My machine is a 4-axis(XYZC) mill-turn machine with Siemens Sinumerik 828D controller installed.
While building its corresponded postprocessor, I found it difficult to get correct post combination.
I try to follow some toturials from forum. Firstly I choose XZC mill-turn as a main post, then link it with a turn post plus a x-head side spindle post. However, the XZC mill-turn config is not selectable for Sinumerik 828D. Then I try to choose 4-axis with rotrary table, but it shows an error "4th axis C table not allowed".
The situation really confuses me and delay my progress in UG CAM application. Appreciated if somebody experienced in this territory could teach me how to proceed it correctly?
Solved! Go to Solution.
I would think that you are right to have an XZC and a lathe post. I am not sure what you mean by side head. XZC will not work for tool vectors that are not along Z - so if you need live milling in this orientation - that will be a third kin configuration. Still another could be "TRANSMIT" style milling (virtual Y - converted by the control.) I think the first step would be to get all the individual posts doing what you want - then think about linking them. There is an alternative way of doing multi kinematic posts that siemens examples switched to as of late. The switch kinematics with kin vars and set up some block templates with check code. Look at the SIM example posts. The XZC post is a combination of kin settings (which linearize) and some tcl routines which are needed as well. Another option is using the lock axis routines for a similar effect to XZC. I am not very familiar with Siemens models other than 840d so not sure whether using that one matters (as a post template.)
Appreciate all of you help me on this issue!
Unfortunately my UG is ver9.0 thus unable to conduct PostConfiguratior for this issue.
A little bit late, but,...
try to post with tge postprocessor "sim15_millturn_9ax_sinumerik_mm" from folder:
C:\Program Files\Siemens\NX 11.0\MACH\resource\library\machine\installed_machines\sim15_millturn_9ax\postprocessor\sinumerik
You will get just the code that you want with the tool ax in X direction and the plane for circle interpolations G19 .
N10 ;Operation : TST_C0
N40 ;Tool Change
N70 G0 C4=180.
N110 G19 G0 G90 X20.071 Z-.003 S2=0 D6 M2=3
N120 ;Approach Move
N130 X-10.071 C4=0.0
N140 ;Engage Move
N150 G94 G1 X-7.071 M8 F250.
N170 ;Retract Move
N190 ;Departure Move
N200 G0 X-20.071
N220 ;Approach Move
N240 ;Engage Move
N250 G1 X-7.071
N270 ;Retract Move
N290 ;Departure Move
N300 G0 X-20.071
N320 ;End of Program