April 7, 2023 at 9:53 amGokizaSubscriber
I have two interlocking rings that is below. I want to see the maximum stress that is between two rings. But I have a a problem about boundary conditions. Problem is temperature is increasing 22C to 100C and there is no boundary conditions on part even standart earth gravity. I need to think these ring on the table and there is no pressure, force, gravity vs. Just I need is which boundary conditions I can apply to these ring. And after that, which stress value should I look (Equivalent, Normal or Max.Principal stress) ?
April 7, 2023 at 2:16 pmpeteroznewmanSubscriber
Your title is 2D Plane Stress. That assumes the thickness of the rings in the Z direction is small compared to the diameter and stress in the Z direction is zero.
Or did you mean 2D Plane Strain which implies the thickness of the rings in the Z direction is large and the strain in the Z direction is zero. Probably not or you would have called the rings pipes or tubes.
In either case, you can use a Remote Displacement on the inner circle and set all three DOF to 0. Notice that I have made a Cylindrical Coordinate system to plot the Normal Stress in the X direction. For this model, the stress at the interface is -9.26 MPa.
You could build an Axisymmetric model which does not assume zero stress in the Z direction, it calculates stress in 3 directions: Radial (X), Axial (Y) and Hoop (Z).
Create new geometry in the XY plane for an Axisymmetric model. The 2 rings are represented as 2 rectangles on the +X side of the Y axis, which is the axis of rotation. In SpaceClaim, create a New Component called Inner and draw one rectangle. Create a New Component called Outer and draw the other rectangle.
In Workbench, make sure to set the Geometry cell property to Analysis Type 2D.
In Mechanical, make sure to set the Geometry 2D Behavoir to Axisymmetric.
Add a Y=0 Displacement boundary condition to one vertex. That properly supports the rings with no restriction on thermal expansion.
If you want the rings bonded at the interface, add a Bonded Contact.
If you want the rings to slip at the interface, add a Frictional Contact and assign a non-zero coefficient of friction.
Create a Normal Stress for the X axis, which is the radial direction. Now you see the variation in stress along the Y axis, which is the Axial direction. There are end effects but in the center, there is a region that behaves similar to the Plane Stress solution.
April 7, 2023 at 3:58 pmGokizaSubscriber
Thanks for your response, but I did not understand which method is more accurate plane stress or axisymmetric? And boundary conditions that you have given is not understandable for me. In 2D axisymmetric where I will apply the displacement on this geometry? Can you show me?
April 7, 2023 at 5:22 pmpeteroznewmanSubscriber
Plane stress is an approximation that assumes stress in the axial direction is zero. As you can see in the Axisymmetric solution, zero axial stress a poor assumption, especially as the thicknesss of the rings becomes larger, so axisymmetric is more accurate.
You can apply a displacement of X = Free, Y=0 to any one vertex. It doesn’t matter which one. The one point you pick is the point from which all the nodes will expand away from. You can only notice which one point was picked when you plot Deformation. If you plot stress, you can’t tell.
April 7, 2023 at 5:53 pmGokizaSubscriber
Thank you sir, If I have to apply remote displacement for Plane Stress version, Where should I apply in structure? and why did you apply the remote displacement? Does not applying the remote displacement to the inner circle restrict the expand of inner circle? Where did you apply remote displacement in the inner circle (Surface, inner edge or outer edge) ?
April 7, 2023 at 6:09 pmpeteroznewmanSubscriber
You need 3 constraints to allow the model to solve in Statics and Remote Displacement allows all three to be applied at a single point.
The Remote Displacement has the Behavior set to Deformable. This adds no stiffness to the ring. You can apply it to any one of the circles, I applied it to the inner circle.
April 7, 2023 at 6:17 pm
April 7, 2023 at 6:26 pmpeteroznewmanSubscriber
Yes, that is right. Do you have more than 4 elements across the thickness of each ring?
April 7, 2023 at 6:34 pmGokizaSubscriber
I have elements that is above. When I run the model from you description, I can't find any big differences between the two models. What is the reason of this? Maybe It can be from the material. Inside ring is stainless steel, other is titanium. Why are we looking normal stress for this case?
April 7, 2023 at 7:59 pmGokizaSubscriber
Hello again, I have solved problem that is about result between axisymmetric and plane stress. Difference is big right now. For 2d axisymmetric which results should I consider? Normal stress in X axis, in Y axis and Z axis. If there is much more than these, please let me know. Why do not we look from equivalent stress in 2D Axisymmetric? Why do we look from normal stress?
April 7, 2023 at 8:36 pmpeteroznewmanSubscriber
My model has larger differences because I used Magnesium and Titanium, which have larger differences in CTE than Steel and Titanium. Also my geometry is different with thicker walls.
Your model still had an 11% higher Normal Radial (X) stress in the Axisymmetric model than the Plane Stress model.
Plot the Normal Axial (Y) Stress in the Axisymmetric model and compare that with 0 from Plane Stress.
You can look at equivalent stress if you want. Normal stress lets you compare directions individually, while equivalent stress mixes them all up into one number.
April 8, 2023 at 4:51 amGokizaSubscriber
Hello sir, Do I need to look with Y axis from Plane stress in order to compare with normal axial (Y) stress in the Axisymmetric model? I did not ubderstand '' 0 from plane stress". Can you give more detail about that?
April 8, 2023 at 1:04 pmpeteroznewmanSubscriber
2D Plane Stress calculates Normal stress in 2 directions: Global X and Global Y and assumes zero stress in the Global Z direction. If you make a Cylindrical Coordinate System for a circular object like a ring in the XY plane, you can make Radial (X), and Tangential (Y) directions.
Axisymmetric calculates Normal stress in 3 directions: Radial (X), Axial (Y) and Hoop (Z). It does not assume zero stress in the Axial direction.
April 8, 2023 at 4:15 pmGokizaSubscriber
Hello again, When I look the normal stress result in X axis, Y axis and Z axis axisymmetric model, which coordinate system should I use? Global coordinate system or Cylindiricak coordinate system?
April 8, 2023 at 4:52 pmpeteroznewmanSubscriber
Use Global coordinates.
Axisymmetric calculates Normal stress in 3 directions: Radial (Global X), Axial (Global Y) and Hoop (Global Z).
The formulation of an axisymmetric model is implicitly in a cylindrical coordinate system because the Z direction is the tangential direction which we call Hoop because if you follow a point in that direction it goes around the circle and forms a hoop.
April 8, 2023 at 5:39 pm
April 8, 2023 at 6:38 pmpeteroznewmanSubscriber
That looks good. The inner ring has a compressive stress in the hoop direction, the outer ring has a tensile stress in the hoop direction.
April 8, 2023 at 7:34 pmGokizaSubscriber
Hello again sir, why do we assume radial stress on the x-axis in the axisymmetric model? Why does the axial stress occur on the y-axis in the axisymmetric model?
April 8, 2023 at 7:39 pmpeteroznewmanSubscriber
An axisymmetric model is constructed on the XY plane where X is the radial direction and Y is the axis of rotation. That is the definition used in all the equations built into the elements that solve for the stress. The Y axis is axial by definition.
April 9, 2023 at 9:02 amGokizaSubscriber
Hello sir, Which stress results(normal stress or equivalent) gives us more logical results in Axisymmetric and Plane stress? And why? because I want to understand very clearly. Many many thanks from now.
April 12, 2023 at 3:09 pmGokizaSubscriber
Hello sir, Which is more true to calculate(hoop direction or tangential direction)in plane stress method? If our structure has small thickness like above (interlocking rings).
April 12, 2023 at 6:25 pmpeteroznewmanSubscriber
A hoop direction applies to axisymmetric models and is the Global Z axis and represents the tangential direction around a circular object that is being viewed in a radial slice. In Axisymmetric models, circular objects are implied by rotation about the Global Y axis.
In Plane Stress, you are not required to have any circular objects. If you draw a circular object in the XY plane, you can put a Cylindrical Coordinate Sytem at the center of the circle. Make sure the Z axis point out of the plane. Now the X axis is Radial and the Y axis of the local cylindrical coordinate system is tangential to the circle.
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
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.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- User manual
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- material damping and modal analysis
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.