Stress at fixed boundary condition

[ksmub]

Hi, I recently started working on Finite element analysis. Is it correct that the stress values at the fixed boundary condition are not realistic? I created a simple cantilevered beam and therotically calculated the bending stress values at the fixed Boundary Condition (B.C). Even with mesh refinement, the FEA stress values at the fixed boundary were slightly different from therotical value. I think that this difference increased when the mesh was corser. So I was thinking that I should not believe the stress values at the fixed BC and at tie regions. I was thinking that the stress may be realistic at one or two elements after the fixed B.C or tie regions. But I do not know the reason why the stresses are not real at boundaries. Can anyone please explain me this?

I was going through the ABAQUS user manual, where they have a fixed B.C to a cantilever (a lug). The example determines the stress at integration point and reaction force at nodes on the elements at fixed B.C, when a bearing pressure load is applied on a hole at the free end. The example uses 20 node brick elements with 8 integration points for meshing.

Since the manual listed the stress value at the fixed B.C, I am not clear whether the stress value for the element invlolved in the fixed boundary condition are realistic? The manual listed the stress at integration point. When I created a simple cantilevered beam for comparison with theorotical bending stress, I was looking at the stress contour plot. I remember reading some where that the contour plot stress, plots nodal stress and that the nodal stress is the average of stress from the surrounding integration points.

So is it correct that I can believe in the stress values at the integration points for the elements at fixed boundary condition but I should not believe in the stress values listed for the nodes at the fixed boundary condition? But again, I read in the manual that for a good refined mesh, the stress at integration point should be close to the nodal stresses. The basic question still remains for me. Are the stresses at the boundary condition realistic and if not why? Please help me understand the concept clearly. Thank you.

 

[GBor]

I think you could probably find the answer to this question with a search of this forum...I believe it has been answered several times, but the brief version is that you are basically correct. Fixed boundary conditions are, in effect, infinitely rigid, so the tend to "absorb" stress. As your mesh becomes more refined, the distance between the integration points and the nodes becomes smaller, so the difference becomes less significant. Generally, you can move a small distance (this is obviously a relative term since to say "1 element" or "2 elements" will be different from model to model and modeler to modeler) from the boundary condition.

There are some specifics related to the integration points and their accuracy, but I'm not the person to answer that...not ABAQUS saavy.

Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.
Lower Alabama SolidWorks Users Group

 

[rb1957]

another thought, if you're using 3D elements ... the "simple" approach to fixing a boundary is to lock up all the freedoms of all the nodes. this over-constrains the elements (more than allowing the boundary to react moments) and contributes to higher stresses.

i'm also not an ABAQUS user, possibly the elements don't particularly like moments (like NASTRAN's CQUAD4).

 

[prost]

I like the explanation of GBor the best. It really matters little where you calculate the stresses; the key is the rigidity of the constraint, the fixed boundary condition. This constraint is too rigid to be realistic. Even in a real cantilevered structure, the attachment to the wall is not rigid, there is some give to it. You are using a model, linear elasticity (I didn't see a mention of plasticity, therefore I'll assume you aren't using nonlinear material models), to make an approximation of the material's behavior. If you are using the fixed boundary condition, the exact solution is infinite strain and stress at the corners. This is not realistic, since 1) no real support is this rigid, and 2) it clearly violates one of the key assumptions of the linear elasticity--namely, that the strains (stresses) remain 'small.' Nevertheless, you can still use the fixed boundary condition IF you are interested in strains (stresses) far away from the fixed boundary. The basic idea is to put a layer of small elements right at the area where you expect the infinite strain in the exact solution to isolate that area in your FE model, then ignore what goes on in this area. You would do the same thing with a crack tip--this isolates the numerical 'pollution' associated with trying to compute the infinite exact solution from the engineering data you are trying to compute away from the infinite strain.

Every engineering model of reality requires you to make certain key assumptions to reduce the problem of reality to something more manageable. With the wonderful tool of FEA, the best you can do is compute the exact solution for the model of reality you have made; systematic approaches for computing how far you are from the exact solution is different thread. Nevertheless, I think that it is possible to get good reliable FEA results if you always keep in mind what the goals of the analysis are--if you are interested in stress 'far away' from the support, you can use a different strategy than if you need stresses at the support.

 

[ksmub]

Thank you all for the suggestions. This was really helpful