Hello,
I have the program for Threadmill. This program for fanuc control is very good but for Okuma osp5020M it alarm 452.
I don't now Why?
Thanks,Attachment 282612
Printable View
Hello,
I have the program for Threadmill. This program for fanuc control is very good but for Okuma osp5020M it alarm 452.
I don't now Why?
Thanks,Attachment 282612
The startpoint, infeed, CL all look good to me; on which line do you get the error?
My first guess, especially since this is a 5000-series control, is that the G42 and G40 lines need to take place on a G01 move rather than a G02/03. Try this... on the G0/G90 line, change the move to X0 Y0, then once inside the hole, G01 G42 D1 X0 Y12, then do the G02 moves.
Like this:
G0 G90 G54 X0. Y0. S500 M5
G43 H1 Z50.
Z3.
G1 Z.5 F200.
G1 G42 D1 X0 Y12.
G2 X17. Y0. Z0. I4.265 J-12.
Then, on the last move, cancel the cutter comp the same way: do a G40 G01 X0 Y0.
X0. Y-17. Z-14.5 I-17. J0.
X-12. Y0. Z-15. I0. J12.735
G40 G1 X0 Y0
G0 Z3.
The older controls were real picky about calling/cancelling cutter comp; I always do it on a G01 line.
If that does not do it, check to see if you have an extremely large value in D01. The move that calls up comp needs to be *at least* as long as the amount of comp.
Okuma uses different codes, close..... but .....no prize givenQuote:
Originally Posted by KHOATRANNGOC
- They don't use G54... or G43
- Spindle is NOT started
- Cutter comp MUST start / end on a linear move...NOT on an arc
- G28 ( may not work )
Okuma alarm message IS the complete line of info, not just the alarm number.....
- it quite often tells you the possible solution
As a clarification:Quote:
Originally Posted by Superman
Okuma HAS G43/G54, they just don't do the same things as a Fanuc does. IE: G54=Tool length offset in the X (55/6/7/8/9=Y/Z/4th/5th/6th)
The Cutter comp linear move mentioned above can be a G00.
Good luck.
Hello,
I change G code G43/G54 but it alarm 452.
I don't now why?
ThanksAttachment 282738
the alarm relates to XYZ end point or IJK center point not correct.
are you sure your machine has helical interpolation option?
post the COMPLETE alarm message the number alone is not enough info
What IS the WHOLE line of the alarm message ?Quote:
Originally Posted by Superman
- what does the Alarms & Errors manual tell you for the solution ?
The alarm #s for this control, usually do not follow on to a different control, I am assuming this is an MC-30VA
1 area that could give a problem
---- machine cannot do a 3 axis arc move ( a MC-4VA I worked could not )
Try this.....Z moves commented out
Set D1 = 0
Set work origin P1 in space above table
--- run it make sure it works, then remove the brackets for the Z moves
I think the control doesn't like lower case letters either
You may get problems trying to do a full circle.....it may just plunge ( as X & Y are already at the start point )Code:%
G21 ( CHECK IF CONTROL IS SET TO METRIC )
G0 G17 G40 G80 G90 G94 ( SAFTEY CODES )
G15 P1 ( USE #1 WORK CO-ORDINATE SYSTEM )
()
T1 M6
()
G0 G90 X0. Y0.
S500 M3
G56 H1 Z50.
Z3. M8
G1 Z.5 F2000.
G42 D1 X17. Y0. Z0. F1000.
G2 X-17. I-17. J0. (Z-1.)
X17 I17. J0. (Z-2.)
X-17. I-17. J0. (Z-3.)
X17. I17. J0. (Z-4.)
X-17. I-17. J0. (Z-5.)
X17. I17. J0. (Z-6.)
X-17. I-17. J0. (Z-7.)
X17. I17. J0. (Z-8.)
G1 G40 X0. Y0.
G0 Z3.
Z50.
M5
M9 ( COOLANT OFF
G80 (CANCEL CYCLES
G94 ( FEED PER MINUTE
G91 G28 Z0.
G91 G28 X0. Y0.
G90 ( ALWAYS LEAVE IN ABSOLUTE )
( G30 P1 )( RETURN TO P1 REFERENCE POINT
( CHECK IF THE ABOVE LINE HAS BEEN SET ----- VERY CAREFULLY
M30
%
circles may need to be broken into 180° arcs
I typed this into a P200 okuma I have out of morbid curiosity.
The program runs in machine lock as you have it shown the second time.
I am fairly certain superman and ford are both correct that your machine doesn't have the helical interpolation option on it. I think you're out of luck.
Hello,
I am set D1=0 but it alarm. This machine have not helical interpolation option, I don't now why?
Attachment 282906
you can't run that program on your machine without the option. there is no way around the problem other than
to contact Okuma and pay some dollars for the helical interpolation option. or don't do that kind of work on your machine.
There is only one way with the current machine config..... not to have Z moves on arcsQuote:
Originally Posted by fordav11
- called.... point to point machining ( no arcs )
accuracy is obtained when small linear moves are used
but....- long code, jerky movements, may have tool comp problems.....but it does work
not having Z moves would create a different toolpath, right? thus, not what is wanted?
depending on the accuracy required,...if set too coarse......a circle can come out like a hexagonQuote:
Originally Posted by fordav11
But...What do you think surfacing involves when an arc filter is turned OFF ?.......point to point code
An arc movement in a CNC is lots of tiny XY linear movements
a helix is just an arc with Z moves...... lots & lots of tiny XYZ linear moves
Hello,
I want have Z moves would create a threadmill. but not having Z moves it not right.
Can you for me the program different create a threamill ?
Thanks,
the only way to do it on your machine is program many small G01 movements.
you machine will not do G02/G03 XYZ IJK
if your Fanuc software can do small straight movements then tell it to generate G01 only
if not you are out of luck or buy some software to do it using G01 only
or contact Okuma and buy Helical Milling option.