Non linear fatigue simulation 1

[Gov45]

I wanted to do a fatigue analysis. The initial stresses I obtain is above the yield limit. There is non-linearity due to contacts and plasticity. I have few queries as below.

Stress Based Approach
For high cycle fatigue I am using a (S-N) approach because the linear stresses are below 70% of yield and in the elastic part of the material curve. I clearly understand this.

Strain Based Approach
When the linear stresses are over yield this is where I am still unclear and have questions.

1. Should I always use a strain based approach when the stress is over yield?
2. Should I use the above linear stresses, over yield, with an elastic plastic correction (Neuber).
3. Should I use non-linear stress results with no elastic plastic correction.

 

[FEA way]

Are you using fe-safe ? Then there are two options:
- import stresses from elastic FEA - fe-safe will apply plasticity correction by default
- import stresses and strains from elasto-plastic FEA - no plasticity correction here

The first one is sufficient to account for local plasticity, the second one is needed to account for global plasticity (stress redistribution).

There are also additional approaches to account for residual stresses / nonlinear preload or forming step but I guess it's not the case here.

 

[Gov45]

Hi, thanks for the response

I am using FEMSITE but its similar to FE-SAFE.

In my model, there are contacts, and hence there is a good amount of plastic deformation in the model, we can say global plasticity.
So in such a case if I do a non-linear FEA calculation (IN Abaqus) then what are the settings I have to take care in say FE-safe to do a non linear fatigue simulations. If I have two steps in ABAQUS calculations, should I provide all the increments of both the steps as input to FE-safe ?

 

[FEA way]

In fe-safe, if you want to include plasticity in fatigue loading (not just as residuals), you have to import both stresses and strains from the nonlinear FEA model and use dataset sequence loading (instead of the superposition - scale and combine approach). Elastic-Plastic Block will be automatically created and you just have to specify the range of increments and ensure pairing of stress and strain datasets.

 

[Gov45]

Hi FEA way

Thanks for the response. I was looking for this answer.
Can you please elaborate on the dataset sequence loading and specifying the range of increments ?

Suppose I have two steps in ABAQUS calculation.
Step -1 has say 10 increments.
Step-2 has 7 increments.

How do I go about doing a non-linear fatigue calculation in fe-safe.

Are there any documentation for the same.

Thanks and Regards

 

[FEA way]

How do I go about doing a non-linear fatigue calculation in fe-safe.

1. Go to Fatigue from FEA --> Loading Settings and add a Block (Elastic initially).
2. In Current FE Models, select the first stress dataset and in Loading Settings right-click on the Block and choose Add dataset.
3. In Current FE Models, select the first strain dataset and in Loading Settings right-click the Stress Dataset added before and click Add dataset.
4. Edit each dataset in the pair to define a matching series of datasets (increments) - you can use ranges like 1-21(2) which means 1 to 21 every second one or just list the numbers separated with commas.

Are there any documentation for the same.

fe-safe User Guide - paragraph 15. Fatigue analysis of elastic-plastic FEA results

 

[Gov45]

1. Go to Fatigue from FEA --> Loading Settings and add a Block (Elastic initially).
2. In Current FE Models, select the first stress dataset and in Loading Settings right-click on the Block and choose Add dataset.
3. In Current FE Models, select the first strain dataset and in Loading Settings right-click the Stress Dataset added before and click Add dataset.
4. Edit each dataset in the pair to define a matching series of datasets (increments) - you can use ranges like 1-21(2) which means 1 to 21 every second one or just list the numbers separated with commas.


fe-safe User Guide - paragraph 15. Fatigue analysis of elastic-plastic FEA results

One more question, in the attached Image ,
(Ignore step-1 to step-4)
step-5 = Compressive load case
step-7 = Tensile load case

every step and increment of ABAQUS calculation is mapped to a particular number in FEMSITE (Fatigue simulation software 1 to 31),

Is this what you were explaining in your point number 4?

 

[FEA way]

This is what it looks like in fe-safe for 3 Abaqus steps with the first two having 5 increments each and the third one having 4 increments.

Imported datasets:



Loading definition: