Cancel
Showing results for 
Search instead for 
Did you mean: 

Post Builder, G99 is being swapped with G98

Solution Partner Genius Solution Partner Genius
Solution Partner Genius

Hello,

 

The drill cycle return is currently G98, which is fine, but the G99 option is missing. I was trying to activate it in the post by turning on the G99 return (Manual/Auto) in the event for drilling cycle.

 

image004.png

 

It shows G99 here, but is postign G98. I must be missing something.

 

And here is the expression defining it:


image001.png

 

Not sure where to look next or how to troubleshoot. Any ideas would be greatly appreciated.

 

Thanks!

 

15 REPLIES 15

Re: Post Builder, G99 is being swapped with G98

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

hi,

hole making  -  G98/99 is switched automatically when it is needed.

depends on tool path.

expreson you are showing is correct.

 

---------------------------------------------
#♫ PB, 5ax, itnc, nx, vericut ♫ #

Re: Post Builder, G99 is being swapped with G98

Solution Partner Genius Solution Partner Genius
Solution Partner Genius
Is there a way to manually override? Or is G98 just the correct

Re: Post Builder, G99 is being swapped with G98

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

this is good video how g98/99 works

https://www.youtube.com/watch?v=YbbZJ7H0NUw

 

And here you are some examples that should be correct:

1.

aa.JPG

N13 G40 G00 X40. Y-40.
N14 G43 Z10. H1
N15 G98 G81 X40. Y-40. Z-43.004 R-17.5 F#104
N16 Y40.
N17 G80
N18 G00 Z10.
N19 X10. Y.75
N20 G81 Z-23.004 R2.5
N21 X-10.
N22 X-40. Y-40. Z-43.004 R-17.5
N23 Y40.
N24 G80

 

2.

bb.JPG

N13 G40 G00 X40. Y-40.
N14 G43 Z10. H1
N15 G99 G81 X40. Y-40. Z-43.004 R-17.5 F#104
N16 G98 G81 X40. Y40. Z-43.004 R-17.5
N17 G80
N18 G00 Z10.
N19 X10. Y.75
N20 G99 G81 Z-23.004 R2.5
N21 G98 G81 X-10. Y.75 Z-23.004 R2.5
N22 G99 G81 X-40. Y-40. Z-43.004 R-17.5
N23 G98 G81 X-40. Y40. Z-43.004 R-17.5
N24 G80

 

3.

ccc.JPG

N14 G43 Z10. H1
N15 G99 G81 X40. Y-40. Z-43.004 R-17.5 F#104
N16 G99 G81 X40. Y40. Z-43.004 R-17.5
N17 G80
N18 G00 Z4.
N19 X10. Y.75
N20 G99 G81 Z-23.004 R2.5
N21 X-10.
N22 G99 G81 X-40. Y-40. Z-43.004 R-17.5
N23 G98 G81 X-40. Y40. Z-43.004 R-17.5
N24 G80

 

Dont forget cycle plane change - it is important (xy-z, z-xy and what you have in z.)

 

cheers

---------------------------------------------
#♫ PB, 5ax, itnc, nx, vericut ♫ #

Re: Post Builder, G99 is being swapped with G98

Phenom
Phenom

@Juraj Thanks for the info.

 

Can you please share the cycle plane change command? I do not see it in the custom_command dir. 

 

I set the "initial" and "final retract" in drilling. This something I usually don't do and usually leave the retracts set to "Clearance - Tool Axis"

 

Anyway... my post outputted G99 and snapped off a tool. I had been using this post with no issues for years so I was a bit surprised. 

 

 

Dont forget cycle plane change - it is important (xy-z, z-xy and what you have in z.)

 

 

 

N42518 G54.1P4
N42519 M8
N42520 S1299 M3
N42521 G0 G90 A0.0 C0.0
N42522 M131
N42523 X2.7735 Y-1.893
N42524 G43 H268 Z7.9985
N42525 G81 G99 X2.7735 Y-1.893 Z4.7985 R4.9985 F3.377
N42526 G81 G99 X-1.1701 Y-1.3757 Z4.6075 R4.8025
N42527 X-1.8849 Y-.8493
N42528 G81 G99 X-3.5925 Y1.9938 Z5.7425 R5.9425   <<<<<<<<<<< CRASH!!!!!!!!!!
N42529 G81 G98 X2.7735 Y2.437 Z4.7985 R4.9985
N42530 G80
;

Glenn Balon
Production: NX 12.0.2 MP10 Primarily CAM

Re: Post Builder, G99 is being swapped with G98

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom
Cycle plane change is not a custom command. It is a section in canned cycles. It is good if tool is going to drill on higher level. So you can prepare blocks there to get tool higher before cycle is executed on XY and so on.
---------------------------------------------
#♫ PB, 5ax, itnc, nx, vericut ♫ #

Re: Post Builder, G99 is being swapped with G98

Phenom
Phenom

I see it now, but what do you place in there to get it to retract if the next move is higher in Z?

 

I am using Fanuc code. 

Glenn Balon
Production: NX 12.0.2 MP10 Primarily CAM

Re: Post Builder, G99 is being swapped with G98

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Hi,

hope I understand well ,

I recommend to have there these :

 

1.G80

2. Z, cycle rapid to pos  (*better is cycle retract to pos of previous hole - so ou can save it in every cycle execution)

3. X, Y, cycle rapid to pos

4.then force G_motion and so on .... to set full drilling cycle again

 

And take a look in my comments above examples of nc code.

 

cheers

 

---------------------------------------------
#♫ PB, 5ax, itnc, nx, vericut ♫ #

Re: Post Builder, G99 is being swapped with G98

Legend
Legend

It's Buggy...

 

For Holemaking... Until NX12 or 12.01

The "Retract Output Mode" was not in the dialog box and had to be customized in.

 

Now that it's added you have (3) options, IMO it's...

(Clearance initial) G99 first hole, then Cancel at level change or obstacle, re-issue, G98 the remainder

(Always) G99, crash crash crash, G98 the last hole (but tool path on the screen will appear good)

(Clearance Only) G99. Cancel when level changes, Hop over obstacles and re-issue drill cycle at all level changes and hops

 

Maybe it's how my post is set-up... but it's all my post to date

 

Pre-NX12 if you have not customized in "Retract Output Mode" you may get good looking path clearance... on the screen, but bad G-code output.

You can prove this with a OTB machine, as I did while making an enhancement request to have "Retact Output Mode added to the dialog box. I'm not sure what it is defaulting to when not there, but I'm assuming it is "Always"

 

I have a a few broke tools until I came up with the solution below...

 

(Pre-NX12) I go into the templates, customize in "Retract Output Mode"  and set it to "Clearance only" with a transfer motion between features set as "lowest safe Z" value .100, no more issues. path on screen and machine behavior are the same. I get a bunch of cycle outputs when levels change or hop over obstacle... but no shattered tools.

In NX12, I do the same you just don't have to do the customize in portion

 

This is also the same behavior I would see in PTP when doing multiple avoidance moves in a hole set or series when clearance is set to "None"

 

Capture.JPG

 

You can read the help I don't think it quit aligns to what really happens, I'd advise to prove it for yourself, see how your post behaves.

I think the fix would be that the Option "Always"... should be G98... Always.

Which is why I think your are saying it seems reversed, I agree

{Paul Schneider}, {CNC Programmer}, {DRT-Rochester}


Production: {NX11.0.2,MP5, NX12.0.2, MP4}

Re: Post Builder, G99 is being swapped with G98

PLM World Member Phenom PLM World Member Phenom
PLM World Member Phenom

Do you have the G_return code set to (Auto/Manual)

g98-99.JPG

John Joyce, Manufacturing Engineer,
Senior Aerospace

NX 11.0.2.7 Vericut 8.0.3 - Statements and opinions are mine alone and do not reflect
the opinion of my employer or any other member of the human race

Learn online





Solution Information