LinkBack URL
About LinkBacks
According to my manuals, the G02/G03 functions were part of the basic commands that were included with all machines.
I didn't see a "K" value in your code... I'd put one in, even if its zero.
John
I would like to know what I am doing wrong, I can not get my lathe to do a G02 or 03, it always gives an alarm #20 (in circular interpolation the programmed end point of an arc is not located within the allowable area) no matter what I try it always gives this alarm. As I understand that the 5T can only do one quadrant arcs, I have tried absolute and incremental values, switching pos/neg directions, I even tried the example in the manual, all with no sucess. Here is my latest example, I am using the rear turret on my lathe so the tool is on the negative side of X zero when I use G50 to set X zero on the spindle center line and Z zero at the end of the part.
N010G00X-10000Z0000 (RAPID TO POSITION 1" DIA. AT Z ZERO)
N020G01Z-10000F0100 (FEED TO Z-1" ARC START POSITION)
N030G02U-5000W-5000I-5000F0100 (CLOCKWISE ARC INC. U-.5", W-.5", ARC END POSITION, ARC CENTER POSITION I-.5")
Can anyone tell me if there is something wrong with this program, or if my control might not be able to do G02/03 commands? Is there a parameter setting that might need tweeking?
Sincerly Frustrated,
Steve
According to my manuals, the G02/G03 functions were part of the basic commands that were included with all machines.
I didn't see a "K" value in your code... I'd put one in, even if its zero.
John
I noticed that your first X move goes to a negative dimension (X-10000). Is this a Mori-Seiki? Mori Seikis of that vintage had the X axis backwards from other machines, meaning that all the dimensions on the part in X were negative. It also means that G02 and G03 are reversed from the operator's perspective. Since the coordinate system is "flipped over", imagine looking UP at the part to determine "clockwise" and "counter-clockwise".
When you convert a "normal" lathe program to run on an Mori with the backwards X axis, you have to mirror all the X dimensions, swap all the G02s and G03s and also swap all the G41s and G42s (cutter comp. left and cutter comp right).
This unusual setup was due to the fact that the early Mori toolchangers were on the "backside" of the spindle, and the spindle rotated so that cutting forces were not trying to "lift" the crosslide off the ways.
I have tried that and it does not seem to matter, I think I must be having some other issue that I don't understand.
Thanks!
Steve
Originally Posted by John3
Hi Dan,
This is a 1980 Howa Sangyo, it has two four tool turrets, one in front toward the operator and one in the rear oposet side of spindle. I think I understand the co-ordinate system on this machine, but that's probably where I am in trouble.
Let me try to explain what I am doing, I first sent the cariage to the zero return position in X&Z, zeroed the readout, installed the tool I wanted to use, moved the tool to the part and recorded the X&Z readings to corespond to the parts X&Z zero. I programmed these readings into the G50X---Z--- command to set the distance the zero return position is, back from the part co-ordinate zero position. The numbers all seem to work, I can do point to point cutter paths, infact if I replace the G02 with G01 and delete the "I" value it runs the program with a diagonal cut instead of an arc. However, what you said about looking at the CW/CCW from the under side makes sence. I may have to try G03 and keep my "I" dimention negative, I think I have tried this, but I am loosing track of everything I have tried.
By the way, thanks for the rapid traverse parameter setting information, it worked perfectly, Now all I have to do is learn the way to propperly program circular interpolation on this machine.
Best Regards,
Steve
"X" is a diameter value and "I" is usually a radial value...... your command of I-5000 means to swing a 1/2 inch radius. Is that what you want?
In this example, yes .500" radius.
Steve
I normally do mills and if you ask I will tell you most lathe programming is FUBAR.
So for what it's worth, why the switch from X,Z axis in the linear moves to U,W in the G2?
I'm I right about this?....
Your U-5000 is a half in change in part diameter. That's a 1/4 step on each side.
If you want to do that, wouldn't the radius of the arc be a 1/4" and not a half?
As bborb points out, your I-5000 is swinging an arc of 1/2"... that won't fit your part.
John
The control is correct, your endpoint is NOT on the defined radius. You've defined a .5 inch radius with its center at X2.0 Z0.0
You've started the the G02 cut at X1.0 Z0.0
You've programmed the endpoint of the cut at X1.5 Z-.5
The endpoint doesn't lie on the programmed radius.
Here are examples of points that DO lie on your radius:
X1.0 Z0.0
X2.0 Z-.5
X3.0 Z0.0
X2.0 Z.5
X is diameter value, U is diameter value, I is radial value
Z is Z and W is W
Hi Andre'
I like using absolute X Y Z in my programming, I tried that first and thought I would try incremental U W to see if it made a difference. I am hoping it is an upside down issue where the G02 needs to be G03, I am going to try this tonight.
Thanks,
Steve
OK,
I might see this for the incremental answer, U-10000 with I=5000.
I will try this!
Thanks,
Steve
Posting Permissions
