VERICUT Users' Forum

Svante

Senior Member

From: Trollhättan, Sweden

Registered: 2005-02-23

Posts: 60

Siemens 840D "TRANS"

Hi,
My name is Svante and I´m a new Vericut user. I have a problem with a CNC-program for a 5-axis rotary head Jobs241 with a Siemens 840D control. An example from the CNC-program looks as below:

N14238 SUPA D0 Z1050
N14239 S[1]=1700 M[1]=03
N14240 MSG ()
N14241 G00 X-460 Y0 Z900 C=DC(0) B0 D1
N14242 TRAORI(1)
N14243 G55
N14244 X-450 Z899 B92.5
N14245 G55
N14246 M18 M68
N14247 G04 F3
N14248 TRANS C12.000
N14249 EXTCALL("/_N_WKS_DIR/_N_PJBOPTI_WPD/_N_MSGRH5_SPF")
N14250 TRANS C36.000
N14251 EXTCALL("/_N_WKS_DIR/_N_PJBOPTI_WPD/_N_MSGRH5_SPF")
N14252 TRANS C60.000
N14253 EXTCALL("/_N_WKS_DIR/_N_PJBOPTI_WPD/_N_MSGRH5_SPF")

It is the TRANS that causes the problem - in the subprogram (which is repeated up to 15 times), there are usual C=DC() as CAxisMotion. Those values are between 358 and 2 degrees. Therefore I want the TRANS to behave like an modal offset. I have tested to use the "RotationPlane" macro but with no success. I also have tried to use the "SetAdditionalWorkCoord" and similar macros but I don´t know how to get the C-value inte the TRANS C12.000 block to update the offset.
This problem might have a simple solution, but since I am a new user I can´t find out.

Thanks!

/Svante

---

Svante Eriksson
System owner
GKN Aerospace Engine Systems Sweden
Vericut 7.2.1, 7.3.4, 7.4 - NX 9.0.3

Volkov

Member

From: St. Petersburg, Russia

Registered: 2004-12-15

Posts: 25

Website

Re: Siemens 840D "TRANS"

Are you sure you can use "C" register with TRANS command? I thought that TRANS just translates the work origin and not rotates.

Anyway try to use macros WorkCoordIndex (OVR=1),SetWorkCoord for TRANS word to set entry in Work Offset Tables window, and WorkCoordCValue for C word (with condition of TRANS in the block).

---

Regards.
Igor
www.bee-pitron.com

Svante

Senior Member

From: Trollhättan, Sweden

Registered: 2005-02-23

Posts: 60

Re: Siemens 840D "TRANS"

Thank you Igor for your answer! Unfortunately I failed with this TRANS-problem anyway. I didn´t understand how I should treat the WorkCoordIndex (OVR=1), that you mentioned first in your solution proposal. I did the way you described with the SetWorkCoord and the WorkCoordCValue macros. After that I did a few experimental variations from your solution. But - if I find out about the WorkCoordIndex it hopefully would help?!

The TRANS C command is used ( and works perfectly) in our Jobs241 with Siemens 840D control.

Regards Svante,

_____________________________
Svante Eriksson
VOLVO AERO
Dept. 9933  CAM-development
S-461 81 Trollhättan, Sweden

Tel:  +46 520 98825
Fax: +46 520 98590
E-mail: Svante.Eriksson@volvo.com

---

Svante Eriksson
System owner
GKN Aerospace Engine Systems Sweden
Vericut 7.2.1, 7.3.4, 7.4 - NX 9.0.3

Volkov

Member

From: St. Petersburg, Russia

Registered: 2004-12-15

Posts: 25

Website

Re: Siemens 840D "TRANS"

Sorry if my explanation was not clear.
If your TRANS command should update the work offset (e.g. G54-G57) then you use WorkCoordIndex, SetWorkCoord and WorkCoordCValue macros:

Here Override Value "1" means that work offset register 54 will be updated ("2" - for register 55, "3" - for 56...)

**********

If your TRANS command should rotate coordinate system immediatly then use RotationPlane2 and RotationPLaneAngle1 macros:

Note that RotationPlane macros require Advanced Machine Features license.

Hope it will help.

---

Regards.
Igor
www.bee-pitron.com