What's new
What's new

What is wrong with this Program?!?

Gamy R

Plastic
Joined
Aug 5, 2011
Location
Odessa, TX.
Hi all, my programmer wrote this program for us then went on vacation..
We want to run this on an older Hitachi Seiki HiTec-Turn 25M with Seicos LMulti control.

Thanks in advance...

O2005(1 1/2" BOP STUD - OP#1)
(1 1/2"-8UN PIN END)
(11/12/2019)

N1G50S1500
G0G54T101(WNMG 432 FACE & TURN)
G96S450M3
X2.4Z.03M8
G1X-.062F.01
G0X2.4W.1
Z0
G1X-.062
G0X2.27Z.1
G71P20Q21U300W30D700F.011
N20G0X1.23
G1Z0
X1.5Z-.135F.006
Z-3.465F.008
X2.037F.004
G3X2.187W-750R.075
N21G1X2.27F.006
G70P20Q21F.008
G28U0M9
G0Z7.
T100
M1
 
What it won't run? I'm not familiar with this control but nothing jumps out at me. Why he uses incremental to swing the radius is weird but whatever floats your boat? I don't see TNRC, I turn the spindle on with G97 then call whatever sfm I'm gonna run with G96 S?. Looks like it should run. Is it throwing an alarm?

Brent
 
I don't see anything that jumps out at me, assuming your lathe accepts single line multi-repetitive cycles.

Are you getting an alarm?

I wouldn't set my feedrates that way- I'd take the F,008 it out of the G70 line and put it in the G1 Z0 line after N20. The G70 line will run whatever feedrates are called out in the P-Q blocks. That shouldn't prevent the program from running though.
 
Hi all, my programmer wrote this program for us then went on vacation..
We want to run this on an older Hitachi Seiki HiTec-Turn 25M with Seicos LMulti control.

Thanks in advance...

O2005(1 1/2" BOP STUD - OP#1)
(1 1/2"-8UN PIN END)
(11/12/2019)

N1G50S1500
G0G54T101(WNMG 432 FACE & TURN)
G96S450M3
X2.4Z.03M8
G1X-.062F.01
G0X2.4W.1
Z0
G1X-.062
G0X2.27Z.1
G71P20Q21U300W30D700F.011
N20G0X1.23
G1Z0
X1.5Z-.135F.006
Z-3.465F.008
X2.037F.004 <<<<< Missing G01
G3X2.187W-750R.075 <<<< no period should be 0.075
N21G1X2.27F.006
G70P20Q21F.008
G28U0M9
G0Z7.
T100
M1

but you have to give someone an idea of what its not doing.
 
X2.037F.004 <<<<< Missing G01
G3X2.187W-750R.075 <<<< no period should be 0.075
First case, it's already in G1 from the G1 Z0 line...

Second case, W-750 is incremental Z-.075, so R.075 is okay...

I'm guessing the control does not like the G71 format.
 
First case, it's already in G1 from the G1 Z0 line...

Second case, W-750 is incremental Z-.075, so R.075 is okay...

I'm guessing the control does not like the G71 format.

Generally the 1st g01 works but it needs to be there before a g02/g03 and after on some machines. My old siecos control needed at as well as my yasnac.

The 750 doesnt seem correct I if I remember the seicos controls need a decimal point. Its been a long time since I ran them and I thought there was a parm for to set for reading with out a decimal

hard to tell with crappy programming and no mention of what its not doing There was a bunch of g70 type formats that worked fine in that control.
 
Thanks Guys... It appears that the machine does did not like the G54 T101 from the 1st line "G0"...
Modified as follows: "G0 T100(WNMG 432 FACE & TURN)" and ran without issues.

Thanks for your help...
 
Operator error.

I run my business, not my machines but explain "operator error" when all you do is push a couple of buttons and machine runs with proper program??? If you don't want to elaborate don't but don't be a simpleton with "operator error" as your comment!
 
when all you do is push a couple of buttons and machine runs with proper program???
:scratchchin:

not quite that simple but its easy to see how a guy that doesnt run the machine thinks all you do is throw the tools in and push a couple of buttons...but thats besides the point

To the original question(which has been answered) next time it would be much more beneficial to let us know what line of code the machine is hung up on
 
Thanks Guys... It appears that the machine does did not like the G54 T101 from the 1st line "G0"...
Modified as follows: "G0 T100(WNMG 432 FACE & TURN)" and ran without issues.

Thanks for your help...

T100 means tool offset not being used.
 








 
Back
Top