Divide By Zero

[Simoneau]

Im running X2 and am getting an Divide by Zero alarm on the Haas mill, has any one had this problem? Haas tells me its something to do with cutter comp, but I dont feel thats the problem since I have been programing the same way for years and no problem.

[Thad]

What type of toolpath? What diameter tool? What type (perp/tangent) and lenth of leadin/out? What type of comp?

 

More info would help.

 

Thad

[Simoneau]

[Brad MacKinnon]

Is there anything in your offset register on the controller ?

 

Edit: after looing up the alarm I dont see how it could be a comp problem either

[Simoneau]

the machine is clear of all offsets.

[Thad]

Do you always turn wear comp on with a tangent move? Perp is a better idea.

 

Thad

[?Mark]

quote:

---

Do you always turn wear comp on with a tangent move? Perp is a better idea.

---

He has a line in there, so all is good (line and then tangent arc...just the way I use it)

I don't see anything wrong with his setup.

What's your tool dia?

[Thad]

Oops, didn't see the arc.

 

Thad teh needs his eyes checked

[Simoneau]

I will try the perp. instead and see if that works.

[Simoneau]

tool is a .5 em

[?Mark]

quote:

---

Haas tells me its something to do with cutter comp

---

Ask them again, could very well be a control issue especially if it worked before.

Is there a sample code you can share that's giving you a problem?

[Simoneau]

heres a simple contour program its doing it on.

 

 

G20

G0 G17 G40 G49 G80 G90

( .498 UNIVERSAL EM )

T2 M6

M01

S4280 M3

G0 G90 G54 X.3587 Y.3476

G43 H2 Z.25

M8

Z.1

G1 Z.01 F27.

G3 Y.3477 Z-.072 I-.0719 J.2383

Z-.154 I-.0719 J.2383

X.5358 Y.586 Z-.1707 I-.0719 J.2383

X.2868 Y.835 Z-.1911 I-.249 J0.

X.0378 Y.586 Z-.2117 I0. J-.249

X.1737 Y.3642 Z-.226 I.249 J0.

G1 X.17 Y.357

Y-.2642

G3 X.2663 Y-.257 I-.044 J1.2452

X.274 Y-.064 I-2.4384 J.1931

X.2384 Y.3517 I-2.446 J0.

X.17 Y.357 I-.0724 J-.4907

G2 X.2067 Y.3185 I-.8933 J-.8879

X.2496 Y.3631 I1.4061 J-1.3081

G1 X.2748 Y.514

G3 X.166 Y.523 I-.1088 J-.653

X.004 Y.5029 I0. J-.662

G1 Y-.4257

G3 X.126 Y-.431 I.122 J1.4067

X.2992 Y-.4203 I0. J1.412

G1 X.2993

G3 X.4183 Y-.4005 I-.1733 J1.4013

X.44 Y-.064 I-2.5903 J.3364

X.3812 Y.4871 I-2.612 J0.

X.2748 Y.514 I-.2152 J-.6261

G1 X.3293 Y.8415

G3 X.166 Y.855 I-.1633 J-.9805

X-.328 Y.7236 I0. J-.994

G1 Y-.7029

G3 X.126 Y-.763 I.454 J1.6839

X.3399 Y-.7499 I0. J1.744

G1 X.34 Y-.7498

G3 X.5535 Y-.7098 I-.214 J1.7308

X.7387 Y-.5058 I-.061 J.2414

X.772 Y-.064 I-2.9107 J.4418

X.6949 Y.6054 I-2.944 J0.

X.5482 Y.7786 I-.2425 J-.0566

X.3293 Y.8415 I-.3821 J-.9176

G0 Z.25

M9

G0 G40 G80 G49

G53 Z0 M5

G53 Y0

G54 X0

M30

%

[Thad]

code:

---

G3 Y.3477 Z-.072 I-.0719 J.2383

---

The parallel axes are XYZ and IJK. It looks like they're getting mixed somehow. In other words, it should be outputting a J and K value, not I and J. It may be even safer to allow arcs only in the XY (G17) plane.

 

Thad

[Midwest]

quote:

---

G0 G90 G54 X.3587 Y.3476

G43 H2 Z.25

M8

Z.1

G1 Z.01 F27.

G3 Y.3477 Z-.072 I-.0719 J.2383

---

Changed the Y.3477 to Y.3476 and runs fine

 

 

G0 G90 G54 X.3587 Y.3476

G43 H2 Z.25

M8

Z.1

G1 Z.01 F27.

G3 Y.3476 Z-.072 I-.0719 J.2383

 

 

HTH

 

 

[Midwest]

Try the free mpmaster for a post for the Haas if you are having trouble

 

mpmaster post found here

 

 

[Thad]

quote:

---

Changed the Y.3477 to Y.3476 and runs fine

---

I'm not sure how it can, Midwest. An arc with a YZ endpoint must have JK arc center. His programs are outputting and IJ arc center.

 

Perhaps your change was enough to make the error go away at the control, but I'd be willing to bet that if you actually ran that program, you'd be unhappy with the results in the workpiece.

 

Thad

[Midwest]

Didn't watch the path in the machine to close.........it was ramping into the cut. I didn't get and error until I ran the program, the cutter path ran on the screen just fine, I thought this was strange. The path seemed to be a pocket toolpath on the screen. Maybe Jason can put the file on the FTP.

 

 

I'll run it in the Haas again tomorrow when I get a chance.........may not be right away.......kind of busy.

 

 

[pip]

G3 Y.3477 Z-.072 I-.0719 J.2383

Where is the X for this move. It looks like a helix down into the job, but no X. This used to trip our old bridgeport out. Think we changed the post..

Try puting in the X coord. Might help..

[Roger Peterson]

Hey Jason you can send me a zip to go and I'll take a look at it. But it looks like the problem is that your first G03 arc has only a .0001" move in Y. Most posts by default will linearize any arc that is less than .0005". The min arc value is in your control def on the tolerances page, and arc length check must be enabled on the arc output page.

 

 

HTH

[Midwest]

quote:

---

ramping into the cut

---

I mean helix.......

 

 

Ran on the Haas again the helix is a little smaller than the pocket it is cutting.

 

[Thad]

I thought this was a 2D contour toolpath?!?!? I give up.

 

Thad

[Simoneau]

I meant to send a 2d contour but apperently I sent the pocket with helix instead, that program still didnt work.

Roger, I will send the file over and have you look at it.

 

Thanks