March 16, 2020 at 4:21 pmhwa0725Subscriber
I am trying to analyse a simple cantilever shear wall (Height: 72m; Breadth: 6m; Thickness: 0.275m) with a pressure of 110897 N/m2 applied to the surface of thin side (its thickness) and the stress calculated from ansys does not match with the bending stress I have calculated with simple analytical equation like moment, M = (wl^2)/2 and bending stress = M*c/I.
I had tried meshing the solid with quadratic solid186 with 3 elements across the gap (i.e. thickness) and also tried to sweep the solid with solid shell 190 with 5 element across the gap. Both of these gave very different answers and does not seem to agree with my analytical calculations. I am sure the mesh is fine enough, finer mesh will take too long to solve. Not sure why is this happening and it would be great if someone can point out a few things that I can tweak to get better answer.
Thanks very much for any help! Much appreciated!
March 16, 2020 at 8:37 pmpeteroznewmanSubscriber
Where are your hand calculations? Where did you come up with a pressure load of 110897 Pa? That sounds like air pressure. You don't apply that to a cantilever beam. A more realistic pressure is 50 Pa.
I created a surface with the length and width of the beam and assigned the thickness.
Hand Calculation = 0.485 m
ANSYS Deformation = 0.482 m (-0.6% error)
Hand Calculation = 10.3 MPa
ANSYS Stress = 10.4 MPa (1.5% error)
If this answers your question, please mark the post Is Solution to make the discussion Solved, or ask a followup question.
March 16, 2020 at 9:04 pmhwa0725Subscriber
Thanks very much for your reply!
My apologies for confusion! The pressure load of 110897 Pa is actually a wind pressure (windward pressure + leeward pressure (suction)) that is acting of the thin side (72m x 0.275m) of a concrete shear wall. Also I have attached picture for my hand calculation and the a test model in .wbpz format. Thanks and appreciate your help!
March 17, 2020 at 3:50 ampeteroznewmanSubscriber
(1) Is this beam standing in the wind or is it inside a building? Because the aspect ratio is so high, 6 to 0.275 is about 22 to 1, what you have is more like a wing than a building. A small change in the angle of the wind will create large sideways forces. Also the sideways flexibility combined with the vortex shedding that may develop can set up an oscillation that will create large dynamic forces.
(2) How did you come up with the value of Pressure load due to wind. Here is a Cornell University webpage. Using such high aspect ratio might take this calculator out of its valid range, but anyway...150 mph is 241 km per hour.
Convert the maximum pressure of 62 psf and you get about 3,000 Pa, not 111,000 Pa. How did you derive the value of pressure?
March 18, 2020 at 12:35 pmhwa0725Subscriber
Thanks for your concern, they were great! Perhaps, I should have descript a bit more regarding what I am doing.
(1) The Shear Wall I mentioned is actually part of a Core Wall (on plan: 6m x 6m, 0.275m thick) which is located at the center of the building, which on plan measures 18m x 18m. The total height of the building is 72m that consists of 24-stories of 3m floor-to-floor height. This is a modular buildings and the number M #01 ... M #16 are individual modular units which is prefabricated and prefinished in the factory and will be dropped into place floor by floor.
The reason the shear wall seems relatively thin is because I would like to only analyse the A-A section as shown in plan below. I have inserted a Frictionless Support that scoped to both the front and back of the Shear Wall and apply the windward and leeward (suction) pressure to the left and right side of the Shear Wall respectively.
(2) The wind velocity is calculated based on the Eurocode together with Local Annex. The wind velocity I had was about 90 kmph, which is about 56 mph. After converting it into a pressure, I ended up with +1205 Pa (windward) and -1054 Pa (leeward) wind pressure which add up to the 2259 Pa. This pressure 2259 Pa is then splitted into 2 as it will be resisted by 2 shear wall. So half the width of the building (18m/2) multiply by this sum of pressure acting on the facade would be the pressure carried by 1 Shear Wall. The resulting pressure need to be multiply by 1.5 (partial safety factor) to get to the final value which is around 30496.5 N/m. If I were to convert this back into a pressure acting on the side of the Shear Wall, this would be, 30496.5/0.275 (the thickness of Shear Wall) = 110897 Pa.
Hope this clarifies a little. Thanks very much for you help! Cheers!
March 21, 2020 at 8:40 pmhwa0725Subscriber
Also, mesh convergence study has been performed and not much luck seeing the stress at support converge but rather, diverge! The finer I go, the further it gets, not sure what went wrong to be honest. Could it be the boundary condition? I used ansys mechanical "Fixed Support" by the way.
March 21, 2020 at 8:44 pm
March 22, 2020 at 3:28 ampeteroznewmanSubscriber
Here is the hand calculation for the Euler Beam Theory equations for your problem:
Here are the results from the ANSYS Beam model of that problem:
So you can see that a beam model almost exactly reproduces the hand calculation.
Here are the results from the ANSYS Solid model of that problem:
So you can see that a solid model almost exactly reproduces the hand calculation. I expect as I use smaller elements, I can get closer to the beam result.
March 23, 2020 at 5:23 pmhwa0725Subscriber
Thanks for the reply!
What type of mesh setting did you used to get the results of solid model? I have the same support condition and loading but the model is in concrete instead and I am getting stress increase every time I reduce the mesh size. That's strange!
First, I had a 3m mesh, I got 16.57 MPa, which is quite close to the value you are getting.
Second, I reduce mesh size to 1m, I am getting 18.29 MPa.
Then when I tried 0.5m mesh, I am getting 19.94 MPa.
It keeps incresing as the mesh size decrease.
March 23, 2020 at 8:37 pmpeteroznewmanSubscriber
Attached is my ANSYS 2019 R3 archive with the two models. I also checked if the normal stress was affected by Poisson's Ratio, but it wasn't.
You can look for where your model is different to mine.
March 24, 2020 at 10:09 pmhwa0725Subscriber
When I further refine the mesh you used, the stress shoot up again.
After a bit of research, now I know where this gets wrong! It was due to stress singularity at the fixed support! This issue only shows up when using ANSYS default Fixed Support.
This is a close-up snapshot of stress singularity at the toe of fixed end when using Fixed Support,
This is a better stress distribution using Remote Dispacement (with all dofs set to 0),
Also, the latter boundary condition shows no sign of divergence when the mesh gets finer and agree well with my hand calculation!
Anyway, thank you very much for your support and dedication! I wish you the best and stay safe and healthy!
March 24, 2020 at 10:38 pmhwa0725Subscriber
Also, for anyone that has the same issues as I did, stress singularity disappear only if you have a Remote Support (with all dofs set to 0) with a Deformable Behaviour! If you set this to Rigid Behaviour, it makes no difference to a Fixed Support and stress singularity will appear!
March 25, 2020 at 4:55 ampeteroznewmanSubscriber
You misunderstand the difference between stress increasing due to a singularity and stress increasing due to elements getting smaller.
I used a material with a Poisson's Ratio = 0 specifically to avoid non bending stress being caused by the fixed support. The stress at a singularity increases to infinity as the element size is reduced to zero. That is not happening here. Let me explain the stress increasing due to elements getting smaller.
Below is the Element Mean stress for the Initial Mesh. The Element Mean stress is the value of stress at the center of the element. This is the fundamental quantity computed in the solution.
The maximum element mean stress is 14.9 MPa which is measured at the center of that corner element.
Now cut the element size in half and the max stress increases to 16.0 MPa, because the element center is closer to the corner.
Cut the element size in half again and the max stress increases to 16.7 MPa, because the element center is even closer to the corner.
I can cut the element size in half again. The stress increases again. I can plot the maximum element mean stress vs these four element sizes and predict the max stress at zero element size. It is not infinite as it would be for a singularity. The plot below is what you do in a Mesh Refinement Study. This stress is at the center of the element in the corner, not the stress in the corner of the material. This plot has a steep slope because the measurement point is moving through the material from lower to higher stress levels.
There is another stress that can be plotted called the Averaged Stress, other programs call it Nodal Stress. That takes the stress at all the element centers connected to a single node and averages them. Then post processing interpolates across the element. This makes for a smooth result and the maximum value is the stress in the corner of the material.
Below is the Initial Mesh and the interpolation out the the corner is 17.246 MPa.
As the element size is cut in half, the averaged value increases to 17.469 MPa
As the element size is cut in half again, the averaged value increases to 17.656 MPa
If you plot these three plus the half again value, the slope of the Averaged Stress is less than the Elemental Mean because the measurement point is always in the corner and is not moving through the material as the element size is reduced.
Again, the Averaged Stress extrapolates the stress out to the corner. But this is not a singularity.
I hope you find this helpful.
March 25, 2020 at 11:04 amhwa0725Subscriber
This is indeed very helpful for a new ANSYS user like me! I will save this for future reference really!
Thank you very much for such a detailed explanation!
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- How to calculate the residual stress on a coating by Vickers indentation?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- whether have the difference between using contact and target bodies
- Colors and Mesh Display
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Massive amount of memory (RAM) required for solve
- What is the difference between bonded contact region and fixed joint
© 2022 Copyright ANSYS, Inc. All rights reserved.