Showing results for 
Search instead for 
Do you mean 
Reply

Need help in Non Linear simulation

[ Edited ]
Dear All...
Can any body guide me on how to apply a load for Non Linear simulation for Sol NLSTATIC 106. It is singe part with thin plate structure (300 X 140 X 0.4mm Thick) with a centre load of 5N. May I what is correct way to apply the load. Please ref to the attached image file. I have upload the simulation file to the scratch Area (NL.zip) for reference. Any one please guide on this step.

Thanks a lot in advance.
Log


10 REPLIES

Re: Need help in Non Linear simulation

The tabular field appears to be defined correctly. Did you also edit the Nonlinear Parameters in the solution set's case control? There is a parameter for Number of Increments. Set that value to 5 and your solve will have 5 steps coinciding with times 1-5 in your time dependent field of your load. There's also an option in the Nonlinear Parameters to store results for intermediate steps. The Intermediate Output Flag can be set to No (default), Yes, or All.

Regards,
Mark

Re: Need help in Non Linear simulation

Logesh,

Solution 106 does not support time dependent loading. Your time dependent loads are being evaluated at the Boundary Condition Field Evaluation Time specified on the Edit solution dialog (default is 0.0 seconds) and written out as a single static load.

You can linearly vary the results output by requesting results be stored at intermediate steps as Mark describes, but only a single static load is used as the final magnitude. The solver automatically subdivides it into NINC increments. The only way to nonlinearly vary load magnitude in SOL 106 is with multiple subcases.

Regards,
Jim
--
Jim Bernard
Advanced Applications Engineer

Siemens PLM Software
2000 Eastman Dr., Milford, OH 45150-2712
www.siemens.com/plm

Re: Need help in Non Linear simulation

[ Edited ]
Hi Mark and Jim
Good Day. Thanks a lot your response. I need to do analysis of thin plate (300*140*0.4mm) with large displacement. The applied load in 5N at the centre.

For this NLSTATIC 106 Non Linear case, Shall I apply a fixed load of 5N directly or I need to vary the load over a specified time?

If I apply a fixed load of 5 N the Displacement value is vary high(108mm)

If I apply as Time varying as below the Max displacment is 4.99mm
Time / Fore(N)
0 / 0.1
10 / 5

If I apply as Time varying as below the Max displacment is 0.499mm
Time / Fore(N)
0 / 0.01
10 / 5

Why initial Force change the Displacement Value? If I need to apply time varying load how to apply? Please kindly advise on this step.


Thanks a lot in advance

With Regards

Log

ID,NASTRAN,preview
SOL 106
CEND
ECHO = NONE
SPC = 1
NLPARM = 100
TEMP(INIT) = 200
OUTPUT
DISPLACEMENT(PLOT,REAL) = ALL
ESE(PLOT,AVERAGE) = ALL
NLSTRESS(PLOT) = ALL
SPCFORCES(PLOT,REAL) = ALL
STRAIN(PLOT,REAL,VONMISES,FIBER,CENTER) = ALL
STRESS(PLOT,REAL,VONMISES,CENTER) = ALL
$ARAM NAME VALUE
PARAM K6ROT100.0000
PARAM LGDISP 1
PARAM OMACHPR YES
PARAM POST -2
PARAM POSTEXT YES
PARAM UNITSYS MN-MM

Re: Need help in Non Linear simulation

The answer is in Jim's reply. It's a subtle one that is verified by the load/displacement data from your 2 runs.

Solution 106 does not support time dependent loading. Your time dependent loads are being evaluated at the Boundary Condition Field Evaluation Time specified on the Edit solution dialog (default is 0.0 seconds) and written out as a single static load.

Set the boundary condition field evaluation time to the highest value in your field to get the full load.

Regards,
Mark

Re: Need help in Non Linear simulation

[ Edited ]
Hi Mark

Good Day Thank for your advise,, I got your answer... There is one more issue when I run the actual model. There is some error and the Analysis terminates. Could you advise what will cause this error?

Number of elements in the mesh : 12467
Number of nodes in the mesh : 35306
Quad8 Thin Shell elements : 9998

Is this Error due to Meshing problem?

*** USER INFORMATION MESSAGE 7310 (VECPRN)
ORIGIN OF SUPERELEMENT BASIC COORDINATE SYSTEM WILL BE USED AS REFERENCE LOCATION.
RESULTANTS ABOUT ORIGIN OF SUPERELEMENT BASIC COORDINATE SYSTEM IN SUPERELEMENT BASIC SYSTEM COORDINATES.
0 OLOAD RESULTANT
SUBCASE/ LOAD
DAREA ID TYPE T1 T2 T3 R1 R2 R3
0 1 FX 3.418481E-31 ---- ---- ---- -3.230589E-24 9.094229E-21
FY ---- -6.963692E-31 ---- 5.195852E-17 ---- -9.188049E-21
FZ ---- ---- 5.000000E+03 3.068241E+04 5.750057E+03 ----
MX ---- ---- ---- 1.103879E-18 ---- ----
MY ---- ---- ---- ---- 1.370697E-21 ----
MZ ---- ---- ---- ---- ---- 9.382014E-23
TOTALS 3.418481E-31 -6.963692E-31 5.000000E+03 3.068241E+04 5.750057E+03 0.000000E+00
*** USER WARNING MESSAGE 3057 (NLITER)
MATRIX IS NOT POSITIVE DEFINITE.
*** SYSTEM FATAL MESSAGE 3007 (NLITER)
ILLEGAL INPUT TO SUBROUTINE NLINIT
0FATAL ERROR
1 * * * END OF JOB * * *

Re: Need help in Non Linear simulation

Hi Logesh,

I am not sure about the error message.

But from the figure you attached, I see that you have a fixed constraint. I assumed you are doing the simulation model in a symmetrical manner, because the force load location in actual is at the center. If so, I think you need to add additional user defined constraint to constraint the symmetrical plane.

About the error, randomly I would try to check the directory of the file, make sure it is close to root directory such as c:\. Sometimes it the address to your input file is too long will have problem in file writing permission.

Regards,

Tuw

Re: Need help in Non Linear simulation

HI Tuw, Thanks for your valuable feed back. Actually we don't have Adina license for Sol 601. I have tried with demo license the file works fine. I also manged to get the result for
with NASTRAN sol 106 by increasing the Number of increment. But it take very long time compared to Sol 601. The result is near about same.

Sol 106 --- Deflection 4mm, Max Stress 29Mpa

Sol 601--- Deflection 3.9mm, Max Stress 30Mpa

Actual physical testing Deflection is 2.9mm

This is a thin case of 0.4mm with a dimension of 300mm X 140mm X 10mm

Any body can advise on which parameter would have caused the deviation from the actual result.

Looking forward to hearing from you.

Thanks a lot in advance.

Logesh

Re: Need help in Non Linear simulation

Hi Logesh,

For more accurate result, you will need to input the stress strain curve of the material in.

Secondly, based on your result, I assume the actual part is "harder", the simulated model is "softer" thus giving you a higher displacement. If you plan to make your simulation model "harder", you can play with the mesh element size and type. The smaller your element size, the "softer" your model. Tet4 is harder then Tet10 anyway.

But I dun think making your mesh element size larger is the right path. In addition, experienced analyst stated that Tet4 is too hard and should never be used for structural analysis. Tet4 is suitable for thermal analysis however.

Regards,

Tuw

Re: Need help in Non Linear simulation

Hi Tuw

As i am doing 2D element analysis, I am using CQUAD4 element with element size of 1mm. I have tried a simple analysis to vary the mesh size. As you have stated larger mesh size gives smaller deflection. But the difference is not significant (0.02mm). So I try to work out with the stress strain curve. thanks for your valuable input.

With Regards
Logesh