Cancel
Showing results for 
Search instead for 
Did you mean: 

No CYCLE 800 output for 45 degree head table 5 axis post

Pioneer
Pioneer

In my Sinumerik 840D post for machine 45 degree head (B-Axis) table (C-Axis) , I carriedout a drilling operation. But I don't get any output inform of CYCLE 800 rather I get it in form of AROT Y, AROT Z. Why so? What setting do I need to change?

 

N10 ;Start of Program
N20 ;
N30 DEF REAL _camtolerance
N40 DEF REAL _X_HOME, _Y_HOME, _Z_HOME, _B_HOME, _C_HOME
N50 DEF REAL _F_CUTTING, _F_ENGAGE, _F_RETRACT
N60 ;
N70 G40 G17 G710 G94 G90 G60 G601 FNORM
N80 ;Start of Path
N90 _camtolerance=.06
N100 _X_HOME=999999.9 _Y_HOME=999999.9 _Z_HOME=999999.9
N110 _B_HOME=0 _C_HOME=0
N120 ;
N130 ;Operation : SPOT_DRILLING
N140 ;
N150 TRAFOOF
N160 SUPA G0 Z=_Z_HOME D0
N170 SUPA G0 X=_X_HOME Y=_Y_HOME B=_B_HOME C=_C_HOME D1
N180 ;First Tool
N190 T="DRILLING_TOOL"
N200 M6
N210 MSG("DRILL_METHOD")
N220 TRAFOOF
N230 SUPA G0 Z=_Z_HOME D0
N240 SUPA G0 X=_X_HOME Y=_Y_HOME B=_B_HOME C=_C_HOME D1
N250 ;Initial Move
N260 G0 B180. C270.
N270 TRAORI
N280 G54
N290 AROT Y90.
N300 AROT Z90.
N310 G0 X0.0 Y170. Z-50. S2122 D1 M3
N320 ;Cutting
N330 G1 Z50. F424.
N340 ;Retract Move
N350 G0 Z-50.
N360 ;End of Path
N370 TRANS X0 Y0 Z0
N380 TRAFOOF
N390 SUPA G0 Z=_Z_HOME D0
N400 SUPA G0 X=_X_HOME Y=_Y_HOME B=_B_HOME C=_C_HOME D1
N410 M5
N420 ;End of Program
N430 M30

9 REPLIES

Re: No CYCLE 800 output for 45 degree head table 5 axis post

Legend
Legend

Hello

 

It seems that you work with PostConfigurator. There is an setting where you can switch between CYCL800 and AROT.pc.png

Re: No CYCLE 800 output for 45 degree head table 5 axis post

Gears Phenom Gears Phenom
Gears Phenom

It is a little bit hard to find / reprogramed something what was programmed by somebody else.

I would suggest to built own postprocesor by Postbuilder from generic template postprocessor.

If you create good base of custom commands,  templates and logic the result can be quite flexible powerfull postprocesor.

 

 

---------------------------------------------
#♫ PB, 5ax, itnc, nx, vericut ♫ #

Re: No CYCLE 800 output for 45 degree head table 5 axis post

Pioneer
Pioneer

No, I didn't use Post Configurator. I have made it from postbuilder.

Re: No CYCLE 800 output for 45 degree head table 5 axis post

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

If you made this post using the Siemens 840D controller template, then (sarcasm on) good luck on your hunting expedition.(Sarcasm off)

I find posts made with this template so obtuse, obscure, or obfuscated that it is just not worth using that template.  (Note I just counted up and I have over 150 PUI files for posts, so it's not like I don't know what I'm doing in Post Builder)

 

For example, one post I made using the Siemens template defined the type of cutter comp (CUT2DF) *4* different places in *3* different procs.  *NONE* of which were in the "cutcom on" event.  How the *** am I supposed to understand how to edit that?

 

For Siemens control posts, I start with a "generic" control, then add what *I* want for the Siemens stuff (you can use your existing post as a mine to steal code from, e.g. calculating Euler angles, but IMHO thats about all it is good for).

 

Sad but true...

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled


Re: No CYCLE 800 output for 45 degree head table 5 axis post

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Hi, @rudra_1005!

You problem is too easy to fixed.

1. In your postprocessor kit you have a cdl-file. Attach all statement from this file to your default ude.cdl, user_defined_events folder. The best way to do it - INCLUDE, like here

 rudra1.png

# UDE.CDL
##########################################################################
#
#   PURPOSE:
#
#      This file is used in the conversion of post commands contained
#      in pre UG V15.0 part files into User Defined Events.
#
##########################################################################
#
#
#

MACHINE FANUC


# Remove the # from the INCLUDE statement to enable Siemens 840D cycle parameters to Hole Making and Manual Holemaking operations.
INCLUDE {$UGII_CAM_USER_DEF_EVENT_DIR/DMC_160U.cdl}


#---------------------------------------------------------------------------

 

2. Restart NX

 

3. Create any 3+2 operation, with fixed tool axis, like here

 

rudra1.png

4. Add Start Event for your operation Siemens Sinumerik 840D

rudra_2.pngAnd set Swiweling type for operation

 

rudra_3.png

 

THATS ALL

 

Postprocess it

 

N290 TRAFOOF

N300 SUPA G0 Z=_Z_HOME D0

N310 SUPA G0 X=_X_HOME Y=_Y_HOME A=_A_HOME C=_C_HOME D0

N320 ;First Tool

N330 T="MILL"

N340 M6

N350 MSG("METHOD")

N360 TRAFOOF

N370 SUPA G0 Z=_Z_HOME D0

N380 SUPA G0 X=_X_HOME Y=_Y_HOME A=_A_HOME C=_C_HOME D0

N390 ;Initial Move

N400 CYCLE832(_camtolerance,0,1)

N410 TRAFOOF

N420 G54

N430 CYCLE800(1,"R_DATA",0,57,0.,0.,0.,45.,0.,-180.,0.,0.,0.,-1,1.)

N440 G0 X44. Y83.246 Z77.175 S0 D0 M3

N450 ;Approach Move

N460 Z70.175

N470 ;Engage Move

N480 G1 Z67.175 F250.

N490 Y80.246

N500 X44.175 Y78.686

N510 X44.778 Y77.231

N520 X45.736 Y75.982

N530 X46.985 Y75.024

N540 X48.439 Y74.422

Re: No CYCLE 800 output for 45 degree head table 5 axis post

Pioneer
Pioneer

errr.png

 

 

getting this error while editing the file "ude.cdl" in "C:\Program Files\Siemens\NX 10.0\MACH\resource\user_def_event" folder

Re: No CYCLE 800 output for 45 degree head table 5 axis post

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom
Copy this file to any folder where you can edit it and then copy back. Win ask you Replace? Yes.

Re: No CYCLE 800 output for 45 degree head table 5 axis post

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom
Or do it as Administrator. Or ask your sysadmin. Or Bill Gates.....

Re: No CYCLE 800 output for 45 degree head table 5 axis post

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

Blame those who create malware, which in turn results in more protection for installed software.

Generally changing anything in the NX installation folder is bad practice, since any update will reverse your changes.

Use the NX_Custom template listed in the "Programming and Customization Forum" for a single point customization.

Stefan Pendl, Systemmanager CAx, HAIDLMAIR GmbH
Production: NX10.0.3, VERICUT 8.1, FBM, MRL 3.1.7 | TcUA 10.1 MP7 Patch 0 (10.1.7.0) | TcVis 11.4
Development: C (ITK), .NET, Tcl/Tk Testing: NX12.0 | AWC 3.4 Preparing: NX12.0

Employees of the customers, together we are strong Smiley Wink
How to Get the Most from Your Signature in the Community
NX Customization - Best Practice Guide

Learn online





Solution Information