Interpret CosmosWorks Results 5

[trascon]

Hi,
I am fairly new to FEA. I have a question regarding viewing/interpreting your results.

For instance, say I have a beam that is .014" thick and I put a force on one end of the beam and fix the other end.

As expected, I see a high stress location close to the fixed base. The von mises stress value is much higher than the materials yield strength. However this high stress area is only on the outer surface of the beam and only goes into the material about .002" of the .014" material thickness. I can see this when I do a section view of the plot.

How do I know if this material will fail or take some permanent set? Is there a percentage guideline of high stress area vs. overall thickness that will tell you how much this surface stress will effect the overall beam?

Thanks for the help

 

[GBor]

You have discovered one of the interpretational issues of FEA. Boundary conditions are basically infinitely rigid nodes of infinitely small area resulting in theoretically infinite stress. If you have an area of interest in a model, you need to make sure to model enough of the surrounding part so that boundary conditions do not affect the outcome of the analysis with false high stresses.

 

[trascon]

GBor,
So if I model enough of the surrounding area I can still apply enough force at some point that will cause the model to show stress well above the yield strengh but only on the surface. If I probe just below the surface area the material is below the yield strength of the material. How can I interpret how the material will behave?

Thanks

 

[BlasMolero]

Dear Trascon,
Without having in hands your FE model it is difficult to assess the quality & accuracy of your stress results: mesh quality is critical to have accurate results, you don't mention if you have used 3D solid TETRAxx or HEXAEDRAL elements. Ah!, you mention COSMOS then only possible to mesh with TETRA elements. In this case you will have to perform a solution convergence analysis test to check the accuracy of your solution, basically double the DOF of the model, rerun solver and compare stress results. If the stress results do not vary say more than 5% - 8% then your solution is mesh undependant, and you can validate your mesh. But this is only a part of the model: also you need to revise if the appliead loads & boundary conditions are correct. And if the problem is static or dynamic, linear or nonlinear, etc.. And the most important, do not rely in solid TETRA mesh solutions, I strongly suggest to use always Shell or BEAM elements when available.

In summary, let's suppose your 3D solid model results are correct and you have a plastic region in your model where vonMises stress is upon the yield limit. Well, I can tell you categorically that this is a bad design, not excuses, we are engineers and we have to do things correctly.

Please note linear static analysis do not exist, this is a simplification, in real life problems are nonlinear & dynamics, then a solution with a security factor = 1.0 is a risk. To solve a problem as pseudo-static you will have to take a look not only to displacements & stresses but also to relation between stiffness & mass distribution, ie, dynamic behaviour of the structure, to check if frequency of loads can affect to the response of the structure.

As you see, FEA is a serious task, not only pretty colours, but a tool for the engineer. Not matter the FEA tool you use, the important is try to be a good engineer.

Best regards,
Blas.

 

[GBor]

Every situation may be a bit different. When you say "probe just below the surface", knowing what element types and mathematical model you are using helps to know the answer to that question, but geometry plays a role.

Considering how new you are to this field, I strongly suggest you contact your reseller/dealer and speak to them about some basic training. Even some videos or something that goes in to greater detail about where FEA ends and engineering judgment begins.

FEA is just a tool...it is not a replacement for using your brain. Have an idea before you start an FEA. Do a handcalc that should at least give you an order of magnitude. Learn about mesh sensitivity and convergence criteria. There is a lot more than just getting a graph of 'pretty colors' and believing the answer.

Garland

 

[johnhors]

Trascon, by your description I assume that you have modelled a cantilever. In reality it never actually exists, no support is ever infinitely rigid. A cantilever is a theoretical mathematical curiosity. The theory of FE is based on a homogenous continuum, for which it works very well. FEA abhors any discontinuity in the "continuum", because the theoretical basis of the method breaks down, it is a singularity or in simple terms it becomes invalid. A rigid clamp of a cantilever is the most severest form of discontinuity that you can apply to a model. As Gbor points out the stresses at the support are infinite and no amount of mesh refinement will improve the situation.

There is an alternative and much better approach:-

Consider the free body diagram of the part, for a cantilever you have the "free" end where you have applied your force (hopefully not as a point load but as distributed load over a finite area or in other words a pressure). For the so-called "fixed" end, your free body diagram should show an equal and opposite load plus a moment, to produce static load equilibrium.

Therefore rather than apply supports, apply the balancing load and moment instead (all as pressures!).

You still have to apply supports to get the problem to run, but do this using minimal 3-2-1 supports that remove the rigid body motions WITHOUT affecting the results (discussed several times on this website).

Do this procedure correctly and you will not have any artificial infinite stresses anywhere in your results.

http://www.Roshaz.com

 

[GBor]

Sorry I didn't refresh my screen before sending my last post...looks like I duplicated Blas in a lot of my rambling.

Follow the link on johnhors post (

http://www.roshaz.com).

I'm sure you can find a paper on 3-2-1 supports. Even if you don't adhere to the principles, the logic helps you understand what you are seeing.

Have fun with FEA...I sure have for the last 13 years!

 

[kellnerp]

...this high stress area is only on the outer surface of the beam and only goes into the material about .002" of the .014" material thickness.

Think about what is happening. You modeled a cantilever which means there is a high moment where it is attached to the fixed base. The connection has to create an equal and opposite moment to that caused by the load on the end of the beam. So to create a moment only the outer surface of the beam is going to be highly stressed. What you are seeing is what is to be expected.

Now the other part of your question is whether those high stresses indicate failure. To answer that there are two issues. One has already been discussed and that is whether the FE model is showing the actual conditions that exist where the beam is attached. Let's say however, that they are accurate. When a beam is in bending the outermost surface sees the highest stresses. When that outer surface see stresses high enough to yield the material then the material will begin to yield and the outer surface is taking up all the moment it can. If the moment increases then yielding will progress through the thickness of the beam till it reaches the neutral axis. At that point the beam is resisting all the moment it can and there will be what is called a plastic hinge at the attachment point.

In your case you probably don't want yielding so any stress higher than the yield allowable should be avoided. At that point you have to ask whether your boundary conditions truly represent what is really happening. You might have to model the attachment and use contact to really see what is going on.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[corus]

Follow the guidelines of design standards for assessing stresses. Generally the surface stress in a structure will repreent the direct (membrane) plus bending (primary and/or secondary) plus peak stress component. Each, and in combination, will have different allowable stress limits. In simple terms the direct stresses are limited to about 2/3 yield, sometimes 60% of yield. Direct plus bending are limited to the yield stress or less. If you have a very high stress above yield at a 'hot spot' then that would be considered as a peak stress and limited by fatigue damage criteria.
For modelling pruposes, use which ever element is appropriate for the geometry and amount of detail you wish to include. Shell and beam elements can be used if you just want to capture membrane plus bending stresses. Use solid elements if the stress distribution is likely to be non-linear through the thickness and if you want to capture more detail.

corus