How do I use simulation results in a new solution?

[femstarter]

Hello everyone,

first of all: I am new here and I am new in FEM. I use NX 8.0, have two questions and would be more than happy if anyone could help me.

1) linear FEM, Solution Type: SESTATIC 101 - single constraint:
I successfully finished a simulation and now want to use the results in another one. I would like to have the deformed model with all the stresses and strains etc in a new solution so that I can add new boundary conditions and loads. Does anyone know how to do this?

2) nonlinear FEM, Solution Type ADVNL 601,106:
I put an enforced displacement constraint on some nodes and defined the rotation around x-axis with a field. Some nodes are fixed. Everything works fine. Now I want to fix some nodes of the deformed geometry and put an enforced displacement constraint on other nodes. So again: I want to do a simulation in two steps using the complete results of the first one. Alternatively - if there is a possibility - I would like to change the boundary conditions of the model with different time steps so that I can change the boundary conditions within one solution. Can anyone help me with this one?

I would be extremely happy if anyone could help me out.

 

[kapmnit123]

Hi,
i am not that into FEM also. But pertaining to your first query (re-using the results).I guess you want to use the deformed object (after first analysis) for further analysis ...am i correct in thinking so? If yes then i would rather say it is not possible as far as the type of solution (linear static) you are using.Reason being for applying Boundary conditions you need to have the FEM model (in your case the deformed meshed one) but you wont get an output like that after the first FEA run (i could be wrong and will be happy if someone correct me on that).
In case you have anything specific in your mind could you please share with us
Best Regards
Kapil Sharma

 

[femstarter]

Thanks for your reply. You are right: I would like to use the deformed object for further analysis. The problem is that I have no idea how to use the deformed geometry including all the stresses/strains etc. in a way, that I can put new boundary conditions on it. I would like to do the simulation in two steps. At first I would like to apply boundary conditions and do the analysis. In the second step I would like to take the resulting geometry from the first step including all of the stresses/strains etc. and calculate with new boundary conditions.

In general I can say that I would like to compare a linear analysis with a nonlinear analysis to find out whether I have to do the simulation nonlinear.

I keep you updated in case I can solve the problem on my own. But still: I would be SO SO SO happy if anyone could HELP ME OUT.

 

[BlasMolero]

Hello!,
1.- In NX NASTRAN Linear Static (SOL101) analysis you can "play" with the combination of loads cases & Boundary Conditions in order to explore different scenarios in real life. Also, you can update nodal coordinates with the resultant displacements of linear static analysis, this is typical situation when running buckling analysis to account for geometric imperfections in the model: to use the deformed shape of linear static as initial configuration for buckling analysis (SOL105).

I remembet this functionality of using the results of a simulation to deform the original mesh for further simulation work available since NX AdvSim 7.5 writing displacement nodal results + nodal coordinates in an EXCEL file. Later using NODE TRANSLATE command in the FEM environment to update the mesh. And also you can deform the CAD geometry surfaces based on the solution results using GLOBAL DEFORMATION command.

2.- In nx nastran advanced nonlinear analysis (SOL601/701) you have the RESTART command (and in linear static analysis as well, of course!).
Restart is a useful feature in Advanced Nonlinear Solution. It can be used when the user wishes to continue an analysis beyond its previous end point, or change the analysis type (eg, from static to transient dynamic), loads or boundary conditions or tolerances. It can also be used to continue an analysis from the last converged solution time. A restart analysis is selected by setting MODEX = 1 in the NXSTRAT entry. Recovering results from a restart file without continuing the analysis can also be done setting MODEX = 2.

A restart is a logical way of continuing from a previous run without having to start from the beginning. Restarting is very powerful, for the purpose of a prestressed normal modes analysis, you can restart from a SOL 106 run into another SOL 103 run to perform the prestressed normal modes calculation with changing boundary conditions, or restart into another linear solution sequence to perform a perturbed linear solution on a preloaded structure. Restarts from SOL 106 into linear solution sequences are not recommended to the novice user because of several limitations. The results of the linear restart are incremental values with respect to the preload, not total values.

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/