# Why do the stresses increase near the supports?

edited December 2020

In the ANSYS, if we plot stresses near a support, specifically fixed support, we see that the stresses are pretty high there, relative to the rest of the structure. Why is that? What is the practical reason behind that? Is that some kind of a numerical glitch, or we would expect that to happen in the reality as well? [ofcourse the support will not be infintely rigid in reality, but still would be see a similar stress concentrations near the fixed supoorts]?

If anyone can explain in a little dept, by the use of equations or laws, that will be very much helpful. Thank you.

• edited December 2020 Accepted Answer

Poisson's Ratio causes the high stress at the Fixed Support on a rectangular plate subject to an axial tensile force.

You can see Poisson's Ratio happening on the plate because it got narrower when it got longer, and that is the definition of Poisson's Ratio.

At the fixed support, the material is trying to get narrower, but the constraint prevents that, which creates stress.

If you edit the material properties and type 0 for Poisson's Ratio, then there will not be a high stress at the fixed support because the material will not be trying to get narrower.

Another way to eliminate the high stress without changing the material Poisson's Ratio is to replace the Fixed Support with a Displacement where X=0, Z = 0 on the edge, while leaving Y Free on that edge. Choose one vertex in the corner and set Y = 0. For a shell model, this is not enough constraints, since the plate can rotate about that edge, so the Fixed Rotation can be added to support the remaining DOF. The plate will get narrower and shrink toward the constrained corner point, avoiding any stress in the Y direction.

• edited December 2020 Accepted Answer

The animated GIF above illustrates Newton-Raphson iteration. The blue line is an unknown function, y = f(x). The search begins at an initial guess of x called x1. The value of y is computed and the slope at x1 is evaluated. Follow the slope down to Y=0 to get the next value of x called x2. Evaluate the function y2 = f(x2) and the slope at x2. Follow the slope to Y=0 to get the next value of x called x3. Continue the process until the evaluation of Y is close enough to zero to stop. @Rameez_ul_Haq

ANSYS uses Newton-Raphson iteration to converge the solution of a nonlinear static structural model to the point of equilibrium. Equilibrium occurs when the difference between the internal forces and the applied forces becomes zero, like y = f(x) in the function above but in ANSYS, there is a vector of unknown displacements {x} to iterate on.

• Why does a large change in stiffness result in a failure to converge?

Consider this highly nonlinear Force-Displacement graph shown below.

Try applying the iterative Newton-Raphson method on this function to find the unknown value of x for an applied load of Fa. Draw the sequence of trial values of x, starting at 0, and see how following the slope at each trial value will shoot the next trial value away from the correct value. The solver will only make a few iterations to try to converge on the correct value before it gives up. By forcing the solver to take many substeps, it should succeed in finding the correct value.

• edited December 2020 Accepted Answer

The singularity at the corner node is a mathematical artifact of the finite element method, which delivers an infinite stress at the corner.

Away from the corner, there are , in reality, internal forces that are equal and opposite from the top half to the bottom half that stretch the material out to the fixed dimension at the base. The Vector Principal plot will show the arrows horizontal at the right end, but changing angle to point toward the top and bottom corners at the left end.

• edited January 13 Accepted Answer

They are all the same error but there can be different corrective actions based on the shape of the N-R Force Convergence Plot. Look at the image below. See how from iteration 40 to 56, the purple curve was almost about to cross the aqua curve and convergence would have happened, if only the solver kept iterating, but it stops after 26 iterations.

The corrective action is to tell the solver to keep going with the NEQIT command. Read this discussion:

https://forum.ansys.com/discussion/2550/understanding-force-convergence-solution-output

Then there are the N-R Force Convergence Plots where the two curves just remain parallel and never trend toward crossing one another. In that case, more iterations won't help.

This lack of convergence is sometimes caused by elements that are too large or poorly shaped, and cannot find equilibrium. The corrective action is to remesh with smaller, better shaped elements. But you have to know which elements have the problem, and this is where the maximum value on the Newton Raphson Residual plots under the Solution Information folder show you where those elements are.

• When a highly distorted element error stops the solver, it is often the case that more substeps will solve that issue. Note that there is a difference between an error stopping the solver and the solver failing to find convergence.

«1

• @peteroznewman, if you can answer this please, I would be so much thankful.

And also, I want to ask the reason why does the 'LARGE DEFLECTION ON' analysis sometimes not converge at directly 1s, and we have to apply the loads in parts (i.e. substeps) to make the analysis converge? What is the practical and theoretical reason behind that?

• About your first question: more information is needed to answer it. What is your model? How it looks like? What impacts are applied? What is the material? High stresses rate close to the supports can be related to big deformations of the model, in my opinion. Try to reduce the mesh size.

About the second question: you can read about this option here. Briefly, large deformation of the model applied on 1 step leads to big stiffness changes and the solution cannot converge in 1 s.

• @ValiullinDamir, I am just talking about a regular plate, as can be observed in the picture below.

Just considering static analysis, it is most of the times seen that the stresses near the fixed supports are very high. Rather it be a face of a solid, or an edge of a shell model. What is the scientific reasoning behind that?

I mean if you also consider a horizontal plate lying on top of two rectangular columns, and then uniform pressure is applied on top of horizontal plate. Assume I am going to make a structural analysis of this, and I only consider the horizontal plate in the analysis (ignoring the columns), then the connections of the plate (to the columns) can be considered as fixed support because the columns are relatively very rigid. The results will show me high concentrations near these fixed supports, and I would also expect them in reality [because there is literally penetration of the columns into the plate where they are connected, and force concentration due to reaction means high stress concentration in the plate there].

But I want to know why and how does the solver know that near these fixed supports, the stresses should be relatively higher there in the plate?

And also about the big deformation thing you mentioned, the deformations near the support are the least, but the stresses are the highest, WHY?

I have already read the document which have linked, but my question is why does large changes in the stiffness [or stiffness matrices] would lead to the solution becoming uncoverged?

• also, can this be explained that why does this create a problem for the solver in ANSYS? How and why the excessive distortion/thickness change is a problem for the solver?

• @peteroznewman, will you please be able to clarify the concept here? I would be extremely grateful.

• Anyone on this one please?

• edited December 2020 Accepted Answer

Poisson's Ratio causes the high stress at the Fixed Support on a rectangular plate subject to an axial tensile force.

You can see Poisson's Ratio happening on the plate because it got narrower when it got longer, and that is the definition of Poisson's Ratio.

At the fixed support, the material is trying to get narrower, but the constraint prevents that, which creates stress.

If you edit the material properties and type 0 for Poisson's Ratio, then there will not be a high stress at the fixed support because the material will not be trying to get narrower.

Another way to eliminate the high stress without changing the material Poisson's Ratio is to replace the Fixed Support with a Displacement where X=0, Z = 0 on the edge, while leaving Y Free on that edge. Choose one vertex in the corner and set Y = 0. For a shell model, this is not enough constraints, since the plate can rotate about that edge, so the Fixed Rotation can be added to support the remaining DOF. The plate will get narrower and shrink toward the constrained corner point, avoiding any stress in the Y direction.

• @peteroznewman, thank you for clarifying things here :)

Will you be able to explain why does large changes in the stiffness [or stiffness matrices] would lead to the solution becoming uncoverged?

[Side Question: Consider the beam below;

Two beams with equal and same cross section. At the shared topology region, I should expect a stress concentration I think, because there is a sudden change within the properties of the structure, where the load is flowing. I know this. I want to ask that why should I expect a stress concentration there? I mean that some say that there is a sudden change in the stiffness matrix at the shared topology region, thats why there is a stress concentration, but why would the sudden change in the stiffness matrix due to sudden change of material properties cause a stress concentration. Will it be there on both the beams? Will it happen in the reality as well?]

And also why does an excessive thickness change or excessive distortion within an element is a problem for the solver? I know there are some tricks to avoid this error, like increase the thickness of the structure so that the stiffness increases and hence the high distortion can be suppressed, and also apply the forces in substeps (please name a few more, if there are any), but I want to ask why do we need to do that? I mean why can't the solver converge without applying any of these changes to my model?

If the solver cannot converge due to excessive thickness change or distortion of an element, what about reality then? Is the structure failing under the same circumstances, or not failing, or something else? Thank you.

• edited December 2020 Accepted Answer

The animated GIF above illustrates Newton-Raphson iteration. The blue line is an unknown function, y = f(x). The search begins at an initial guess of x called x1. The value of y is computed and the slope at x1 is evaluated. Follow the slope down to Y=0 to get the next value of x called x2. Evaluate the function y2 = f(x2) and the slope at x2. Follow the slope to Y=0 to get the next value of x called x3. Continue the process until the evaluation of Y is close enough to zero to stop. @Rameez_ul_Haq

ANSYS uses Newton-Raphson iteration to converge the solution of a nonlinear static structural model to the point of equilibrium. Equilibrium occurs when the difference between the internal forces and the applied forces becomes zero, like y = f(x) in the function above but in ANSYS, there is a vector of unknown displacements {x} to iterate on.

• Why do I see a stress singularity in these red marked regions, and no where else @peteroznewman?

And the reason given is this:

I didn't understand why the corner nodes should enforce a free edge condition i.e. Normal stress equal to zero? And how does it actually cause a singularity within FEA?

• Why does a large change in stiffness result in a failure to converge?

Consider this highly nonlinear Force-Displacement graph shown below.

Try applying the iterative Newton-Raphson method on this function to find the unknown value of x for an applied load of Fa. Draw the sequence of trial values of x, starting at 0, and see how following the slope at each trial value will shoot the next trial value away from the correct value. The solver will only make a few iterations to try to converge on the correct value before it gives up. By forcing the solver to take many substeps, it should succeed in finding the correct value.

• @Rameez_ul_Haq that was a very good article, thank you.

This video explains the difference between an acceptable singularity and a stress concentration. https://www.youtube.com/watch?v=-OHXl-mvR5U&ab_channel=DatawaveMarineSolutions

Here is a good video on singularities. https://www.youtube.com/watch?v=ZP9nh4GOkIc&ab_channel=SimuTechGroup

A simple way to understand a singularity in FEA is when a point force is applied to a single node on a solid body. Stress = Force / Area but the area of a single node is zero, and when you divide by zero, the answer is infinity.

In the clamped end example above, the material is shrinking in the Y axis due to Poisson's Ratio. Away from the clamped end, the Y component of stress is zero. There is a Y component of force on each clamped node (except the center node is zero) to stretch the clamped edge to its fixed value. The Y component of force gets larger the further the node is from the center on the clamped edge. But there is no area at the corner node.

• Thank you @peteroznewman, I saw the video and it was quite helpful into getting an insight that how is a singularity actually caused because of mathematics in the solver's background.

However, I want to ask one more thing here. Since you can see in the picture that I have shared already, there is a stress concentration near the fixed end, and it persists for a few elements before it. I am just applying a force in the X direction initially on the right end, and I know that there must exist a vertical Y direction force on the nodes in the left end. But for some length/elements before the fixed end, the stress concentration indicates that there is also a force there in the Y direction. At the same time, I have only applied an external force in the X direction. So what I want to ask is that this Y direction force will also influence the load path in that region of the structure, which we should experience just because of the external force applied in X direction? What I mean to say is that the overall load path in that region will be a combination of the X force and also the Y force experienced there, right? IN THE REALITY as well (assuming the boundary condition implemented exactly mimics the reality).

• edited December 2020 Accepted Answer

The singularity at the corner node is a mathematical artifact of the finite element method, which delivers an infinite stress at the corner.

Away from the corner, there are , in reality, internal forces that are equal and opposite from the top half to the bottom half that stretch the material out to the fixed dimension at the base. The Vector Principal plot will show the arrows horizontal at the right end, but changing angle to point toward the top and bottom corners at the left end.

• @peteroznewman, thank you once again. So what you have said implies that the stress concentrations which starts to form a few elements before the left end boundary condition is real because of the existence of force in the Y direction at the left end. This force in the Y direction actually makes the stresses in those few elements to rise, and the load paths (or the vector principal stresses) will be a result of the stress in the X direction (due to external force) and the stress in the Y direction (arising due to fixed left end boundary condition).

How do we determine critical distance, in this case, of the singularity happening at the top and bottom corner nodes of the left end? [beyond which the St. Venant's principal is going to be valid].

• The distance for a stress disturbance to be significantly reduced is 2 times the maximum dimension in the cut face. It is not a critical distance, just a guideline.

You other question shows an example of this. https://forum.ansys.com/discussion/comment/101294#Comment_101294

Here is a video on that. https://www.youtube.com/watch?v=Fv23fkX0YhQ

• @peteroznewman, since we have already discussed about the convergence of the solver in this thread, I won't be opening another thread and will try to ask my concern here.

While conducting some analysis, I encountered an error something like this.

*** ERROR ***

Solution not converged at time 0.1.

OR

Solution not converged at time 0.5 (or 0.6 or 0.7 or 0.8)

OR

Solution not converged at time 1.

I want to ask how are these errors different from each other?

What kind of factors can cause these errors to occur? A general idea would help. Can geometry be a problem, maybe mesh, maybe boundary or loading condition, maybe contact, or something else? How could any of these be a problem for convergence?

• edited January 13 Accepted Answer

They are all the same error but there can be different corrective actions based on the shape of the N-R Force Convergence Plot. Look at the image below. See how from iteration 40 to 56, the purple curve was almost about to cross the aqua curve and convergence would have happened, if only the solver kept iterating, but it stops after 26 iterations.

The corrective action is to tell the solver to keep going with the NEQIT command. Read this discussion:

https://forum.ansys.com/discussion/2550/understanding-force-convergence-solution-output

Then there are the N-R Force Convergence Plots where the two curves just remain parallel and never trend toward crossing one another. In that case, more iterations won't help.

This lack of convergence is sometimes caused by elements that are too large or poorly shaped, and cannot find equilibrium. The corrective action is to remesh with smaller, better shaped elements. But you have to know which elements have the problem, and this is where the maximum value on the Newton Raphson Residual plots under the Solution Information folder show you where those elements are.