Learning Forum

[pv00170]

I am modelling a bridge structure in which the deck is connected to the piers through elastomeric bearings.

I have modelled the bridge deck as solid. As I am not modelling a 3D of the elastomeric bearings, I have modelled the upper and lower part of the bearings as as surfaces with 0.001 m of thickness. The upper part is embedded with the deck and the lower with the pier.

I have connected both surface (up and down) by bushing connections. In which the lower part is the reference, and the upper part is the mobile. Additionally, I assume the lower parts (pier) as fixed.

Elastomeric bearings are elastic systems which gives freedom of movement and rotation. Elastomeric properties are given by stiffness and rotation in each direction and axis.

Question 0: Is this a good approach?

Question 1: Should I put the reference coordinate system the Reference face gravity centre?

Question 2: What is the difference between MPC or Bushing formulation? Whenever I use Bushing formulation, I get an error saying: “The current analysis is not supported with joint defined with bushing formulation.”.

Question 3: Once I run the simulation, I get results with the following warning. The solution to this problem is only to use a better computer?

- During this solution, the elapsed time exceeded the CPU time by an excessive margin.  Often this indicates either a lack of physical memory (RAM) required to efficiently handle this simulation or it indicates a particularly slow hard drive configuration.  This simulation can be expected to run faster on identical hardware if additional RAM or a faster hard drive configuration is made available.  For more details, please see the Ansys Performance Guide which is part of the Ansys Help system.

Question 4: If the material used is concrete, should I use stiffness behaviour Rigid? And if it is structural steel, Flexible?

 

[peteroznewman]

1. What is the purpose of the simulation? What is the output you want? The answers to these questions determine the answer to this question.
2. Please read the Ansys Help on a Joint Type Bushing for answers to your questions. 
   https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v231/en/wb_sim/ds_Joints_types_bushing.html
3. You can ignore this warning if you are satisfied with the time it took to solve, or you can’t afford to upgrade your computer hardware. If you can afford to upgrade your computer hardware you can install more RAM up to the maximum supported by that computer and/or you can install an SSD if you currently have a HDD because the access time on an SSD is much lower than a HDD.
4. There is a lot less computation when you make solid bodies rigid instead of flexible. Since the elastomer is orders of magnitude less stiff than concrete or steel, you could make a first model where they are both rigid. The warning in question 3 might go away. After you get some results, you can change the steel to flexible and get some new results. Then you can change the concrete to flexible and get some final results. 

[pv00170]

1. The purpose is to see the reaction of the bridge structure under external pressures. Therefore, I am focused on deformation, stresses, and strains in the structure, not only in the bearing systems.
   • Also, I wanted to extract shear forces and bending moments of the girders (beams). But I have modelled them as 3D solids not Beam lines. Is there anyway to extract these values for 3D solids?
2. Okay!
3. Okay!
4.  (Please correct me) As far as I understand, Rigid imply that no deformation, stresses, and strains in these bodies are expected, and therefore not computed. Is this right? Is that why Rigid bodies are not meshed?
   • On the other hand, external pressures are imported on the bridge surfaces and if there’s no mesh (Rigid) then the solver does not have any node into which attach the pressures. Is there any way to import pressures to Rigid bodies if there’s no mesh?

[peteroznewman]

Yes, rigid means no deformation, stress or strain. Rigid bodies are able to transfer forces from one place to another. Most loads and boundary conditions including contact can be applied to a rigid body in the same way as can be applied to a flexible body, but not every single thing. In older versions, you needed to substitue a Fixed Joint for a Fixed Support. Another example is with contact between two flexible bodies, you are free to flip the Target and Contact side of the contact definition, but when one side of the pair is rigid, that side must be the Target side. The mesher will automatically create surface elements on the Target faces to pickup the contact forces to apply to the rigid body and transfer to another part of the rigid body.

I don’t know if imported pressures are supported on a rigid body. If they are, then surface nodes and elements will automatically be created. If they aren’t then you have to make that body flexible.

Given your purpose, you could start with the concrete parts such as the pier etc as rigid bodies and leave the steel parts as flexible bodies. If you need stress and strain in the concrete parts, you could change them back to flexible after you solve for the steel parts.

I will caution you that meshing thin walled structures such as the bridge girder with 3D solid elements has some requirements on the number of elements through the thickness. Where the plate experiences bending stress, there should be a minimum of 4 linear or 2 quadratic elements through the thickness to get accurate stress output. The default element order is quadratic, but you should set that manually and not leave it program controlled.

On the girder, it would be more efficient in terms of solution time to have shell elements instead of solid elements. That means going back to geometry and using the Midsurface feature to extract a surface to mesh with shell elements. The benefit of shell elements is that internally it can calculate stress at 5 or more points through the thickness so the accuracy of stress is high even with a fairly coarse mesh. This would also make the solution compute in much less time.

One compromise is to use the SOLSH190 element, which is specially formulated to be more accurate with bending stresses when there is only 1 layer of elements through the thickness. The difficulty of using that element is that you must ensure that the body can be meshed using a sweep mesh control because the element has a through-thickness direction which must be correctly oriented for it to work properly. A solid element has no such thing.

One more way to have the best of both worlds is in geometry, place a cutting plane one road-width away from the bearings along the axis of the span. Split the solid geometry using that plane. Convert to midsurface the girder between the pier where it is very easy to use midsurfacing. Leave as solid the complex geometry near the bearings. Use Bonded Contact to connect the edges of the midsurface to the cut face of the solids on the bearing side of the cutting plane.

[pv00170]

Hi Peter, I will use 3D solids for the thin steel girders in the end. How can I tell the meshing program to do minimum four layers of meshing between two faces?

[pv00170]

I will use only Flexible as I am interested in deformations, stresses, and strains in all solids.

I am analysing two different bridge girders (concrete and steel):

• Concrete which have thick girders (the image shows a cross-section) (vertical elements are not piers, are girders (beams)).
• Steel which have thin cross sections

In order to use shell elements, should I use them in both typologies or only in the steel one as I am dealing with thin elements?

[peteroznewman]

For the steel girders, you have two options.

Beam Elements

SpaceClaim, on the Prepare tab, has an ability to convert a solid shape that is a clean extruded shape, into a beam element, which looks like a line but has the cross-sectional properties of the solid.  The advantage of using Beam elements is you can output Bending Moments and Shear Forces very easily from the analysis. However, there is just a row of nodes along the neutral axis of the beam so the deck connection has to reach down to that row of nodes using a joint.

Shell Elements

SpaceClaim has a Midsurface Tool on the Prepare tab. Shell elements allow you to connect to nodes on the top flange or bottom flange. Now there are girder nodes next to the deck nodes to make a connection, but it is more complicated to extract bending moments and shear forces.

Keep the concrete girders as solid elements.

[pv00170]

Is there any way to extract bending moments and shear forces of the concrete girders if those are modelled as solid elements?

 

[peteroznewman]

Yes.

Under Geometry, you have to create a Coordinate System and Construction Surface to cut through the elements. 

Under Analysis Settings, in the Output Controls section, you have to turn on Nodal Forces.

Insert a Probe for the Force Reaction scoped to the construction surface and coordinate system to measure the shear forces created by the elements on one side of the plane. Insert a Probe for Moment Reaction for bending moment.  Repeat with as many planes and probes as you want along the length of the girder.

When you use a Beam element and insert a Bending Moment result or a Shear Force result, you get a graph along the length of the beam.

 

 

[pv00170]

Hi Peter,

I have tried the Shell elements on the steel girders.

Now, I am importing pressures on the girders' surfaces. There are presures on both sides of each girder, but if I transform the solid to a Shell element, it detects the Shell elements as a single surface, and therefore only pressures of one side of the 3D solid are transfered.

In the following image only Girders (1 to 4) are shown. Depending on how Shells are created, upstream or downstream pressures of the solid are therefore transmitted to the shell, ignoring the other side.

 

 

Is there anyway to transfer the pressures on both sides?

[peteroznewman]

It's interesting that you import pressure on one side or the other of the shell elements.  The correct load is the pressure difference applied to the shell elements.

[pv00170]

Is there any way to compute this pressure difference directly in fluent? (I know how to get the drag force, but pressures)?

 

Also, is there any way to extract the results of Force and Moment Reactions as .csv or any other format?

As I have multiple surfaces, I need to go one by one and check the results in X, Y and Z for each of them, so I thought to extract the results of all surfaces directly.

 

[pv00170]

.