G18 problem with Highfeed V9

[Chris Flint Two Ft Pty Ltd]

I have encountered a programming problem this is the first time I have used "HIGHFEED" to post an elaborate surface machining program and during the program run it crashed the controller with an error saying "In G2-G3, 3rd Axis programmed without helical option" ???

H ere is a part of the program where it stopped:

G17 G71 G90 G40 M177

T8 M06

( 3/8 9.525MM BALL END CUTTER TOOL8 TOOL - 8 DIA. OFF. - 8 LEN. - 8 DIA. - 9.525 )

G0 X4.763 Y4.798 M40 M03 M23

D8 S18000

M03

M111

Z25.

Z-46.688

G1 Z-51.688 F2000.

X9.403 F500.

X14.043 F1000.

X18.683 F1500.

X23.324 F2000.

X27.964 F2500.

X32.604 F3000.

X37.244 F3500.

X41.885 F4000.

X134.69

X139.33 F3500.

X143.971 F3000.

X148.611 F2500.

X153.251 F2000.

G18 G3 X155.983 Y4.798 Z-52.55 R4.763 F1500.

 

It would "seem" from the crappy program manual that it might be looking for a G41/42 cutter compensation radius?? the tool is a 3/8th ball cutter.

Anyone out there know how to solve this as I cannot rerun the whole program to take out the highfeed which is a locked value.

thanks

chris f

[BernieT]

quote:

---

"In G2-G3, 3rd Axis programmed without helical option" ???

---

It sounds like your control does not have the Helix option turned on. This is a helical movement:

quote:

---

G18 G3 X155.983 Y4.798 Z-52.55 R4.763 F1500.

---

Also, your control may not recognize G18 or G19 helix moves even if the helix option is on.

 

In the filter options try turning off the XZ and YZ arcs or all arcs.

 

HTH Good luck.

 

I just reread your post, my filter suggestions won't work without regenerating the file. Hopefully you can figure out how to turn on the helix option in the control, if that is the problem.

[Chris Flint Two Ft Pty Ltd]

BernieT,

the heix option is on in the control and th controller can recognize G18, but it seems that the information regarding the G41/42 is also a requirement in that it seems not to know where the tool offset should be either left or right.

I cannot regen the file as I have been on an upgrade sim licence for testing ( I do not normaly have surfaces)and it was supposed to be renewed a few weeks ago bit it seems that someone is dragging their heels and it is not me, so I am screwed unless I can establish what other parameters to add by editing the existing gcode

[Greg Williams]

quote:

---

G18 G3 X155.983 Y4.798 Z-52.55 R4.763 F1500

---

quote:

---

the heix option is on in the control and the controller can recognize G18, but it seems that the information regarding the G41/42

---

Chris,

 

G18 may be turned on but can the controller cut a helix in that plane?

 

Does it accept this 2 aixs move?

G18 G3 X155.983 Y4.798 R4.763 F1500

 

or this 3 axis move?

G18 G3 X155.983 Y4.798 Z-52.55 R4.763 F1500

 

There is a big difference here.

 

I would guess that your controller will need

G18 G3 X155.983 Y4.798 Z-52.55 I4.763 K0.0 F1500

[Chris Flint Two Ft Pty Ltd]

No Greg Bob and I tried the I and J thing and that was completely unsuccessful.

I think that it needs:

G18 G41 ( or G42)G3 X155.983 Y4.798 Z-52.55 R4.763 F1500

but I don't know so I will call the USA at NUM tomorrow and see if they can assist.

thanks

chris

[Bruce Caulley]

Linearise helixes? I know you can't regen the file there, but maybe someone here could help?

 

Bruce

[Chris Flint Two Ft Pty Ltd]

Thanks Bruce, I am hoping Bob can get the USA off of their Ar$$es to solve this for the morning.

chris

[BernieT]

Look for this in your post processer:

code:

---

 helix_arc   : 1     #Support helix arc output, 0=no, 1=all planes, 2=XY plane only 

---

try changing it to

code:

---

 helix_arc  : 2       #Support ........ 

---

and repost the operation.

 

It's a good idea to make a copy of the post processer first in a serarate directory.

 

Good luck.