[D_Turner]

I only have NX experience with typical Fanuc controls. A friend of mine recently bought a used VMC with a Sinumerik 840D control so I am diving into the Siemens controls for the first time. I am helping him get it all figured out. We have most everything figured out at the machine, but I can't make a post processor work inside NX 7.5 for a Siemens.

I have used some of the examples in NX 7.5 including "mill_3axis_Sinumerik_840D_in" which is a preloaded post. It seems to work on the cycles like drilling(Cycle81/82/etc). The problem I am having is it does not do circular moves. I have a standard pocket with radius corners and the toolpath on the screen in NX looks good. I post process it using a Sinumerik post processor and it always comes out as linear xy moves. If I change to a fanuc post, including one I use at work all the time for a Mori Sieki....the moves are posted as circular G2/3 moves.

I have tried looking in postbuilder at this Sinumerik post and it has a Circular Move section under "Motion" that lists G2/3 moves, but the post never uses them.

So, my question....what I am I missing to make the generic Sinumerik posts do G2/3 circular moves? Just seems odd it posts fine using a Fanuc type post.

Thanks for any suggestions.




Sample piece of the code which should include circular arc engages and retracts, plus there are arcs in the corner of the pocket. Everything is just linear xy moves....

N1740 ;Approach Move
N1750 Z-.65
N1760 ;Engage Move
N1770 G1 Z-.75
N1780 X2.7519 Y-1.9161
N1790 X2.7124 Y-1.946
N1800 X2.6821 Y-1.9852
N1810 X2.663 Y-2.0309
N1820 X2.6575 Y-2.08
N1830 ;Cutting
N1840 Y-2.2892
N1850 ;Retract Move
N1860 X2.663 Y-2.3384
N1870 X2.6822 Y-2.3842
N1880 X2.7126 Y-2.4234
N1890 X2.7522 Y-2.4533
N1900 X2.7985 Y-2.4709
N1910 Z-.65
N1920 ;Departure Move
N1930 G0 Z.5
N1940 X2.7981 Y-1.8985

[markrief]

Have you tried creating a new post in Post Builder, and selecting Siemens 840D as the control?
This could give you a more up to date post than the sample.

[D_Turner]

Just tried that...created a new post using the Siemens 840D from the library. Went into NX and posted toolpath using this new post processor and still do not get circular G2/3 moves using a Siemens post. I guess it is something stupid I am missing, but so far I can't seem to figure it out. The toolpath postprocessed with a Fanuc control looks fine. My knowledge of Postbuilder is limited although I have did small edits to two posts for the Haas and Mori Seiki machines we have at work to fine tune a few machine specific things. First time ever messing with Sinumerik Controls.

Here is the difference in code using the same toolpath but two different post processors:

New Siemens 840D post created in Postbuilder(deleted some of the commenting the post does and extra garbage):
N400 ;Initial Move
N410 CYCLE832(_camtolerance,0,1)
N420 TRAFOOF
N430 G500
N440 G0 X3.4561 Y4.6527 Z.5 S0 D2 M3
N450 ;Approach Move
N460 Z-.09
N470 ;Engage Move
N480 G1 Z-.19 M8 F10.
N490 X3.4781 Y4.6971
N500 X3.4868 Y4.746
N510 X3.4824 Y4.7954
N520 X3.4652 Y4.842
N530 X3.4358 Y4.8818
N540 ;Cutting
N550 X3.2941 Y5.0343
N560 X3.2816 Y5.0451
N570 X3.2664 Y5.0514
N580 X3.25 Y5.0525
N590 X1.3591
N600 X1.3438
N610 X1.3306 Y5.052
N620 X1.3174 Y5.0533
N630 X1.3046 Y5.0566
N640 X1.2776 Y5.0527
N650 X1.2502 Y5.0525
N660 X1.0469
N670 X1.0366 Y5.0527
N680 X1.0266 Y5.0502
N690 X1.0175 Y5.0452
N700 ;Retract Move
N710 X1.0229 Y4.9964
N720 X1.0418 Y4.951
N730 X1.0717 Y4.9119
N740 X1.1107 Y4.882
N750 X1.1562 Y4.8631
N760 X1.205 Y4.8577
N770 Z-.09
N780 ;Departure Move


Same toolpath using "Mill 3 Axis" post:
%
N0010 G40 G17 G90 G70
N0020 G91 G28 Z0.0
:0030 T02 M06
N0040 G0 G90 X3.4561 Y4.6527 S0 M03
N0050 G43 Z.5 H02
N0060 Z-.09
N0070 G1 Z-.19 F10. M08
N0080 G3 X3.4358 Y4.8818 I-.1577 J.1014
N0090 G1 X3.2941 Y5.0343
N0100 G3 X3.25 Y5.0525 I-.0441 J-.0443
N0110 G1 X1.3591
N0120 X1.3438
N0130 G2 X1.3046 Y5.0566 I-.0001 J.1862
N0140 X1.2502 Y5.0525 I-.06 J.4305
N0150 G1 X1.0469
N0160 G3 X1.0175 Y5.0452 I0.0 J-.0625
N0170 X1.205 Y4.8577 I.1875 J0.0
N0180 G1 Z-.09
N0190 G0 Z.5
N0200 M02
%

[markrief]

The problem is probably that compressor is on - good for HSM, but not basic circular output.

To create a basic Siemens post, When you create a new post in PB, for the control select "SIEMENS" --> "Sinumerik_840D_basic". This will output circular.

If you want to modify your existing post, in PB go to Custom commands, edit set_Sinumerik_default_setting, and change this line:

set mom_siemens_compressor "COMPOF"; #COMPCAD/COMPOF

If that doesn't do it, please log a call with GTAC.

[D_Turner]

There is no "Sinumerik_840D_basic" in my Postbuilder version. Mine just has "SIEMENS" -> "Siemens - Sinumerik 840D". I don't see any "basic" options anywhere.

I found the line you mentioned in the Custom commands and changed it. That does the trick! It starts posting circular moves after that change. The line you mentioned shows up 3 times in the else/else if statements and I changed all three. Not sure if I really needed to change all three or not.

There is also another line in this custom command: "set mom_siemens_compressor "COMPCURV"; #COMPCURV/COMPOF"
I left this line alone.

Without taking much of your time as I am sure you are plenty busy with other stuff, but could you tell me what I did by changing COMPCAD to COMPOF? I like to understand what is happening so I begin to understand the way Postbuilder functions. What does Compcad and Compof stand for?

There are so many variables and such in these posts it seems overwhelming looking at these Siemens posts. Where is the best tutorials/description of PostBuilder? I can look on my NX DVDs tomorrow at work...there may be something there? As I stated earlier, this is the first time I have ever really tried using Postbuilder other than changing basic formatting of the output code so I am learning.

Thanks again for all your help! I think I may be on my way now...just need to edit a few simple things that are specific to the machine and we can start machining from NX!!

[markrief]

I am not sure why you don't see the additional controls in Post Builder - I assume you are using an older version.
We provide these different "flavors" so that you don't have to deal with all the variables.

To learn about this option, look for Compressor in the Sinumerik programming manual.