CODE FOR "GO TO POINT"

[Flycut]

If anyone can help?

 

I know there is a code for fanuc controles that forces the machine to reach it's next point before reading the next line.

 

I don't even know if it's G or M code.

More so I need to know what the oppisite is.

 

What I'm trying to do is machine a contour that's made of hundreds of plines at 100 inches a minute

but my machine keeps stopping at every point, therefore never going more then 30 ipm.

 

This would cut my 10 minute cycle time in half and I have 1000 of these to make... so any help would be nice.

 

Tanks again guys.

[RNelson]

If my memory is correct:

G61 is exact stop

G64 cancel exact stop

[Psychomill]

quote:

---

If my memory is correct:

G61 is exact stop

G64 cancel exact stop

---

If G61 is on (or G60), this will stop at every point. If you shut it off (back to G64) you will probably lose some (or alot, depending) of accuracy at 100 ipm. At the very least, you may want to turn on "G8P1" (lookahead for accuracy, but won't stutter like G61). "G8P0" shuts this off.

 

HTH

[Flycut]

Thanks guys!

 

I don't think accuracy is a big concerne this time.

 

+/- .125" or something like that.

Will let you know how it works.

[Flycut]

 

Didn't work guys!

 

It's alot smoother, no more jerking, but my speed is still stuck at 35ipm.

 

Any other sugestions?

[Mike Whitten CAD/CAM Contractors]

Flycut,

 

What kind of machine is it? Does it have a "look ahead code" as mentioned earlier? HPCC? or any other high speed cutting modes?

 

Some machines simply can't process the data like this. There are a few work arounds for this though. The first thing that you need to do is filter the cut so that you can get more arcs in there. Hopefully this is possible. You may also need to work on the geometry a bit.

 

Mike

[Guest]

What kind of machine is this your are running?

[Psychomill]

If you don't need the accuracy, (at +/- .125 !! I wish I had those!) shut off 'lookahead'. 'G8PO' and/or G5P0 (although I think G8P0 should shut G5 off too).

 

And by the way (as we are all curious), what machine and controller are you using? Your 'stutter' may be the process speed of the control (if its old). The machine may be moving faster than the control can read it (especially if the splines are real tight).

 

[Flycut]

The machine is a Hardinge VMC1000.

Controle is Fanuc 0-Md.

 

It will accept G64 but won't speed things up.

The G8 stuff doesn't give me any alarms but don't seem to make a difference.

 

G05 gives me a 10 (invalid code alarm).

This was the first thing I tried.

 

Thanks for all the interest guys.

Didn't expect to get this much help.

[Lee.]

If your accuracy is that slack, why don't you convert the spline / s into arcs?

 

If you use a slack tolerance on that process, you should have way less code and be able to run really fast.

 

HTH

[Flycut]

I've tried converting the splines but only 50 of the 500 will convert and then my machine will still stop at the end of each arc!?!

[Lee.]

By any slim chance did you try looking to see if your running single block mode?

[Flycut]

You're joking right?

[Bob_Looney]

My initial guesstimate would be that the pline segments are too small for the control to read at 100 ipm and unless you can open up the pline tols and regenerate the code you're stuck.

in other words, if the segments are .001" and you're trying to go 100ipm, it's not going to happen unless you have a look ahead control that actually looks ahead and even then .001 segments at 100 ipm is faster than most controls can read.

[medaq]

On my fanuc o-m I use g62 right after the tool change. See how that does for you.

[Mike Whitten CAD/CAM Contractors]

flycut,

 

At this point, it may be a good idea to check the book out and/or call for tech support. There may just be an 800 number with someone that has an answer. As far as optimizing the code, we need to see the MC9 file. We are all at kind of a loss for data here.

 

Mike

[jeff]

quote:

---

I've tried converting the splines but only 50 of the 500 will convert and then my machine will still stop at the end of each arc!?!

---

This is a long shot,but will Xform/Squash help you convert these splines to arcs?

[BernieT]

Is your filter on and set to 'create arcs' with a 2/1 ratio and maybe .005 total tolerance???

 

[Craig Madsen from CM3D]

At 100ipm, if your control can process a line in the memory buffer in .005 seconds, that works out to a minimum move of .0083". SO, if your moves are shorter than this, your machine is getting to position faster than your control can process the next move.

 

Since you have such a large positioning tolerance available, you can do as BernieT just suggested, but I would open the total tolerance up to .01" and turn off the arc filter. If you have too large a tolerance with the arc filter on you may get random 'full circle' moves when your control tries to fit things together to compensate for errors in postition data.

 

Craig Madsen

[Mike Whitten CAD/CAM Contractors]

Craig,

 

quote:

---

If you have too large a tolerance with the arc filter on you may get random 'full circle' moves when your control tries to fit things together to compensate for errors in postition data.

---

Great info Craig. I am glad I don't have to find this one out the hard way now. At least if I do, I will know why. I did not realize that this could happen.

 

Thanks,

Mike

[Henk]

quote:

---

quote:

--------------------------------------------------------------------------------

If you have too large a tolerance with the arc filter on you may get random 'full circle' moves when your control tries to fit things together to compensate for errors in postition data.

 

--------------------------------------------------------------------------------

 

Great info Craig. I am glad I don't have to find this one out the hard way now. At least if I do, I will know why. I did not realize that this could happen.

---

Mike,

 

I found the hard way that MC some times create very short radiï in the NCI-file, these wil give in the NC-file arcs with startpoint-coördinate = endpoint-coördinate. That will result in an full arc move.!!

My reseller fixed that in my posts.

[Harryman]

How about posting a sample of the code you're running?

[Mike Whitten CAD/CAM Contractors]

Henk,

 

Thanks for the extra info!

 

 

Flycut,

 

Have you got it working now?

 

 

Thanks,

Mike