Huge different in stress result in RADIOSS

[nizammuaidi]

Hi there,

Currently I am fully use Hyperworks product in strength analysis. Start from pre-processing (HyperMesh), Solving (RADIOSS non-linear) and post-processing (HyperView & HyperGraph).

For comparing purpose, I also run same FE model (in terms of mesh model, load & BCs, material properties, stress-strain data) in ABAQUS and NASTRAN.

The stress that I look for is Maximum principal stress and nodal based result. NASTRAN and ABAQUS gives similar maximum principal stress while RADIOSS stress result is lower ~250 MPa which is considered very big in strength analysis and will drive to wrongly interpret the fatigue life cycle.

Can anybody suggest why this huge stress different occur and how can I resolve this problem. I have asked this issue to the support team and currently there is no solution yet.

An analogy:
If we go to the market and ask 5kg of fish, suppose it will shows 5kg in the mass scale. Either with seller A, B, C, D and E.
Suddenly we go to the seller H and ask for 5kg of fish. In the mass scale shows 3kg but the seller H strongly said that is 5kg. ---Is that make sence?

Note1: 5kg fish= stress result. seller = software.

Note2: Definitely it will be a different, maybe mass scale at seller A shows 4.9kg, seller B 4.86kg, seller C 5.1kg, seller D 4.88kg and so on... It doesn't matter since it close to the 5kg that we require. We can not accept the 5kg fish with 3kg indicator at mass scale.

Lets discuss.

Thanks.

KN.

 

[GregLocock]

What are the actual stress levels you are seeing? what material model are you using? Were your nastran and Abaqus models non linear as well? what do you mean by non linear, material, displacement, or both?

what happens if you compare linear results instead?



Cheers

Greg Locock

SIGlease see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[nizammuaidi]

Basically it is a spring analysis. So it involves geomtric non-linearities.

Since current trend requires an ultimate optimize spring design, so the stress level set to be ~1000 MPa (SUP12 or SAE 9254). Based on tight maximum stress target, we also need to include material non-linear properties to be aware of yielding and stress fatigue limit.

I have compared along the spring dispalcement between RADIOSS and ABAQUS, and RADIOSS stress result is lower along the displacement.

Beside spring comparison, I also compared the stress result of knuckle between NASTRAN and RADIOSS. Still RADIOSS gives lower stress result. This knuckle analysis also included material non-linear properties.

As a conclusion, definition of non-linear applies for material and also geometry.

rgds,
KN

 

[nizammuaidi]

Some additional info..

Beside spring comparison, I also compared the stress result of knuckle between NASTRAN and RADIOSS. Still RADIOSS gives lower stress result. This knuckle analysis also included material non-linear properties.

[blue]I also run knuckle analysis using ABAQUS and the stress result between ABAQUS and NASTRAN is close to each other. while RADIOSS is lower than these 2 software.[/blue]

 

[GregLocock]

Well, unless you are willing to post far more detail than you have so far, we're a bit stuck. As an expert yourself, what could you deduce from the info in this thread?




Cheers

Greg Locock

SIGlease see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[nizammuaidi]

First of all, I'm not the expert and I believe many more experts and specialists in this forum. I am just a beginner CAE operator.

Here I attached some capture view of the stress result. In this example, the stress different is ~150 MPa which is considered huge also.. If we refer back to analogy, suppose it would not differ in that huge.

The stress concentration area at the same place. The differrent only the value.

Both result were read at same displacement, stress of Maximum principal, nodal based (simple averaging method in RADIOSS and banded in ABAQUS).

[blue]Since the FE model setup is same, what is the possible mistake I done cause my stress result in RADIOSS differ.?[/blue]

 

[GregLocock]

Well, how sure are you that the two measurments f stress are identical? It seems odd that they both identify the same node as the max stress, yet further away from that point the colours look completely different.

Cheers

Greg Locock

SIGlease see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[nizammuaidi]

Capture view that I sent is two different result. The left result is from ABAQUS result while right hand result is RADIOSS result. But it is a same FE model. So the high stress occur at the same node however the value is different. This is my problem before.

By the way this problem is resolved.

Let me explain...

RADIOSS are using purely element based result as their stress result. So the stress value is at the middle of the solid element. ABAQUS also has the element based stress result.

Right now the only different between ABAQUS and RADIOSS is the method of averaging the stress value between the element at the shared node. The averaging method in ABAQUS will represnt the stress at the surface while RADIOSS can't gives this types of averaging.

So, to get stress value at the surface in RADIOSS solver, skin element need to be applied on the part. The stress result at the skin element are now similar with ABAQUS.

[blue]Problem resolved..[/blue]