cancel
Showing results for 
Search instead for 
Did you mean: 

Setting a 4-axis(XYZC) mill-turn postprocessor with Sinumerik 828D

Experimenter
Experimenter

Hello Everyone,

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?

5 REPLIES

Re: Setting a 4-axis(XYZC) mill-turn postprocessor with Sinumerik 828D

Phenom
Phenom

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.)

NX10.03
Windows 7 Pro

Re: Setting a 4-axis(XYZC) mill-turn postprocessor with Sinumerik 828D

Genius
Genius
Have you tried the new module "PostConfigurator." It is much more easy to get an correct Output for such a machine.

Re: Setting a 4-axis(XYZC) mill-turn postprocessor with Sinumerik 828D

Experimenter
Experimenter

Appreciate all of you help me on this issue!

Unfortunately my UG is ver9.0 thus unable to conduct PostConfiguratior for this issue. 

Re: Setting a 4-axis(XYZC) mill-turn postprocessor with Sinumerik 828D

Genius
Genius
If you have installed NX10 on your computer, you can use it for create and adjusting the post.
It should be run also in NX9

regards

Re: Setting a 4-axis(XYZC) mill-turn postprocessor with Sinumerik 828D

Experimenter
Experimenter

Hello, 

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 .

 

code:

N10 ;Operation : TST_C0
N20 DIAMOF
N30 GETD(C4)
N40 ;Tool Change
N50 G17
N60 SETMS(2)
N70 G0 C4=180.
N80 TRAFOOF
N90 G54
N100 D6
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.
N160 ;Cutting
N170 ;Retract Move
N180 X-10.071
N190 ;Departure Move
N200 G0 X-20.071
N210 Z-6.
N220 ;Approach Move
N230 X-10.071
N240 ;Engage Move
N250 G1 X-7.071
N260 ;Cutting
N270 ;Retract Move
N280 X-10.071
N290 ;Departure Move
N300 G0 X-20.071
N310 M2=5
N320 ;End of Program
N330 M30

 

image.png

Learn online





Solution Information