Now I get a "197 C-AXIS COMMANDED IN SPINDLE MODE" ALARM

[theemudracer]

Once again I am having problems. Hope you guys dont get tired of me asking questions.

The variables load into the macro page ok.
M43 engages the C-axis.

can you guys see what Im doing wrong??

here is the Macro
%
O9100(2.00 DIA MACRO CALL)
G01C[#1*.0174527]#26
M99
%


here is the part PRG.



G56
N39T0505(BALL END MILL)
N40G50M43
N41G0C0.
N42G97S4000M13
N43G0Z0.
G0X2.1
G98G01X2.F20.
G66P9100Z.0002A.0117
N56Z.0007A.0233
N57Z.0017A.0349
N58Z.003A.0466
N59Z.0046A.0582
N60Z.0067A.0698
N61Z.0091A.0814
N62Z.0118A.0929
N63Z.015A.1044
N64Z.0185A.1159
N65Z.0223A.1274
N66Z.0266A.1388
N67Z.0312A.1502
N68Z.0361A.1615
N69Z.0414A.1728
N70Z.0471A.184
N71Z.0531A.1952
N72Z.0595A.2063
N73Z.0663A.2174


thanks again
Jon

[dcoupar]

Jon,

Probably not causing that alarm, but in the macro:

G01C[#1*.0174527]#26 <-- missing "Z"?

When does the alarm occur? What Machine/Control?

Dave

[theemudracer]

Originally Posted by dcoupar Jon, Probably not causing that alarm, but in the macro: G01C[#1*.0174527]#26 <-- missing "Z"? When does the alarm occur? What Machine/Control? Dave

The Z and A are being passed to the macro page. I am wanting the C and Z axis to move at the same time. The Z# is in the main part prg.

The alarm occurs during the macro but after the variables are passed to the macro page. Im sorry I have posted two other times on this same subject so thats why I did not say what machine I had and such.

It is a Hyundai Kia SKT250MS Lathe with a fanuc 18-I TB with x,z,with a sub-spindle B. The main Chuck is the C axis and the Sub spindle chuck is A axis.


Thanks Jon

[dcoupar]

I understand what the macro does, but your post has:

G01C[#1*.0174527]#26

I'm not sure if this was a typo in the post or if that's what's really in the macro. My point was, I belive the line should be:

G01C[#1*.0174527]Z#26

...but I don't know if this relates to the alarm.

Have you programmed the live-tool with C-Axis on this machine before, or is this machine new to you? What happens if you activate both the "A" and "C" axes prior to running the macro? What happens if you use C instead of A to pass the variable to the macro, and #3 instead of #1 in the macro?

Sorry I can't be of more help... I don't know Kia machines.

[theemudracer]

Originally Posted by dcoupar I understand what the macro does, but your post has: G01C[#1*.0174527]#26 I'm not sure if this was a typo in the post or if that's what's really in the macro. My point was, I belive the line should be: G01C[#1*.0174527]Z#26 ...but I don't know if this relates to the alarm. Have you programmed the live-tool with C-Axis on this machine before, or is this machine new to you? What happens if you activate both the "A" and "C" axes prior to running the macro? What happens if you use C instead of A to pass the variable to the macro, and #3 instead of #1 in the macro? Sorry I can't be of more help... I don't know Kia machines.

I thought #26 was sufficent but it makes sense to have Z#26. Thanks...
All this macro stuff is new to me...


Yes I have programmed the live tool with the C-axis moving before on this machine, But it is still somewhat new to me. I have only been on this machine for 10 months and recieved 3 days of training on the fanuc controller. I have spent the last 10 years on a HMC with a Delta DynaPath controller and it is alot different than a fanuc.
I will try the other things you suggested Tue. when I return to work.

thanks
Jon

[Genguy]

I noticed the G98 prior to the macro call.
Does it need to use G99 (feed per revolution) instead?
Maybe that is the "spindle mode" error.

[M-man]

I think using M43 and G50 in the same block causes the alarm..

[theemudracer]

I will try both again when i get back to work.

In the past I have noticed it wont feed a live tool if you use a G99, because it does not sense any RPM from the main spindle I guess. Is this normal on a Lathe not to be able to use G99 with a live tool???

I will take the G50 out and try it.

thanks guys
Jon

[M-man]

G99 works with live tooling for me.. Do you have the rigid tapping option ?

[theemudracer]

Yes I have the rigid tap option on Live tooling,main and sub.

I can use G99 for rigid tapping on the live tools.

[theemudracer]

I got it working today thanks to all your guys help. I took out the G50 and put the Z in the macro and it took right off.

Thanks again.
Jon

[M-man]

Have you actually tested this prg?

This doesnt work on my 18It, I get a "quadrup macro call alarm, with g66 and with g65 it calls all the lines but doesnt call the sub other then the first line with g65... So, have you machined any with this yet?