Load Function in Nonlinear Static

[jerza]

Hi,
I'm new in Femap with NX Nastran. I did a lot of examples and my own comparison. Now I'm interesting in Nonlinear analysis. I went through many examples in Femap, Youtube, I read some info in Nastran Guide book.

My question is:
Can I use in Nonlinear Static Analysis load function, e.g. exp(x) or other complex function? So in Loads menu I set Load of "something" with Time/Freq Dependence of my function? Or it is no possible?

Regards

JK

 

[BlasMolero]

Dear JK,
The static loads in nonlinear analysis (SOL106) with NX NASTRAN consist of a subset of the total NX Nastran static load set. Most of the relevant loads data applicable to the linear static analysis are also applicable to nonlinear static analysis. NOT NEED TO DEFINE A FUNCTION OF LOAD vs. TIME, this is more simply (see example here

http://www.iberisa.com/soporte/femap/nolineal/soldadura_punto_a_punto_nolineal.htm)

The loads are selected in each subcase by the LOAD Case Control command. The load for a subcase is subdivided into the number of increments specified for the subcase. The solution strategy in nonlinear is to apply the loads in an incremental fashion until the desired load level is reached. The algorithms “remember” the loads from one subcase to the next. If the load reaches the desired level in a subcase and if the load description is left out in the subsequent subcase inadvertently, the nonlinear solution algorithm will begin in an incremental fashion to remove the load.

The unique data required for SOL 106 is supplied on the NLPARM entry, which controls the incremental and iterative solution processes. Simply define the number of increments (10 Time Steps by default), and the maximum iterations per step and you are done!

There are advantages to divide the entire loading history into many subcases so that each subcase does not have excessive number of increments, e.g., not to exceed 20 steps. The data blocks containing solutions can be generated at each increment or the end of each subcase depending on the intermediate output option specified in the INTOUT field of NLPARM data entry.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[jerza]

Hi BlasMolero

I hope I understand that. In your example the load pressure 0,13 MPa is divided into 10 steps, so in the first step is the pressure 0,13/10 MPa, etc.

But what if the pressure is parabolic function or nonlinear force? It works too? If you don't understand me what I ask, here an example 1, it's possible do that way? Of course with NX Nastran. Or I missed something?

Regards

JK

 

[BlasMolero]

Dear JK,
Depending the nonlinear module you use with FEMAP & NX Nastran (depending of your license), you must follow one strategy or another:
• Basic Nonlinear Static (SOL106) & Dynamic (SOL129): you must divide your loading history using LOAD CASES as explained before. To understand the procedure better read the EXAMPLES MANUAL OF FEMAP: 25. Plastic Deformation of Rod - Nonlinear Material where you will learn how to define a LOAD-UNLOAD CASES. This module is part of the Basic system. To load the manual enter in FEMAP, and go to HELP > EXAMPLES.
• Advanced Nonlinear Implicit Static (SOL601, 106) and Dynamic (SOL601,129), and Advanced Nonlinear Dynamic Explicit (SOL701): here you can define explicitely any function vs. Time to associate to any loading force/pressure, etc... This module is an add-on to the basic system, very powerful.

Best regards,
Blas.



~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[jerza]

Thanks that's what I want to hear. I wasn't sure and now I'm a bit clever. One more time thanks.

Regards

JK