Apply pressure on axisymmetric elements

Altair Forum User

Hi,

I'd like to apply a pressure load on a fully axisymmetric pipe which I modelled with CTAXI Elements and the property PAXI.

In the picture below, you can see the crossection of the vertical pipe, on the left side the meshed region and on the white line I'd like to apply a pressure.

 

Error message:

  'PLOAD          2    25.0     473     475       0'
 
 *** ERROR # 1000 *** in the input data:
 Incorrect data in field # 6.

 

Is it not possible to use pressure loads in combination with axisymmetric elements in optistruct?

 

 

Thank you

Girish Mudigonda_21018

Try PLOADX1 instead of PLOAD. PLOADX1 is used to apply pressure load on axisymmetric element.

 

 

Altair Forum User

Hi,

I only got these 4 load types to chose from?!

Rahul Rajan_21763

Apply it via bulk unsupported card.See attached screenshot.

<?xml version="1.0" encoding="UTF-8"?>

<?xml version="1.0" encoding="UTF-8"?>

Altair Forum User

Thank you very much Mr. Rajan, I managed to apply the pressure and passed a static analysis without errors.

My goal is a geometrical nonlinear analysis though and here I get my next error:

 

*** ERROR # 4012 ***
 Element type CTAXI (EID = 1) is not supported in NLGEOM, IMPDYN and 
 EXPDYN subcases.
 
 *** Run terminated because of error(s) in the input data.

 

I also tried to update the used CTAXI elements to CTRIAX6 ones but then I get the following error:

 

*** ERROR # 1449 *** in the input data:
 Nastran style CTRIAX6 elements cannot be mixed together with
 OptiStruct CTAXI elements or PAXI properties.
 Please use HyperMesh to convert the deck.

 

The help files says that both CTAXI and CTRIAX6 are used for linear simulations. Is it still possible to do a geom. nonlinear axisymmetric analysis?

 

I also got a question considering the CTRIAX6 elements. The Help tells me that they can also be used for axisymmetric analysis, which property do I have to use with them though? PAXI only supports CTAXI elements.

 

Again, thank you very much.

Girish Mudigonda_21018

OS doesn't support axisymmetric elements for nonlinear analysis yet.

 

Also CTRIAX6 doesn't need a property card. Material ID can directly be assigned to the element.

Altair Forum User

Hi, Girish, thanks for your reply.

I now tried to model 1/4 of the model with solid elements and the simulation finishes without errors.

 

In a next step I'd like to apply an axial force by using a rigid element. The rigid master node is in the center of the tube and connected with the cross section of the tube.

I only want to apply load in axial direction. I do not want the rigid to lock any displacements in radial direction but if I only select dof3, I get a kinematic condition error.

I guess, I need a cyclindric coordinate system to do this properly but here I get a second error, telling me cylindric coordinate systems are not supported in geom nl. analysis.

 

Is there a way to still make use of cyclindric coordinate systems in combination with geom nl. analysis?

If not, I'll have to apply the force as a pressure.

 

thank you very much.

 

 

Girish Mudigonda_21018

which version of OS are you using? Please use the latest version to run nonlinear implicit analysis, Also use ANALYSIS= NLSTAT and define NLPARM. OS doesn't support NLGEOM or IMPDYN anymore.

Check below section in user's guide for more details:

http://www.altairhyperworks.com/hwhelp/Altair/hw14.0/help/hwsolvers/hwsolvers.htm?nonlinear_quasistatic_analysis.htm

Altair Forum User

I am using OS 14, this is the error message that I get when using a cylindrical coordinate system:

'CORD1C card is not supported in NLGEOM, IMPDYN and EXPDYN subcases'

 

Altair Forum User said:

Also use ANALYSIS= NLSTAT and define NLPARM. OS doesn't support NLGEOM or IMPDYN anymore.

 

I am not interessted in a quasi static analysis though, my problem requires a geometricaly none linear analysis.