November 12, 2019 at 10:50 pmJoeySubscriber
I am new to Ansys. Apologies if the questions are repeated. If so, Please link me to similar posts.
I am trying to simulate eccentric axial loading on a hollow beam of circular cross section. I have Large Deflection as on. I have numbered and put the questions in bold throughout my post.
The dimensions of my beam are as follows:
Inner radius: 0.3 mm
Outer radius: 0.4 mm
Length: 35 mm
Basically, it is a thin cable. For now, I have kept the material as steel. I intend to use superelastic material properties eventually.
I have meshed the part with the parameters as shown. I just followed an online example (I have no clue as to which Physics Preference and Solver Preference to use, but Mechanical gave me a very non-uniform mesh).
1) Is there a proper manual/documentation as to what meshing is to be used for which situation? How do I get a uniform mesh which is axisymmetric?
I applied fixed support on one face of the beam. On the other face, I want to apply a force as shown below:
However, when I choose Static Structural>Loads>Force and select a point on the face, I select the whole face:
I know that I can choose to insert a remote point and apply a remote force, or choose a point of application using Element Node selection.
2) If I define a remote point, and a remote force on it, does it continue to apply as the beam deforms? As in, does the remote point move along with the beam as it deforms so the force continues to apply at the point?
(I believe the above is true, because the beam does deform quite a bit, so my intuition says that obviously the force applies throughout the deformation process)
3) How can I apply my eccentric axial force over a local area on that face of the beam? Say, over a circular area between the inner and outer radii, on the rim.
4) If I apply my force and define it either by Vector or Components, does it remain perpendicular to the surface as the beam deforms? Or do I need to use pressure in this case? If the latter is true, then what is the answer for (3)?
I know that my beam deforms quite a bit (hence large deflection) and that my load should always remain perpendicular to the surface of the face of the beam, at the same point/location.
Please let me know if I need to give more details. Thanks
November 13, 2019 at 1:11 ampeteroznewmanSubscriber
(1) To get a uniform mesh, apply a Mesh Method of Sweep to the pipe solid and apply Face Meshing to the end face and set the number of divisions to a minimum of 2.
(2) A remote point with a remote force will continue to apply that force as the part deforms. The point will move with the end face that it is scoped to, and the sideways deformation will add to the eccentricity. The direction of the force will not follow any tilting of the end face, it will remain aligned with the coordinate direction it was initially defined with.
(3) Do you mean a circle with a diameter of < 0.1 mm at some location on the end face? You would go into the geometry editor and draw that circle on that end face. That however would ruin the mesh created in (1).
(4) You need a Pressure to have the force remain perpendicular to the end face as it deflects.
November 14, 2019 at 7:03 pmJoeySubscriber
(1) I am unable to see where to select/apply different mesh methods in the Mesh window. Where is it available?
(3) Yes, I do mean a circle with diameter <0.1 mm. Could you explain why an external feature would affect the mesh created?
I also have some more questions:
I have to apply to eccentric load not at the face but somewhere in between. Since I need to load to always be perpendicular to the cross section at that point, I am going ahead with using pressure. As I need a surface, I have made a small cut in my geometry as shown:
(5) Selecting the face over which I want my load gives me the area, so I can just use that to find the equivalent pressure I have to give, right? Is this approach valid?
(6) Will this also affect my mesh to be non uniform? If I want more fine meshing around this cut, should I just enable Adaptive Meshing? (Mesh>Sizing>Use Adaptive Sizing>Yes)
November 15, 2019 at 12:37 ampeteroznewmanSubscriber
(1) Now that you have made a cut in the solid, it is no longer sweepable geometry, so the mesh method of sweep no longer applies. Before you did that, you would pick the solid and right mouse click to get the list of mesh controls, and Method is on the list. The type of method is sweep. If you drew a circle on the end face, then the body would stop being sweepable because there would not be a matching circle on the opposite end.
(6) Don't use Adaptive Meshing just yet. If you are applying a load to that face in a cutout, it seems like the pipe above that cutout has no load. It would be better to cut it off and not include it in the analysis. You could just have an end face with two lines to create the same area. If you did the same at the opposite end, then the body remains sweepable.
November 15, 2019 at 10:39 pmJoeySubscriber
I was able to use sweep method for a simple tubular beam. However, without changing any parameters, the meshing is as shown:
(1) How do I get those element edges to be axisymmetric? I applied Face meshing to one end face, and set the number of divisions as 2, as you said, the meshing failed:
When I selected both faces, then the option for number of divisions does not appear:
(In the above case, I also added the lines while constructing geometry to demarcate the area for applying my pressure, I did the same on the opposite face as you said. I Ctrl+Selected the four faces and applied Face meshing)
What can I do to resolve this?
(6) When I draw the lines on the face, do they have to be axisymmetric? I just drew two vertical lines on both faces as shown:
Kindly let me know how I may resolve the above.
If possible, kindly direct me to a manual that I may refer to for meshing as a whole.
November 16, 2019 at 3:47 ampeteroznewmanSubscriber
Face Meshing applied to the end face with the number of divisions to a minimum of 2 was the advice when there was a single face on the end with no line breaking it up into 2 faces. There were only 2 edges and so the Internal divisions could only apply between the inner and the outer edge.
Once you split the face into two pieces as shown in the last image, each face has 4 edges. Use Face Meshing, but don't specify Number of Divisions. Instead, add two Sizing mesh controls. Pick the two short edges that connect the inner and outer diameter and set those to have a Number of Divisions to be 2 or 3. Pick the four circular edges and set the element size to an appropriate value. Then you will get a good mesh on the end face.
The two short edges don't have to be radial, they can be parallel.
November 22, 2019 at 12:29 amJoeySubscriber
I applies the the mesh as I understood from your instructions:
I applied face meshing on each of the partitions, on both faces:
I applied two sizing controls, one on the lines from outer to inner diameters, on both faces (so total 4 lines), with number of divisions as 2:
and another on the four curved edges on both faces (total 8 edges), with element sizes 0.1 mm, 0.01 mm and 0.05 mm each time:
I then applied sweep method mesh to the whole part:
And I'm still getting an error that the mesh fails. I tried applying all of the above (except sweep) on a single face too, and it still failed. Is there something I misunderstood from your instructions, or that I haven't considered?
November 22, 2019 at 12:53 ampeteroznewmanSubscriber
File, Archive and save a .wbpz file. Attach that file to your reply and say what version of ANSYS you are using.
November 22, 2019 at 8:16 pmJoeySubscriber
Ansys Workbench Version 19.1
November 22, 2019 at 10:39 pmpeteroznewmanSubscriber
Go back to SpaceClaim, you can use Repair to get rid of the two lines at each end.
Create a Plane through the center and Move it off to one side and then repeat. Use Split Body to Cut the pipe using the planes. Use Combine to unite the three parts back together to end up with two solids.
Use the Workbench tab to Share. The shared lines will turn purple. Close SpaceClaim.
In Mechanical, Use the Sweep Method on just the large solid. Pick the end face as the Source of the Sweep. You can use your edge sizing on all the circular edges at the source end and the other edge sizing for 2 elements through the thickness.
- 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.