Nastran sol 106

[vanji1]

Hi everybody,

I am trying to do something simple using Nastran SOL106.
I have a two element mesh (CHEXA elements) and I put a simple point load on a node with a given direction (three subclasses for three directions) and I want to compute the nonlinear displacement in case of large displacements.
(Just note that the two element mesh is in fact just one element because the properties concerning the second elements are chosen to be degenerated.)
When I do that, I never can activate the nonlinearity. If I multiply the load by a factor 10000, I go on with linear calculations, that is to say a SOL101.

What I would like is to carry out this nonlinear calculation.

This is my .bdf. What do I miss for activating the large displacements ?

I thank you in advance,

Best regards,


INIT DBALL LOGICAL=(DB(100000))
INIT MASTER LOGI=(MS)
$
SOL 106'
TIME 600
DIAG 8
CEND
$
TITLE=FNL
SUBCASE 1
NLPARM=1
SPC=2
LOAD=3
$SPCFORCES(SORT1,REAL)=ALL
DISP=ALL
SUBCASE 2
NLPARM=1
SPC=2
LOAD=4
$SPCFORCES(SORT1,REAL)=ALL
DISP=ALL
SUBCASE 3
NLPARM=1
SPC=2
LOAD=5
$SPCFORCES(SORT1,REAL)=ALL
DISP=ALL
$
BEGIN BULK
$ activation du non lineaire geometrique
PARAM,NLGEOM,1
$ activation grands deplacements
PARAM,LGDISP,1
PARAM,AUTOSPC,YES
$ matrice de masse complete (non concentree)
PARAM,COUPMASS,1
$ format exportation
PARAM,POST,0
PARAM,PRGPST,YES
$ inclus la force suiveuse dans le calcul de la matrice tangente
PARAM,FOLLOWK,YES
$ integration full with 3*3*3=27 gauss points
PSOLID,1,1,,3,,FULL
PSOLID,2,2,,3,,FULL
$ elements HEXA with 8 nodes (linear interpolation)
CHEXA 1 1 1 3 4 2 7 9
10 8
CHEXA 2 2 3 5 6 4 9 11
12 10
$ material with card 1
MAT1 1 1.89e+11 2.50e-017.86e+03
$ material with card 2 (null material properties artificial)
$ artificiellement le deuxieme element masse nulle
MAT1 2 1.89e-01 2.50e-017.86e-9
$ node list
GRID* 1 3.50000000e-02 0.00000000e+00
* 0.00000000e+00
GRID* 2 3.47005701e-02 4.56841673e-03
* 0.00000000e+00
GRID* 3 5.12500000e-02 0.00000000e+00
* 0.00000000e+00
GRID* 4 5.08115491e-02 6.68946735e-03
* 0.00000000e+00
GRID* 5 6.75000000e-02 0.00000000e+00
* 0.00000000e+00
GRID* 6 6.69225281e-02 8.81051797e-03
* 0.00000000e+00
GRID* 7 3.50000000e-02 0.00000000e+00
* 5.00000000e-02
GRID* 8 3.47005701e-02 4.56841673e-03
* 5.00000000e-02
GRID* 9 5.12500000e-02 0.00000000e+00
* 5.00000000e-02
GRID* 10 5.08115491e-02 6.68946735e-03
* 5.00000000e-02
GRID* 11 6.75000000e-02 0.00000000e+00
* 5.00000000e-02
GRID* 12 6.69225281e-02 8.81051797e-03
* 5.00000000e-02
$ Dirichlet condition for node 1
$ SPC1,2,123456,1
$ Dirichlet condition for nodes 1,2,3,4
SPC1,2,123456,1
SPC1,2,123456,2
SPC1,2,123456,3
SPC1,2,123456,4
$ static concentrated force intensity 1e6, node 8, dof 1
FORCE,3,10,,1e6,1.,0.,0.
$ static concentrated force intensity 1e6, node 8, dof 2
FORCE,4,10,,1e6,0.,1.,0.
$ static concentrated force intensity 1e6, node 8, dof 3
FORCE,5,10,,1e6,0.,0.,1.
$ nonlinear calcul
NLPARM,1,2 $,,AUTO,UPW,NO$1,25,UP,YES
$NLPARM 1 10 AUTO UPW NO
ENDDATA

 

[sdm919]

What type of behavior are you expecting? If you're just testing the nonlinear capabilities of Nastran, you would probably be better off using one of their example problems.

Is Nastran trying to iterate at all? Check the f06 file for the convergence information. It might be converging right away (that is just spitting out the linear result), but if you see the listing of convergence information, that would indicate that it is at least attempting to iterate. Look for the word "CONVERGED" for example. Since your NLPARM card is requesting NINC=2, you should see at least 2 occurrences of the word "CONVERGED" in the f06 file.

I suspect the main problem is this: a single element is probably not adequate to demonstrate nonlinear geometric behavior. It might be adequate to demonstrate nonlinear material behavior, but not nonlinear geometric. One thing you could do would be to stack 10 of these CHEXA elements on top of each other (in the z-direction) and apply the load to the top nodes (and continuing to restrain the bottom as you are now). Then you might see some iterations occurring.

Finally, I believe the SUBCASEs in Nastran SOL 106 build one upon the other, they are not 3 independent conditions. So, SUBCASE 2 will start where SUBCASE 1 left off and so forth. This may or may not be what you intend with your 3 load cases. Usually the total load is broken into steps and each SUBCASE represents one of those steps. If you want to model a completely different load condition, you would usually make a separate Nastran run for each condition.