[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]

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]

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?

[theemudracer]

Yes I have cut with this prg but I had to make a few changes.
I changed the variable to C and still had the G66 in there. It would run the prg. but it would use the very first arguments I put in the macro on every line.
So I change it again and used G65 on every line so it would pass the values to the macro on every line. It is not very smooth when cutting, running a macro on every line but it did work.I dont have the final prg. here at home or I would post it . I will do it monday.

I have been talking to Wayne Myers, the designer of my cad/cam software.
He said there is a scale factor in the post processor that I can set to generate the right code for degrees of rotation. Then I dont have to run any macros and should end up with a much smoother running prg.

thanks
Jon

[M-man]

there are parameters that sets the control to highspeedoperation, as I understand, this will make the control smother when reading this kind of program.

[theemudracer]

here it is ...I lied I did bring it home this weekend...
%
O9100(2.00 DIA MACRO CALL)
G01C[#3/.0174527]Z#26
M99
%
.................................................. ....................

G56
N39T0505(BALL END MILL)
N40M43
N41G0C0.
N42G97S4000M13
N43G0Z0.
G0X2.1
G98
G01X1.99F800.




N1004G65P9100Z-.001C-.0126
N1005G65P9100Z-.0017C-.0383
N1006G65P9100Z-.0015C-.0491
N1007G65P9100Z-.0012C-.0598
N1008G65P9100Z-.0006C-.0704
N1009G65P9100Z.0002C-.0811
N1010G65P9100Z.0012C-.0913
N1011G65P9100Z.0024C-.1019
N1012G65P9100Z.0039C-.1123
N1013G65P9100Z.0056C-.1227
N1014G65P9100Z.0075C-.1329
N1015G65P9100Z.0094C-.143
N1016G65P9100Z.0117C-.1531
N1017G65P9100Z.0143C-.1631
N1018G65P9100Z.0169C-.1731
N1019G65P9100Z.0198C-.183
N1020G65P9100Z.0229C-.1926
N1021G65P9100Z.0262C-.2024
N1022G65P9100Z.0295C-.2121
N1023G65P9100Z.0333C-.2216
N1024G65P9100Z.0371C-.2309
N1025G65P9100Z.0412C-.2402
N1026G65P9100Z.0453C-.2494
N1027G65P9100Z.0497C-.2584
N1028G65P9100Z.0543C-.2676
N1029G65P9100Z.059C-.2764
N1030G65P9100Z.064C-.2852
N1031G65P9100Z.0691C-.2939
N1032G65P9100Z.0743C-.3025
N1033G65P9100Z.0796C-.3109
N1034G65P9100Z.0853C-.3192
N1035G65P9100Z.0911C-.3274
N1036G65P9100Z.0969C-.3354
N1037G65P9100Z.1031C-.3435
N1038G65P9100Z.264C-.2178
N1039G65P9100Z.2606C-.2131
N1040G65P9100Z.2569C-.2083
N1041G65P9100Z.2536C-.2035
N1042G65P9100Z.2505C-.1986
N1043G65P9100Z.2472C-.1937
N1044G65P9100Z.2442C-.1887
N1045G65P9100Z.2412C-.1835
N1046G65P9100Z.2382C-.1783
N1047G65P9100Z.2355C-.1731
N1048G65P9100Z.2327C-.1677
N1049G65P9100Z.2303C-.1624