SolidWorks Simulation Non-Linear & ASME VIII-2 2

[IdanPV]

According to ASME Section VIII Division 2 paragraph 5.2.4.4, and as part of the assessment procedure, an elastic plastic material model shall be used in the analysis:
"An elastic plastic material model shall be used in the analysis. The von Mises yield function and associated flow rule should be utilized if plasticity is anticipated. A material model that includes hardening or softening, or an elastic perfectly plastic model may be utilized. A true stress–strain curve model that includes temperature dependent hardening behavior is provided in Annex 3-D. When using this material model, the hardening behavior shall be included up to the true ultimate stress and perfect plasticity behavior (i.e., the slope of the stress–strain curves is zero) beyond this limit. The effects of non-linear geometry shall be considered in the analysis"

I made an elastic plastic material model, by using Annex 3-D and that website:

http://fsefea.com/asme-ptb-3-validation-elastic-plastic-analysis

(this example were made with ANSYS)
My questions are:
1. When I enter the material properties in Solidworks I have a lot of options there, which one should I used in order to meet the ASME rules for non-linear analysis?
2. Anouther question regarding the stress-strain curve, does the strain in the curve is the total strain or the plastic strain.
3. Is it possible to meet the requirements of ASME VIII-2 with solidworks non-linear?

 

[FEA way]

These requirements can be met when using nonlinear analysis in SolidWorks Simulation. Select von Mises plasticity and then you will have two possibilities:
- bilinear model: specify Young's modulus, yield strength, tangent modulus (0 for perfect plasticity) and hardening factor (0 for pure isotropic hardening, 1 for pure kinematic hardening) in the table
- multi-linear model: click the "Create stress-strain curve" button and specify data points defining stress-strain curve (use total strain)

 

[IdanPV]

FEA way, Thank you very much!

Few more question:
1. According to ASME VIII-2 5.3.3.1 in need to determine the "equivalent plastic strain" but SolidWorks only shows the equivalent strain (ESTRN) can I use it?
2. As for the multi-linear model, why should I use the total strain?
3. According to ASME VIII-2 5.3.3.1 in need to determine the principal stresses, but in
SolidWorks there is the max. and min. for each prinicpal stress, which value should I use?

Thank you very much!

 

[FEA way]

In advanced settings of ESTRN contour plot you can select plastic strain.

Total strain should be used for multi-linear model definition because of the way SW Simulation interprets the data. Some software requires the first point to be yield strength with zero strain (and therefore plastic strain is specified) while other programs use total strain.

You can plot all principal stress components individually using variables named P1 (max), P2 (mid) and P3 (min).

 

[IdanPV]

FEA way,Thanks again!

Regarding the principal stress, I know I can plot each of them, but the stress value for each one is start at -X (MPa) and ends in +Y (MPa)
I made an example:

The values of the P2 stress plot is changing from min. -304.636 to max. 237.998.
Should I use the absolute (|-304.636|=304.636) value of the min. which is larger than the actual max. value?

 

[FEA way]

For failure criterion you should use absolute value (304.636 MPa in this case).

 

[IdanPV]

Thank you very much for your help.

 

[mskds545]

That is not correct. Using the maximum absolute value of each principal stress component from any location in the model makes no sense. The strain limit is local. 5.3.3.1 requires the local strain limit be met at each point in the component. You need to calculate the limit as a function of S1,S2,S3 and Seq at every point in the model and compare it to the local plastic strain. There is only one value of each principal stress at each location and only one value of the equivalent stress at each location. The principal stresses have a sign, which should be kept when evaluating the triaxiality factor. Do not use the absolute value. This will not correctly predict the local ductility.

-mskds545

 

[IdanPV]

mskds545,
Thank you very much for your comment.
I would like to ask few questions about it,
1. 5.3.3.1 requier to check each point in the component, is that mean I need to pick one NODE in the model and check there? and repeat that for each NODE?
2. Assuming I picked up one NODE, the equivalent plastic strain and the equivalent stress will be posative for sure.
But the principal stresses can be either positive or negative.
The absoulte value of negative might be more than the positive (see my post from 16 March).
In this case, which value should I use?
For example:
S1=310.505
S2=207.479
S3=-258.379
For the case above, does S1+S2+S3=310.505+207.479+(-258.379) OR S1+S2+S3=310.505+207.479+|(-258.379)| ?

 

[mskds545]

For your first question, what I've typically done is create a user defined result of plastic strain / local strain limit and create a contour plot of that ratio. Any location over 1.0 fails to meet the local criterion.

For your second question, you should not use the absolute value. Use the sum S1+S2+S3. You're evaluating a low ductility failure due to high hydrostatic stress. If you have S1 = -S2 = -S3, you will have a low hydrostatic stress and a high deviatoric stress (picture a large Mohr's circle, with the major circle centered around the origin). If you have S1 = S2 = S3, you will have a high hydrostatic stress and zero deviatoric stress (Mohr's circle becomes a point, off to the right of the origin).

-mskds545

 

[IdanPV]

mskds545,
Thank you.

Regarding your first answer, about the user defined result of the plastic strain, how can you or the user can estimate it?
Is there any "rule of tumb" for it?

 

[mskds545]

If you're following section 5.3.3, I interpret the code as requiring you to evaluate it at each point in the component and I recommend you do that. I suppose if you run the calculation with the highest values of S1, S2, S3, and plastic strain, and the lowest Seq from anywhere in the model and it passes, this would be conservative and you'd be okay everywhere. Finding the worst individual location without actually evaluating the limit everywhere would require quite a bit of judgment. Areas with high triaxility (S1+S2+S3) or high plastic strain are most likely to fail. So you could target areas where S3 is positive or S1 is very large, regardless of plastic strain, and also areas where plastic strain is significant, regardless of triaxility. High triaxility tends to occur in areas with a lot of restraint (i.e., notches). Again, though, this requires a lot of judgment and doesn't really meet the letter of the code. If you evaluate the plastic strain limit everywhere, the computer does the work and you just need to look for values greater than 1. It's quite a bit faster.

-mskds545

 

[IdanPV]

Hi mskds545,
Questions for you and others:

1. Regarindg this: " If you evaluate the plastic strain limit everywhere, the computer does the work and you just need to look for values greater than 1. It's quite a bit faster."
and this: "what I've typically done is create a user defined result of plastic strain / local strain limit and create a contour plot of that ratio"
How can I do it using SolidWorks Simulation?

2. Is there any mesh setings requirments for the elastic-plastic method?
I know that for the elastic analysis, you must have enough elements through the thickness in order to get an accurate SCLs.
But, what about the elastic-plastic method?

What I have done so far is to create this table from the FEA results:

But, I don't know if it's enough.
The ratio of plastic strain / local strain limit is greater than 1 for each element I checked...

 

[mskds545]

I don't use Solidworks, so I can't advise you on the software. For mesh settings, your stresses and strains should be converged to make the results meaningful. I'm not sure what to say beyond that. Regarding your table, you are calculating local strain limit / plastic strain, rather than plastic strain / local strain limit. The limits you calculated are all greater than the plastic strains you calculated. This would be acceptable, so long as your math is right, your model is right, and there is no forming strain to account for as in Eq. 5.7.

-mskds545

 

[IdanPV]

mskds545,

Thanks for your help.
Regarding my first question, any SW user here can help?

One more question regarding the use of SolidWorks to meet the requirements of ASME VIII-2:
Accrpding to ASME VIII-2 Part 5, 5.2.4.4: "Perform an elastic–plastic analysis for each of the load cases defined in Step 4. If convergence is achieved, the
component is stable under the applied loads for this load case."

How can I know if convergence is achieved in solidworks?

 

[mskds545]

Convergence in this context just means 'found a solution'. Plastic collapse is all about maintaining static equilibrium in the structure. If the plastic strains start to go unbounded, the solver will crash. The last time step before it crashes is the last time step where convergence was achieved.

The elastic-plastic local failure criterion is a bit of an oddball part of the code that is not well documented outside of the code itself. Plastic collapse, however, is absolutely fundamental to the design of pressure vessels by analysis. If you are designing real pressure vessels, I'd strongly recommend you take a training course and find yourself a good mentor. The code allows the lowest design margin when designing with the most opaque and error-prone method, i.e., design-by-analysis. Getting it right is a great responsibility, as others are putting their safety in your hands.

Also, you should consider posting these questions to the pressure vessel forum. You'll probably get more opinions there.

-mskds545

 

[IdanPV]

Hi mskds545,

"The last time step before it crashes is the last time step where convergence was achieved."
How can I find this point using the SolidWorks Simulation Slover, any SW users can help?

I am not designing a real pressure vessel,I just want to learn.

Training course is something I would like to do, but the Coronavirus just ruined my plans.
Maybe next year.

Thank you very much for your help, here and in the ASME (mechanical) Code Issues Forum.

 

[mskds545]

Glad to hear that, and sorry, I didn't mean to jump all over you. I just see a lot of bad FEA out there and the rising popularity of design-by-analysis concerns me a great deal. Keep asking questions, and keep learning. To your question, if you run the model and it produces an answer, it converged. There can be some mesh- and timestep-sensitivity in some cases, but it usually isn't anywhere near as sensitive as elastic methods.

-mskds545

 

[IdanPV]

Hi mskds545,
Thank you for your answers.

As for this question:
"The last time step before it crashes is the last time step where convergence was achieved."
How can I find this point using the SolidWorks Simulation Slover, any SW users can help?

Can someone please advise?