Results 1 to 14 of 14
01-02-2008, 11:18 AM #1
Whats more accurate, R or I,J for arcs??
Does anyone know if using I and J values for arc moves is more accurate than just using R value,, this is on a Hardinge VMC1000 with an OM D control,, I do mostly aluminum parts and when running at higher feed rates there seems to be a bit of deviation from the programmed path,,Is there a parameter that can be changed for more block look ahead possibly or for tightening up the accuracy?
01-02-2008, 02:21 PM #2
Are you using G8? This made a world of difference for me when feeding anything over 30IPM. (BDPT XV 710 w/OMc control)
My software post spits out I's and J's and I don't seem to have any accuracy problems. But I use R's on my Hardinge turning center because I pretty much hand program and it's easier.
01-02-2008, 02:37 PM #3
There shouldn't be much difference between using an R or an I/J. But, if the arc is 180 degrees or greater, then I and J will give better results at high speed as only one line of info needs to be processed.
You can have the servos tuned to provide better performance. There are a variety of companies that perform this service. You might start by asking you local machine dealer or Hardinge for a recommendation.
01-02-2008, 03:32 PM #4
I don`t have G8 listed in the machine manual,, is it similar to G61 exact stop code?
01-02-2008, 04:17 PM #5
According to my Oi-MC manual:
"G08 is designed for high-speed precise machining. With this function, the delay due to acceleration/deceleration and the delay in the servo system which increase as the feedrate becomes higher can be suppressed."
"The tool can then follow specified values accurately and errors in the machining profile can be reduced."
G08 P2: turns off the function
Plug in the line: G08 P1; before your Z clearance move and see what happens. If the function is available on your control, it'll be a good thing. But then again, it's not in your manual so it may not be an option.
I wonder if G08 and G61 can be executed concurrently? I've never used G61.
Because I machine mostly superalloys and stainless steels, I'm pretty much a novice when it comes to high-speed machining. So maybe somebody with more experience can shed some light.
01-02-2008, 04:41 PM #6
If i understand G08 (high speed function), what it does is ignore the following error, opening up what is normally a closed-loop system. That is, if your machine has it turned on. I'd see about making sure its on, from Hardinge. I think G61 (positioning mode) would be useless if G08 is used. It waits for the feedback to be within a certain window before the next block is processed.
As far as the I,J,K versus the R, I don't think there's any difference, because they both use the X squared plus Y squared equals R squared equation for a circle. The calculation would depend on the number of decimal places used in the equation, and I'm sure its more than four decimal places.
Just if you use R for an arc greater than 180°, then you have to use an R minus value.
Many people would rather use a I, J or K for an arc of 360°
01-02-2008, 05:21 PM #7
Thanks for the quick replies,, I will do a bit of testing tomorrow if the G8 works or not,, the control doesn`t alarm when its entered in MDI so hopefully the control has the option,,
01-02-2008, 06:06 PM #8
I prefer using IJK as you will get a true arc. XYZ endpoint must be within .0002 (parameter setting) using I, J, & K or you get an alarm. Just about any endpoint works with an R.
Try G0G90X0Y0; G2X10.Y0R1.F?? Watch what happens!
01-02-2008, 07:30 PM #9
Your example on the HAAS results in "Invalid R in G02" message.
Don't know about Fanuc, but on Haas R and I/J must obey the very same accuracy setting, default is .001.
If your start end endpoints are correct, with the given I/J or R values the block must be resolveable with identical results.
Remember, the G-code is interpreted and the motion control receives the very same instructions to complete the block, regardless of how it was defined in the program.
As for me, I use R for less than 360 arcs, I/J for full circles when programming by hand.
In CAM it's I and J always.
01-02-2008, 08:36 PM #10
Thanks, I was not sure about the Haas, Fanuc will accept the command, it's pretty interesting to watch the result! I am in the habit of using IJK, even on a 90* corner.
01-03-2008, 02:17 AM #11
HessTool : sent you a PM.
01-03-2008, 10:36 AM #12
01-03-2008, 11:10 AM #13
I remember that kind of thing happening occasionally on an Okuma lathe with OSP2200 control (vintage ~1979). It used I and K exclusively, and was a very sophisticated control for the time.
That sucker would throw up an alarm if I rounded a tenth in the wrong direction, but once in a great while would happily try to make the arc if I had added an extra digit by mistake - as in I16.0 instead of I1.0.
One time the setup guy came into the office and asked me why one block had been cutting air for twenty minutes with a new program. Who knows what the control was "thinking"?
Software For Metalworking
01-03-2008, 12:15 PM #14
handprogrammed- i've tried this many times at VMC Fanuc 0im with Al material also.. 90 degree-cornering;
G03 X_ Y_ R_
G02 X_ Y_ R_
don't specify F for this block..