September 15, 2018 at 10:41 amaakib.voraSubscriberSir I am having a "round cross section beam" which is simply supported (i.e fixed support at one end and displacement at other end ) having force at the center ( at mid point ) on top surface of the round 3d beam.
So my question is that how to apply this constraints of fixed support and displacement (i.e either on surface or edge or point) for simply supported beam. And how to apply force at the "mid point" of the outer surface of round beam.
I'm using ansys aim 18.1
September 16, 2018 at 2:48 pmSandeep MedikondaAnsys Employee
Please go through the tutorials, I previously provided.
I will explain it here:
First, All you would have to do to create a fixed support is to right click on the face and select this condition:
Then do the same for displacement at the other end and enter the values:
Lastly, select the 2 vertices of the circles and insert a force as shown in the middle:
This will result in the following results:
Hope this helps.
September 17, 2018 at 5:27 pmaakib.voraSubscriberSir thanks for the explanation But I'm still in a doubt, i.e as in the case of "square" cross section simply supported beam, we apply fixed support to the "edge" of rectangular beam and displacement to "edge" at the other end of the beam ( by setting the respective axis to free and constant).
Similarly, if we consider the case of simply supported beam with round cross section, where we have to apply the fixed support and displacement i.e either on edge or point of circular cross section.
Because, as shown by you sir if we apply the fixed support to the surface of round cross section it will lead to the case of cantiliver beam.
I'm using ansys aim 18.1
September 17, 2018 at 6:09 pm
September 20, 2018 at 8:54 amaakib.voraSubscriber
- Thank u sir for the response, so sir as shown by you that edge has to be chosen, sir but I am having different options here.
Thus sir Just make me to know that which option has to be chosen ( from the image shown) for fixed support and roller support in round cross section "simply supported beam"?
Also, for this support "where" I have to apply it either on edge/surface/vertice for fixed support and roller support?
(Here the image shows the front view of a round simply supported beam with a fixed support on one end and roller support at another )
I really appreciate you sir, for responding to every post.
September 20, 2018 at 6:04 pmpeteroznewmanSubscriber
Here is a sketch of a simply supported beam, with a pinned end and a roller end.
This is very different from a fixed end and a roller end.
With a center load, the shape of the deformation for a fixed-roller is very different to a pinned-roller beam. Do you see that the tangent to the beam at the left end has a zero angle, while for the pinned-roller case, there is a non-zero tangent angle on the left end of the beam.
What end conditions do you really want on your beam: Fixed or Pinned (simply supported)?
I think you want a Pinned left end, even though you are saying Fixed.
September 20, 2018 at 6:33 pmaakib.voraSubscriber
Yes sir, my question is for a "pinned end and a roller end". ( Simply supported beam with round cross section )
(Sorry for saying as fixed support I thought both are same)
Having a force at the top surface at a point.
Having options of boundary conditions as like this in image.
So sir let me know that where to apply the boundary conditions either on point edge or surface ? (For pinned end and roller end)
I'm using ansys 18.1
September 20, 2018 at 8:46 pmSandeep MedikondaAnsys Employee
I thought you said you were doing this in AIM 18.1?
September 20, 2018 at 8:58 pmpeteroznewmanSubscriber
In AIM, the interface is simplified, so to get a pinned end on a solid beam, you open the Geometry and draw a line across the end to form an edge on a face. You also put a plane in the center and Split the face so you get an edge in the center to apply the Force.
There is a line at both end faces.
Then in Physics, you Add a Structural condition, and add a Fixed Support at one end but you pick the Edge not the Face. A face can rotate around a fixed edge, but a fixed face can't rotate at all.
Then you Add a second Structural condition, it is the User specified Support, and you Fix the Edge in Y only, and leave X and Z free.
September 21, 2018 at 7:43 amaakib.voraSubscriber
sir thanks for the explanation, but as seen in figure the support are at bottom side, and as shown by you we are applying boundary condition at the central edges.
Are both the cases same??
Also, if we applied the contrain at the circular edge (as seen in figure) which condition this shows.
Or, if we apply the constrain at the bottom semicircle does it give correct solution?
September 21, 2018 at 11:02 ampeteroznewmanSubscriber
FEA models are idealizations of physical systems. For beam bending problems, the freedom of the end of the beam is what is important. On a solid model, a fixed straight edge provides a pinned connection to ground. If you hold the circular edge fixed, that is the same as holding the face fixed and you no longer have a pinned end, you have a fixed end and a very different displacement solution.
If you leave AIM and use Mechanical, you have more tools available such as Remote Displacement. With remote displacement, a point is created at the center of the face, connected to the face, and you specify how you want to hold the point. You can hold three translations, and it becomes a spherical joint, You can hold one translation and it becomes a roller support, you would hold three translations and two rotations and it becomes a pinned connection to ground. The point can be located a the center of the face.
Don't worry about whether the support is located at the bottom of the rod or the center of the rod, the deformation and stress are going to be identical for the small deflections of a beam.
September 21, 2018 at 6:43 pmaakib.voraSubscriberSir can you pls. Show (through images) how this "remote displacement" is used for having pinned support and roller support in round Cross section simply supported beam.
September 22, 2018 at 2:41 ampeteroznewmanSubscriber
Open ANSYS Workbench 19.1, drag a Static Structural onto the Project page, double click on Geometry and draw the rod and divide the face at the center, then double click on Model to start Mechanical. You will see this:
Now create the Roller support on one end by picking Remote Displacement.
Pick the face and assign a 0 Y displacement.
Now apply a Remote Displacement to the other end and 0 everything by the Rotation about Z, that is a Pinned end.
Now apply the force.
Solve and create a Deformation and Normal Stress plots.
September 23, 2018 at 9:32 amaakib.voraSubscriber
Sir instead If I apply constraints of "fixed support" and "displacement" to the two lower "half semicircle"( as shown). Is I'm doing right ? for simply supported beam ( having pinned at one end and roller at other).
What is the problem if I apply constrains to the bottom two points? ( Or their any way to get the same result by using point and semicircle selections).
September 23, 2018 at 12:02 pmpeteroznewmanSubscriber
Making a pinned connection to ground is like making a hinge for a door.
When I drew a straight line across the face, that made a pinned connection that could pivot because it was a straight line. When each node along that straight line has a fixed support, that prevents translation, that doesn't prevent the face from rotating about the line. Now consider the case of the half circle. The nodes at the start and end are in the same position as they were for the straight line, so could make a pinned connection if you only did those two points. But as soon as you add nodes around the rest of the semi-circle, those nodes are not allowed to move, so you just turned it into a fixed support and not a pinned connection.
One point on the bottom is fine for the roller constraint. One point on the bottom is insufficient for the pinned connection. A single point doesn't create a hinge axis. You need two points to do that, and not any two points, but two points spaced in the Z axis at the same Y coordinate, if you are applying a Y force in the center. If you use one point on the roller end, what is wrong with one point for the pinned end is it leaves the rod free to spin around the line connecting the two points. FEA solvers can't solve a Statics problem when a body is free to spin with no resistance.
- You must be logged in to reply to this topic.
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.
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- How to calculate the residual stress on a coating by Vickers indentation?
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
© 2023 Copyright ANSYS, Inc. All rights reserved.