February 18, 2018 at 12:27 pmminkoSubscriber
Hi I have question about singularity and cnvergence.I have easy static structural problem. I have reactangle at one side fixe at second is applyied force. But I don´t uderstand convergence and singularities.
At the image you can see there are singularities at sharp corners but is possible to remove them? Or is some exact way to say how exacty stress is? In hand calculation it shoud by 13 MPa but in sharp corners is 28 MPa. How i can say from this image how much stress is there?
I do some convergence but what this curve mean? It mean that it never convenge becouse there are singularities?
February 18, 2018 at 1:33 pmpeteroznewmanSubscriber
If you explain the supports and loads fully (or attach an archive), it will be easier to offer suggestions. For example, are those two edges selected to apply a force? Applying a force to edges of a 3D solid results in a singularity because the theoretical stress is infinite since the area is zero. The solution is not infinite because the elements have a finite area, but as the elements are reduced in size, the stress increases without bound. If you put a convergence plot on those edges, the plot would just keep going up and never level off. Apply the force only to faces to avoid that.
Many times, a fixed support creates these kinds of stress concentrations that are undesirable. The stresses calculated are real. For example in a simple tensile test of a straight rectangular sample, the normal stress along the tension line cause a Poission's Ratio effect orthogonal to the tension line. At the clamps, a stress is generated due to that effect. That is why tensile test samples have the "dog bone" shape that flares out to a wider portion where the clamps hold the sample. Otherwise the straight sample would always fail at the clamps! This is not a singularity, and a convergence plot would show the stress leveling off. However, a hand calculation for a straight tensile test would not include the stress from the clamp, so if you are trying to compare an FEA result with a hand calculation, you have to have a way to ignore the elements near the stress concentration. One way to do that is with a multibody part. Slice your sample a little distance away from the clamp. Then plot the results on the body that does not have the fixed support on it.
Sometimes the geometry is symmetric. In the tensile test example, you can eliminate the stress concentration of the clamp by doing a quarter model. Slice the sample along the length, x, and through the thickness, z, and apply an x=0 and z=0 Displacement support on those two slice faces. Then instead of a fixed support on the clamp end, you can have a y=0 Displacement support. Now there is no constraint preventing the material at the clamp from moving in the y=0 plane and no stress concentration appears.
February 18, 2018 at 7:02 pmminkoSubscriber
There is attached file look at it
February 18, 2018 at 8:11 pmpeteroznewmanSubscriber
The symmetry method delivers the hand calculation result. The force has to be cut in half along with the geometry.
February 19, 2018 at 7:09 pmminkoSubscriber
- 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.