Be aware that stresses in Fe analysis are always calculated at integration points, but are extrapolated to the surface in contour plots. this extrapolation may be correct, but it may also give results that are wrong by a large factor.

Check the results directly at the integration points and see how the gradient of the stress close to the surface runs.

Stress calculations also depend on the element type - use quadratic elements for elastic calculations if at all possible.

Dear Miss Mash,

I am not an ANSYS user, but your results does look extraordinary to me.  But as you have suspicion there may an error somewhere. I am sure error is not in the software.  You must also consider the piece is not good enough for the loading.

You haven’t said why you are determining SCF. If it is for the fatigue analysis, then SCF between 3 and 5 is quite common.

I also suspect you are doing elastic analysis. For this reason you are getting stresses in excess of the material yield. Codes of practice such as ASME section 8, dive 2 and 3, allows the localised stresses to be as high as twice of  the yield provided they don’t exceed the material UT. For definitions please see the code.

If you are designing the piece, then it is better to perform a no-linear analysis in which you define the material property and use Mises Plasticity.  Plastic strain a better measure for localised high plastic strains.

Having a fine mesh is a good thing as you will capture hot spot stresses. However, to capture strain correctly you need  the element size to be really small; several elements through the thickness.

I can have a look, if you can produce your model in Abaqus. I  am curious to know why you suspect your results.  

Be aware that stresses in Fe analysis are always calculated at integration points, but are extrapolated to the surface in contour plots. this extrapolation may be correct, but it may also give results that are wrong by a large factor.

Check the results directly at the integration points and see how the gradient of the stress close to the surface runs.

Stress calculations also depend on the element type - use quadratic elements for elastic calculations if at all possible.

Hi Dr Martin,

You have raised good point. we all do well to remember them.   However, if the  mesh is fine in high stress gradient  regions, the error due to extrapolation from the integration point to the nodal point is not outrageously high. 

I suggest to make mesh independence study, this way You will identify if max value moves to another mesh node.  

Hallo Miss Mash,

Please do check the following:

1. UNITS (Tonn, mm, N, etc) consestency.

2. Static loading magnitude.

3. Element type. Would be good if you have same element type for slave and Master (same type)

If Every thing is okay i would apply pressure and See if the stress value remains.

How was the result when your mesh was not that fine? As the picture tells, your mesh is too fine Sometime you May face numerical instabilities and other Assembly Matrix issue. I would not make it that fine! And try to romove element legth jumps! 

Please inform me which Material model you use ?

Many thanks for all your responses,

I am performing the structural analysis of an axial compressor vanes. These vanes are under pressure and thermal loads. The bigger part of the stress is due to thermal load.

Dear Sirous, as you mentioned, I am doing elastic linear analysis (with bonded contacts) to determine maximum stress. The considered criterion is that the max stress will be less than yield/n which n is the design factor.

You have raised a very good point. Maybe I should change the criteria and high local stresses may be allowed. But I do not know where I can consider high local stresses allowed. I am cheking the mentioned ASME code and nonlinear plastic analysis.  Also, I do not know where plastic deformation is allowed regarding fatigue life considering that vanes are under cyclic and static loads.

One problem is that with smaller element, stress becomes larger while max value place also moves (The smallest element size is 0.01 mm while the biggest size of model is about 15 cm). In addition, I checked averaged and unaveraged stresses. It is stated that their difference shows the necessity of making mesh finer. While there are big differences here, it does not change by reducing the element size. On the other hand, in Ansys workbench, there is a parameter named as structural error driven from strain energy. Although,I do not find any special limiting value for this parameter, Here, its maximum has occurred in the max stress positions.  These points specially the lack of stress convergence make me feel untrusted toward results.

Dear Martin, unfortunately very small quadratic elements are not possible. Although I could not check integration points stresses, there are very high stress gradient close to max value place.

Dear Tamer, I have used linear elastic material model. How can I get it weather high stresses are due to numerical instabilities?

I also cheked something else. I added the soild model of the braze to the model. In this way there is no gap between two parts of the contact. The result is very different and mesh independent

Hallo Fahimeh,

Answere to your question. Is simply to run the same Simulation with larger element size and See what happens if you get the same stress value.

Tips from my side:

1. In Order to understand yield and PlastiC Flow Limit you should use elasto-plasic Material model with tempratur dependency!  to See at which point yield ocours and how the vane behaves in plastic regime at x tempreture.

2. In Order to determine what is critical and what is not, you should answere the following question:

- How often does this vane feels such a load and how much is allowed in coustomer specification (cs)? Once a life time? 10 a life time? 1 000 000 a life time? Answere to this question can be usually find in coustomer requirments and specificarion.

3. After point 2. You should Performe fatigue Analysis! . Why? 

Because if linear elastic Analysis gives you acceptable stress value. This does not mean that this Part is okay in cyclic fatigue Analysis, where you may See much higher stress values which is not acceptable or too much high er than yield!. And i See your problem pure Dynamic! And offcourse it Dependes on you, how you idealize the problem. Such as you say an aircraft wing is a cantilever beam! Which is okay if you aware of the Daviation to reality!.

I belive you are doing well, howerver you May need much more input or Parameters and then you should deicide which Material model is important for you and which Analysis should be Performed to reach the Research gaol efficiently with min. Cost.

Regards,

Tamer

Thanks Tamer.  Today I have focused on dynamic behavior and modal analysis of the vane. I studied the natural frequencies and plotted Campbell diagram. Unfortunately, a resonance occur in operating speed of the aerodynamically designed vane. This resonance may lead to fatigue crack. Therefor, a modification should be performed either by changing the airfoil profile or by altering the thickness. But I still do not make a decision what to do.

The question was asked long before, but this answer might be useful for whoever facing these problem. The sharp corners are considered as singular points and the fact that refining the mesh increase the stress is something expected (the deformation result will not change and can be used for mesh independency). One solution to overcome this is to use a very fine mesh at the location with sharp corners and then use an average stress value of the adjacent cells. If the mesh is fine enough, the adjacent cells will converge and the value is pretty close the stress of the desired location.