Variation in Simulation results and experimental results

RAMGANESH

Dear All,

 

I have done the seat strength simulation in Radioss ,in simulation it is passed and deflects as required.But in experimental it is very stiff and failed.

 

Kindly give your valuable suggestions.

 

Thanks

RAM

Altair Forum User

Hi Ram,

Normally the simulation results from RADIOSS and experimental results should match approximately. A difference of 10 - 15% in FEA and experimental experimental results is considered a good correlation. Wrongly defined boundary conditions, material properties...etc can be the probable reasons for more deviation of results.

Please ensure that all the modelling (material, property, boundary conditions...etc) aspects set for the model match in both simulation and experimental cases.

RAMGANESH

Dear George,

 

During my simulation in radioss the energy error reaches 99.9%.Kindly give me suggestions

 

Thanks

RAM

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

Altair Forum User

Hi Ram,

When the energy error is positive, there is an energy creation. Please check your model for any incompatible kinematic conditions.

If the initial energy in the system is low, then it is possible to have large energy errors early in a simulation that reduce as energy is added to the system. This is because, small numerical differences in the energy causes large percentage energy errors and in such cases high energy error can be acceptable.

RAMGANESH

Dear George,

 

During simulation i am facing the element distortion issue.

Please give ur valuable suggestions

 

Thanks

RAM

 

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

Altair Forum User

Hi Ram,

There can be multiple reasons for element distortion during the run.

Please check the material properties defined in the model. Wrongly defined material parameters can result in element distortion.

Hourglass is another issue. Hourglass modes are element distortions that have zero strain energy. Hourglassing may easily lead to excessive distortions  To control hourglass assign Ishell-24 and N-5 for shell elements. And for solids use Isolid-14.

 

 

gopal_rathore

Hi Ram,

Are you doing this simulation as per AIS-023 standard i.e H1 and H2 static test.?

RAMGANESH

Dear Gopal,

 

Yes, i am doing the simulation as per AIS-023 Standard.

 

Thanks

RAM

 

RAMGANESH

Dear George,

 

How these parameters  Ishell-24 and N-5 for shell elements affects the simulation results?

 

If these parameters are switched OFF,the results are varying more???

 

Kindly provide your suggestions

 

Thanks

RAM

Altair Forum User

Hi Ram,

Especially for explicit structural analysis Ishell 24 formulation (QEPH shells) is recommended. QEPH shells are more accurate for elastic or elasto-plastic loads, whatever the loading type - quasi-static or dynamic.

If only one integration point is used, a membrane only behavior will be obtained. In case of an elastic behavior, one gets the exact solution from three integration points – that is to say that the bending moments are exactly integrated through the thickness of the shell. In case of a plastic behavior, the bending moments are not integrated exactly. Using more integration points, the solution becomes more accurate; so it is recommended to use five integration points. Also, it controls hourglassing happening in shell elements.

RAMGANESH

Dear George,

 

Thanks for your valuable response.

 

 

Thanks

RAM

gopal_rathore

Hi Ram,

Are you applying the imposed displacement to the rigid body nodes of the actuator's surface behind the seats. Also what is the ramp time being used to apply the same?

Are your results matching with experimental case?

RAMGANESH

Dear Gopal,

 

I am applying the force as per standard using load curve to the rigid body surface.

Simulation time is .2 seconds.

 

Thanks

RAM

gopal_rathore

Hi Ram,

With this condition, are you able to achieve the experimental results?

 

RAMGANESH

Dear Gopal,

 

I am trying to achieve the same. if there is any mistake in the condition please guide me..

 

Thanks

RAM

RAMGANESH

Dear Gopal,

 

Also what are the values to be given in Type 7 interface used b/w rigid body structure and Structure member in this analysis?

 

Thanks

RAM

gopal_rathore

Hi Ram,

For type 7 you can go for keeping Istf :4,Inacti :6 and optimum Gap min. value. For boundary condition, we can go for either imposed displacement or force.

In physical testing, what is the time value achieved from zero to max. load, if your are using the same time ramp value then it is ok, otherwise consider this also into simulation.

Also, your displacement results coming higher or lower than the actual scenario? 

RAMGANESH

Dear Gopal,

 

I didn't considered any time ramp value in this simulation,because there is no data for that value.

I have used imposed load using load curve.

The results are coming lower than the actual scenario.

For type 7 used Iadm=0 & Fric =.2 

 

Thanks

RAM 

gopal_rathore

Dear Ram,

I meant  regarding the time value in which the loads were reached in experimental testing  and the value you are using in the simulation?Also use the parameters mentioned for TYPE 7 in above comments. Are you using MAT LAW 36 (True  stress-strain curve) or Johnson-Cook model for material modelling? 

RAMGANESH

Dear Gopal,

 

Regarding the time at which max load reaches in experimental testing,there is no input available.

I think that need to take some linear value with respect to time.

I am using  Johnson-Cook model for material modelling.

 

Thanks

RAM

gopal_rathore

Hi ram,

How much variation (in %) are you getting from the experimental results. How the weld modelling is done? Is this a 2-seater or 3-seater , school bus seat or an adult bus seat, as load will vary depending on these conditions. Is the load calculated considering these conditions or you have taken the load as applied in experiment.

RAMGANESH

Dear Gopal,

 

I have done weld modeling using spring elements with high stiffness value.

Two seater and three seater (adult bus seat)

Load is applied as per standard.

 

Currently running as per your suggestions.

Once completed will update you.

 

Thanks

RAM

RAMGANESH

Dear Gopal,

 

If load curve with respect to time not available what to do?

Can i give constant loading as mentioned in standards

 

Thanks

RAM

gopal_rathore

Hi,

You can go for giving a load curve with certain ramp time like for H1 point for 2-seater and then maintain it:

Load  Time

0.0            0.0

2666.66    0.2

2666.66    0.4

This being a quasi static process , higher the ramp time is better but with explicit solving limitations we need to go for small ramp time.

RAMGANESH

Dear Gopal,

 

I have run the analysis as per your guidelines ,but the result by loading (2666.66) at Time (0.2) is not meeting the standard.

 

By same loading (2666.66) at time (0.23) the result is meeting the standard. whether this result is reliable and can be consider for testing???

 

Awaiting for your valuable response

 

Thanks

RAM

 

 

gopal_rathore

HI,

This depends on the physical testing condition. As per the standard, the load needs to be applied as soon as possible and this value is not defined. Also you can consider the effect of 20 N preload as given in the standard. Have you done any physical testing on the seat samples and if you have at least displacement data of the seats, the same can be compared .

RAMGANESH

Dear Gopal,

 

we had tested the sample  2 seater seat and got the displacement H1=57 mm and H2 = 44 mm.

 

Simulated the same in system and got displacement H1= 43 mm and H2 = 36 mm.

 

Got variation of 10-15 mm in results.

 

After modification in seats ,now i got the results to meet the standards but had doubt which i asked in previous query...

 

The forces indicated in para. 5.3.1 and 5.3.2 shall be applied as rapidly as
possible and shall be maintained together at the specified value, whatever the
deformation, for at least 0.2 second.  

 

For at least 0.2 second means which duration???

 

Thanks

RAM 

gopal_rathore

Hi,

We have already considered this force in the table as you can see it is 2666.66 at 0.2 and 2666.66 till 0, 4 sec

The comparison shows more stiff seat back when compared to the physical model. This may be taken care by varying spring stiffness used for welds. Do you have force vs displacement curve for the physical testing.

RAMGANESH

Dear Gopal,

 

Please find the  force vs displacement curve for the physical testing .

 

Thanks

RAM

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

gopal_rathore

Hi,

The graph shows different result from what you have mentioned above for H1 and H2 points. The values mentioned above are at the point when the load reached peak and then at constant load the displacement is increasing. What is the case in your simulation , can you put both simulation and physical graphs in one image  for better comparison.

RAMGANESH

Dear Gopal,

 

We have done the physical testing on the seat samples but its is not co-relating with simulation results.

 

In simulation its passing but in physical testing its failed.

 

please give guidance for  solving this problem.

 

Thanks

RAM