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.

 

[marine59]

Fixed boundary conditions aren't real, but an approximation to a real-world condition. As you mesh finer, the calculated stresses converge on the theoretical values you are calculating by hand, which are also not real.
All boundary conditions are an approximation.
I use ANSYS. I always use nodal stresses (which I can select in ANSYS) averaged in the manner of my choosing.
For relatively brick-like elements, I get more continuous stresses than the element stresses. And avoid the harshly unrealistic presentation of element stresses.
Nodal stresses typically average the (<=6) stresses around them.
Elemental stresses are at the center, not the fixed boundary.
One of the things that has always bothered me about element stresses is the integration-point stresses from which they derive. Plot/list them and you may see what I mean.

 

[rob768]

Even worse: fixed boundaries shouldn't be considered at all. After all, the fixing removes them from the problem, and the presented results are averaged from the rest of the model.

 

[corus]

You might find that the FE results are different from hand calculation results as the latter don't consider other effects such as shear or the restraint on poisson's effect. Stresses at the integration points are the most accurately calculated for that position. These stresses are extrapolated (to put it simply) to the nodal positions from which all the element nodal values at that point are averaged. Poor element shape or large elements will make that extrapolation process less accurate.
Boundary conditions do not remove nodes from the problem and the stresses there should be considered, as elsewhere. In some situations a fixed boundary condition may be considered over conservative, such as that provided by bolted joints. The results there may be unrealistic but should not be dismissed for that reason.

corus

 

[vonlueke]

ksmub: (1) What type of elements (solid, shell, or beam) are you using for your cantilever beam finite element model? How did you constrain it at the fixed support? (2) What is the length to depth ratio of your cantilever? (3) What is the percent error between your FEA and theoretical stress?

 

[prost]

vonlueke:
The theoretical (exact solution) stress is infinity at the corners of the fixed boundary constraint, therefore the percent error between FEA and theoretical stress has no meaning.

Is there some sort of guidance about asking the same question in two different forums? We have two threads going here, same topic, same poster. If there isn't a good way to intertwine the two threads, there should be.

 

[ksmub]

Thank you all for the explanation.

Vonlueke, I created 2 models. One was a 2D plane stress and other was 3D model. Dimensions are 150x5x5 mm for the cantilever. I fixed both the models at one end. At other end I gave 100N of load. The elements I chose in ABAQUS for 2D model are 2D plane stress quadratic elements with reduced integration; for 3D model I chose quadratic 3D brick elements with reduced integration. I meshed both the models with same element sizes. 50 elements along the length and 4 elements along the thickness (and 4 nodes along the width for 3D model).

Bending stress values at the nodes
For 2D model- 706MPa at the fixed boundary, 715MPa in the node next to the boundary and 690 in the next node.

For 3D model- 686MPA at the fixed boundary, 742MPa in the node next to the boundary and 690 in the next node.

If we use simple hand calculations, Bending stress=720MPa (because MomentM=100N*150mm I=(5^4)/12 Distance of farthest point y=5/2 So stress=My/I)

I do not have further mesh refinement calculations. But based on the explanation I got from the forum, since stress at the boundary is infinite, I assume that as I further refine the mesh by adding more elements along the length, the stress values at the boundary continues to increase due to the fixed boundary conditon. But the stress values after small distance from the boundary will stabalize.

Prost, I also posted the exact same question in another forum. Earlier I posted the question here. But then I found Finite element forum. Since that was the first time I started using this forum, I was not sure where to post it. So I posted it in that forum too. Next time, I will avoid multiple postings of same question.

Thank you all for the inputs. This was really helpful.

 

[rob768]

Corus, proper boundary conditions do not remove nodes, fixed boundaries do, and that was the remark of ksmub.

 

[vonlueke]

ksmub: Taking a look at your 2-D model, I assume the z axis is vertical, and your tip load is applied in the z direction.

First, your mesh is slightly coarse at the fixed support. You might try refining your mesh near the fixed support, if you wish. Secondly, if you've constrained all nodes at the fixed support against Tz, you are setting up a Poisson effect at the fixed support. You might try constraining Tz only at your neutral axis node, to eliminate the Poisson effect, since you're only trying to match theoretical results.

When I constrained Tz only at the neutral axis node on the 2-D model described in your previous post (using 8-node quadratic quadrilateral elements, and 9 nodes constrained at the fixed support), I obtained sigma_x = 722.19 MPa at the fixed support, which differs from your theoretical stress by 0.304%. When I refined the mesh near the fixed support to 0.25 by 0.25 mm mesh (much smaller than what you need), I obtained sigma_x = 721.84 MPa at the fixed support, which differs from your theoretical stress by 0.256%.

 

[corus]

Another effect not mentioned is that the 3D model will include some plain strain effects, whereas the 2D plane stress model will not. This will affect the results across the width of the beam by a small amount in this case.
As vonleuke points out (and as I did previously) a full restraint will suppress posson's effect in one direction in 2D, and in 2 directions in 3D. This will accumulate at the corner nodes in the 3D model to give you higher stresses there. The stresses won't be infinite though.
If reailty says that there is no full restraint then to match theoretical values use a symmetry type restraint at the end of the beam, together with a single node (or nodes in 3D) restrained vertically to prevent rigid body motion.

rob768, What is a proper restraint as opposed to a fixed restraint?

Nice homework question anyway.

corus

 

[rob768]

Fixed with constrain all 6 DOF, whereas a proper defnition would allow displacements or rotations in certain directions (depending on the model and the boudary conditions).

 

[krepus]

just to pitch in, i think the discrepancy between the exact solution and the result from FEA is due mainly to the very idea that FEA is an approximate method of solving diferrential equations by discreteizing the problem domain and by using some functions to interpolate the results at gauss points (or integration points)to the nodal points.

cheers.

josh