How to model a beam on elastic foundation?
I am trying to model a simplysupported beam on elastic foundation, kind of like the figure below:
So far, I have not been able to properly model the elastic foundation. I know that Ansys has an "Elastic Support" feature for 2D and 3D structures [N/m³]. However, I need it to be applied along the beam, that is, at an edge [N/m²]. I can think of two possible solutions (which I could not successfully apply yet):
1) To model an elastic support at an edge, so that Ansys will automatically distribute the stiffness at nodes. This is the best option, as I would not need to manually adjust the stiffness factor according to the mesh density.
2) To define springs (or bushing joints), one by one, at each node. This solution is inconvenient, since it would require me to individually define hundreds of "Named Selections" and "Connections", and to adjust the stiffness factor for each connection.
That being said, my question is: is there any way to define an Elastic Support along an edge? If not, is there any way to efficiently define connections at a number of nodes (for example, using command lines or editing Ansys' data files)?
In case it helps, my Ansys file is below:
Best Answers

peteroznewman Member
Please review the attached ANSYS 2020 R1 archive that shows a 2D Plane Strain model of a 0.5 mm thick aluminum sheet on an elastic foundation.

peteroznewman Member
1) Most FE software, including ANSYS, offers two kinds of 2D Planar models: Plane Stress and Plane Strain.
Plane Stress is for modeling thin objects and you get to define the thickness of the object. The Z component of stress is zero. If you double the thickness of the model, the part gets twice as stiff in the plane.
Plane Strain is for modeling infinitely thick objects. The Z component of strain is zero. The loads are infinitely deep in the Z direction, so it only makes sense to describe loads/unit depth. So if you are in the units of meters, then the loads are N/m of depth. You can't change the thickness of the part because it is infinite.
2) ANSYS writes out a text file that you could edit with Notepad if you wanted. But Mechanical includes the Object Generator. With a few clicks, you can select 100 entities on the Mobile side of the spring and another 100 entities for the Reference side of a spring as two Named Selections. Create a single spring between the first entity on each side. Then use the Object Generator to automatically make 99 more. I have a tutorial in the link below.
Answers
Please review the attached ANSYS 2020 R1 archive that shows a 2D Plane Strain model of a 0.5 mm thick aluminum sheet on an elastic foundation.
Your solution works for me, thank you. Anyway, let me ask you two more questions:
1) In other FE softwares, we can modify the surface's standard thickness (in Z direction). However, in Mechanical APDL I could not find such an option anywhere. In SpaceClaim, I did find it, but it does not affect the final results at all. Since the results provided by Ansys' 2D Plane Strain model match with a beam with crosssection 0.5 x 1000 mm, I suppose the standard thickness is 1 m. Can I change that?
2) Although your solution is very suitable for my particular objetive (which was to validate the analytical model of a beam on elastic support), I am still curious to know how can one efficiently define a large amount of instances (e.g.: loads, springs, concentrated masses etc). In other FE softwares, one can simply open the source file using, for example, Nodepad, and then manually write command lines to define such a large number of instances. What about in Ansys? How could I, let us say, define 100 springs, one for each node?
1) Most FE software, including ANSYS, offers two kinds of 2D Planar models: Plane Stress and Plane Strain.
Plane Stress is for modeling thin objects and you get to define the thickness of the object. The Z component of stress is zero. If you double the thickness of the model, the part gets twice as stiff in the plane.
Plane Strain is for modeling infinitely thick objects. The Z component of strain is zero. The loads are infinitely deep in the Z direction, so it only makes sense to describe loads/unit depth. So if you are in the units of meters, then the loads are N/m of depth. You can't change the thickness of the part because it is infinite.
2) ANSYS writes out a text file that you could edit with Notepad if you wanted. But Mechanical includes the Object Generator. With a few clicks, you can select 100 entities on the Mobile side of the spring and another 100 entities for the Reference side of a spring as two Named Selections. Create a single spring between the first entity on each side. Then use the Object Generator to automatically make 99 more. I have a tutorial in the link below.
https://forum.ansys.com/discussion/2513/usingthemechanicalobjectgeneratortosavetimeonrepetitivetasks
Thank you, that was exactly what I needed. As other users might have the same doubt in the future, I am here attaching a file with the modal analysis of three analogous models:
1) A 2D surface under plane stress;
2) A beam on elastic foundation (modelled with a set of springs);
3) And a cylindrical shell (axisymmetric modes, analogous to the previous models via Timoshenko's analogy between beams on elastic foundation and cylindrical shells subjected to axisymmetric loads).
You can model the edge beam with Shell 63.