , on the lathe in mach turn the machine will no longer make any moves at any speeds other than the rapid traverse speed.  All g1 inputs run at full rapid traverse speed (200IPM) . Not sure how to reset/clear the condition other than rebooting mach .  I thought the g80 at the beginning of the next program should clear it but no luck . I am sure I am missing something simple. Thanks
Title: Re: problems after g76 in turn
Post by: Hood on September 16, 2008, 09:58:06 AM
Is this with the 008 version?

Hood
Title: Re: problems after g76 in turn
Post by: panaceabeachbum on September 16, 2008, 10:00:30 AM
Its happening on all three of my lathes , two of which are running 2.64 and 2.57
Title: Re: problems after g76 in turn
Post by: Overloaded on September 16, 2008, 10:58:44 AM
RT,
There maybe should be a G94 in the begining. G76 uses G95 and it may still be in effect.
RC
Title: Re: problems after g76 in turn
Post by: panaceabeachbum on September 16, 2008, 12:37:04 PM
I have the following at the begining

G18 G40 G49 G90 G94 G80
Title: Re: problems after g76 in turn
Post by: Overloaded on September 16, 2008, 12:59:15 PM
Might check that it is actually in G94 on the diag. screen.
Could put G94 in the line right after the G76.
RC
Title: Re: problems after g76 in turn
Post by: Hood on September 16, 2008, 01:23:34 PM
Can you attach a sample of the code and i will test it out on the lathe tomorrow.
Hood
Title: Re: problems after g76 in turn
Post by: panaceabeachbum on September 16, 2008, 07:40:35 PM
Here is the basic code I use to cut 20 tpi internal thread in 1.5 ID 4130 tubing.


G0 G40 G18 G80 G50 G90
G00 z4
x4
T1010M6
G00  X0.77
G00 Z0.1
G00 X0.745
M03 S200
M08
g4p2
G76 X0.778 Z-1.05 Q2 P0.05 J0.003 L45 H0.002 I29 C0.025 B0.0001 T0
M9
M5
M30
Title: Re: problems after g76 in turn
Post by: panaceabeachbum on September 16, 2008, 07:50:31 PM
Other than the position before tool change this is the code straight out of the  wizard in Mach ,  It runs fine but in all the machines I cant seem to call out the speed in anything run after a g76 without rebooting mach . I can run the same code as above hundreds of times a day with no problem , but if I type in a G01 F** after a g76 it runs everything at rapid transit speeds , which gets quite exciting on the machine that will run 600IPM . Any programs run after a g76 all operate at rapid speeds regardless of the speeds called out in the program.

The following is the first line of the code I need to run after the g76 and I thought it had the proper gcode to cancell the canned cycle

G18 G40 G49 G90 G94 G80

After the g76 I am just running a basic turn cycle generated in the turn wizard
Title: Re: problems after g76 in turn
Post by: Overloaded on September 16, 2008, 07:53:05 PM
In this code G95 is implemented in the G76 cycle. It is modal. It needs a G94 to go back to units per min. unless your G1 moves are IN G95 which is in. per rev.
What are your other G1's in...G95 or G94 ?
I'm confusing me,
RC
Title: Re: problems after g76 in turn
Post by: Overloaded on September 16, 2008, 08:00:01 PM
In other words...G94 F1 is 1" per minute
                       G95 F1 is 1" per revolution
Title: Re: problems after g76 in turn
Post by: Hood on September 16, 2008, 08:04:34 PM
If previous to the G76 you were running G94 then it should automatically revert, I am sure it does for me but will test out properly tomorrow. If I remember ::)

Hood
Title: Re: problems after g76 in turn
Post by: panaceabeachbum on September 16, 2008, 08:07:58 PM
so g94 after g76 should bring me back to IPM
Title: Re: problems after g76 in turn
Post by: Hood on September 16, 2008, 08:08:57 PM
You shouldnt need it I dont think but try and see.
Hood
Title: Re: problems after g76 in turn
Post by: Overloaded on September 16, 2008, 08:10:51 PM
I'll try to remind you ;)....I wasn't aware that it did. But i'm still new at this.
Was it mentioned what Rev. we're using ?
RC
Title: Re: problems after g76 in turn
Post by: Hood on September 16, 2008, 08:17:58 PM
I think there were issues a while back with it not reverting but Richard said he has various versions including 008, or at least I think he did ::)

Hood
Title: Re: problems after g76 in turn
Post by: RICH on September 16, 2008, 08:48:26 PM
This thread must be the polite way of saying no updates today  ;D

Didn't see any response if it's going back to a G94 ( light turns green ) when in diagnostics after threading is completed. If the green light stays green ( G95  box ) and you then use a G94 via MDI line it should switch to indicate the change.
It should alternate between G94 and G95 post a  thread pass if index signal is picked up. But then the diagnostics screen may be bugged out since you guys are using tests version and this may be totaly without merit.

RICH without an ARD  :)
Title: Re: problems after g76 in turn
Post by: panaceabeachbum on September 16, 2008, 09:37:17 PM
I just double checked, 2.61 on one machine, 2.57 on the second and the latest development version on the third and all three seem to be having the problem . The one with the latest version .008 I havent run a full program with after the g76 on this paticular machine but when I type in g1 z** f1. in the MDI line the z axis moves at 600IPM , which is quite an eye opener since the saddle and tool changer wieght somewhere over 500 lbs
Title: Re: problems after g76 in turn
Post by: Overloaded on September 16, 2008, 09:42:49 PM
Try MDI     G94 G1 Z** F1     and see what happens
Title: Re: problems after g76 in turn
Post by: Hood on September 17, 2008, 07:09:18 AM
OK just remembered a few mins ago ;)
Tried it and RC is indeed correct, there was mention of it returning to previous G94 if it was, looks like its not been done though :(
Putting a G94 sfter the tyhreading is complete however does return it to feed per min, I have just confirmed.
Hood
Title: Re: problems after g76 in turn
Post by: DaveDoesIT on September 17, 2008, 10:45:53 AM
Here is the basic code I use to cut 20 tpi internal thread in 1.5 ID 4130 tubing.

Put G94 after the G76 call, I think it is still set to G95 from within G76. The fact it does the same on 3 machines means it is in the code. No?

Dave
Title: Re: problems after g76 in turn
Post by: panaceabeachbum on September 17, 2008, 06:49:40 PM
Yep that works, for some reason I thought it would return to g94 after the thread cycle , will just add g94 to my post processor. thanks
Title: Re: problems after g76 in turn
Post by: Vicke on September 18, 2008, 06:37:24 PM
Would you like to make a short copy of the top of the program. Becaurse it is always nice to see G-code in real.