HelpDesk
sign in

Simply supported bridge boundaries

Creation date: 7/26/2020 6:16 PM    Updated: 8/1/2020 7:20 AM
Print...
Question:

Hello,

I have modeled a simply supported bridge with precast beams and applied the boundary conditions I have found in this forum for this purpose. When I run the analysis and check the moments, I get bending moments in one of the supports. Could you please help with this? I attach the model.

Thank you  
Answer:

Hello, 

Thanks for getting in touch.
The moment at the supports appears because of two reasons :-

1) Section Offset
The offset provided is Centre-Top for the sections.
Check out in the image below, how the Moment reduces at Element No. 2 at I-end (Support node) when Offset is changed from Centre-Top to Centre-Centre for all the sections in the model.


To understand how the offset creates moments at the supports, kindly refer to the link below.

click on details for Section Offset in the above link


However, since the loads actually act at the top of the beams and not at center, our suggestion would be to continue with the Centre-Top offset.

 2) Presence of DIAPHRAGM (cross-beam) elements because of which the support nodes act like Continuous Supports creating moments at supports.



Kindly let us know if further assistance is required.

Regards,
Rohan Agarwal
Technical Support Engineer

Click here to give FEEDBACK


Hello,

Thank you for your message. I understand the concept but I am still getting strange displacement warnings when I run the analysis which I am not sure if they are due to the supports or due to a wrong input in the construction stages. My bridge will be supported on bearings and it looks like the supports are at the nodes which are offset at the top of the slab. I am not sure if this is right. 

Could you please let me know the reason of this warnings? I would appreciate if you can also help me with the construction stage input as I don´t really understand how to input the activation of my composite beams, the prestress, the age, etc

Find attached the model

Thank you in advance


Hello, 

Yes the errors are due to erroneous boundary conditions for construction stage analysis. 
Let me give an example,

The above image is for stage 1. Here, in this stage all the girders are independent and not joined together to provide stability by an cross-beams (something which we do in stage 2) . So the software would check the independent stability for each girder. 

Now if we pick any girder in stage 1, we see that for each girder, atleast for one direction no support condition is provided. So each girder would be unstable.

The solution lies in providing temporary supports for Stage 1 (which could be pinned supports everywhere or depending upon what would be actually carried out on site) and then replacing them with permanent support at a later stage. 

*My bridge will be supported on bearings and it looks like the supports are at the nodes which are offset at the top of the slab.
Yes, this is correct.

Kindly check out the link below for PSC Composite bridges. 

Some tutorials are attached for reference. One tutorial is using our PSC Composite Wizard.
Also, the tutorial may not necessarily be using Eurocode but the concept is the same.

Regards,
Rohan Agarwal
Technical Support Engineer

Click here to give FEEDBACK


Hello again, 

Thank you for your response. I am trying to model the boundary conditions as per the tutorials and I have a couple of questions that you may be able to answer:
- First, Could I assign the same nodes for temporary and for permanent supports? 
- I have modeled the rigid links and rigid elastic links for an assumed bearing thickness of 15mm. Do I need to model the elastic links to simulate the bearings or can I just assign the supports to the bottom nodes without the elastic links? Will I get the reactions at these supports for the bearing calculation? 
- When modelling the boundary conditions as per the tutorial, I am getting an error message when analyzing the structure that says: Boundary condition has not been defined. Any thoughts of what might be the reason?


Hello, 

 1) First, Could I assign the same nodes for temporary and for permanent supports? 

Yes, though assign them in different boundary groups and then activate and deactivate accordingly

2)  I have modeled the rigid links and rigid elastic links for an assumed bearing thickness of 15mm. Do I need to model the elastic links to simulate the bearings or can I just assign the supports to the bottom nodes without the elastic links? Will I get the reactions at these supports for the bearing calculation? 

A bearing has a finite stiffness in some direction depending upon the type of bearing it is. So, to simulate the bearings it is suggested to use elastic links through which the stiffness value as desired could be entered. 
Reactions would always be obtained at the supports in the form of Fx,Fy,Fz.
To get the bearing force, we need to check out the forces in the elastic links using Results -> Results Table -> Elastic Links.

-3) When modelling the boundary conditions as per the tutorial, I am getting an error message when analyzing the structure that says: Boundary condition has not been defined. Any thoughts of what might be the reason?

In stage 1, only Rigid Links have been provided.

A rigid link connects the two nodes rigidly such that it behaves as one. That is, there would be no relative deformation between the two nodes.
But how about the stability of the model. The model is still unstable as no Supports are provided at the bottom nodes.

These supports as shown below has to be activated in the Stage 1 to provide stability to the model.

Regards,
Rohan Agarwal
Technical Support Engineer

Click here to give FEEDBACK
DataImage59.png
DataImage50.png
DataImage45.jpg
DataImage72.png
DataImage11.png
OSD REV0[1].mcb
DataImage12.png
2 Span PSC Composite Bridge.pdf
2-Span_PSC_Composite_Girder_Final.pdf
OSD REV0.mcb
OSD REV0 without construction stages.mcb
Files
Sort by Name Sort by Date
Get help for this page