RADIOSS BLOCK - NON LINEAR ANALISYS PROBLEMS

Hi,

MATX25 is a OptiStruct Material card extension whereas MAT25 is for RADIOSS. please confirm this?

1) in context of explicit analysis the timestep is dependent on characteristic length of the element and the material sound speed {(E/RHO)^0.5}. if you know the timestep for the simulation you can derive the characteristic length of the element based on this rule and the element size should not be less than the characteristic length.

2) what kind of 2nd order elements are used in your model? do you have any contact interfaces?
also, can you please let us know the version of HW you are using? use the link to find out the software update information http://www.altairuniversity.com/support-forum/?mingleforumaction=viewtopic&t=252

3) I am not sure what is causing the problem, my suggestion would be check the unit consistency for material and properties in your model.

[...] do you have any contact interfaces? [...]

Can contact interfaces cause trouble? I am using Freeze contact to tie parts together but when I try to run a geometric non-linear analysis I get errors because of contact interfaces. Any clue? I have no problems with small displacement analysis, but only with large displacement analysis.

Here one of around 800 identical errors:

STARTER ERROR:
 ERROR ID :          556
 ** ERROR IN INTERFACE TYPE2
 DESCRIPTION :
    -- INTERFACE ID : 50
    -- INTERFACE TITLE : INTER_TYPE2_50
    MASTER NODE ID=97392 IS ALSO SLAVE NODE OF ANOTHER INTERFACE TYPE2

Which version of Hyperworks you are using?Optistruct 14.0 nlstat for large displacement will work fine.

MASTER NODE ID=97392 IS ALSO SLAVE NODE OF ANOTHER INTERFACE TYPE2

Hi,

Looks like the one of the nodes is in both master and slave. Try to clear that and try again.

Which version of Hyperworks you are using?Optistruct 14.0 nlstat for large displacement will work fine.

Yes, 14.0. So I should use non-linear static subcase instead of geometric nonlinear subcase? I will try.

Btw, I have a modell with shell elements mainly. The documentation states that OptiStruct cannot perform large displacement analysis for shell elements. What should I do? Using Radioss? Is my OptiStruct modell fully compatible with Radioss?

 

Hi,

 

Looks like the one of the nodes is in both master and slave. Try to clear that and try again.

At several regions I have tied 3 parts together which means that one element (of component A) will be tied (freeze contact) to two other elements of components B and C.

In OptiStruct 13.0/14.0 it works fine, but for geometric non-linear analysis the Radioss solver is used automatically. Maybe Radioss does not allow this definition, is that true?

Not sure.

Can you share the entire .out file and if possible the model file?

The slave-master definition is definitely causing my problem with Radioss...I will have a look at it and try to fix it.

Can you tell me where to activate the NLOUT entry? It does not seem to be available GUI...I cannot find it in HM14.0

'The NLOUT entry can be used in the Subcase Information section to select the incremental result output parameters used for Nonlinear Static Analysis and Nonlinear Transient Analysis. '

'The NLOUT bulk data entry defines incremental result output parameters for small displacement nonlinear analysis and large displacement analysis. '

Hi Msc,

You need to add NLOUT through Control Cards>> Bulk_UnSupported_Crads in a specified format as shown in the image.

After adding the card, you need to refer the same in the loadcase by editing the loadcase/subcase>>Subcase_Unsupported cards.

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

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

Hi Msc,

 

You need to add NLOUT through Control Cards>> Bulk_UnSupported_Crads in a specified format as shown in the image.

 

After adding the card, you need to refer the same in the loadcase by editing the loadcase/subcase>>Subcase_Unsupported cards.

Thank you, it works :-)

Two more questions concerning non linear analysis:

1) How can I control the output increments for NLGEOM analysis (Geom non-linear (impl static))? The NLOUT parameter seems to work only for NLSTAT anlysis.

2) What is the difference between running a NLSTAT simulation and activating LGDISP and running a NLGEOM analysis?

Is the stiffness matrix also updated during NLSTAT-LGDISP simulation? Are different solvers used? For a shell plate I get two different results as soon as I reach the buckling load...but the step sizes are different as well: With the same parameter NLPARM/NINC=20 which defines the first step size of 0.05 I get output 20 equidistant steps for NLSTAT-LGDISP, but only 13 steps for NLGEOM analysis. The time steps after reaching the buckling load are bigger for NLGEOM so it is hard to compare the curves as the output is not gained at the same time point.

Hi,

NLGEOM uses RADIOSS in the background so you get incemental results based on the frequency.

NLSTAT without LGDISP will work for small displacement problems where as activating LGDISP will work for large displacement implicit problems.