SUSPENSION BRIDGE PROBLEM!

[Anonymous]

Hi guys,

Any thoughts on the best way to model a suspension bridge? I'am really struggeling with a digital model of suspension bridge built in norway in 1954, for a school-assignment. I am struggeling with the connections with the beams, deck and cables.  I've had a quick try but seem to be coming unstuck. 

It seems to me that this sort of model is actually not really possible, and maybe I should be looking at other options? Can somebody help me with the model?

Simon

[Artur.Kosakowski]

Hi @Anonymous

The deck has to be defined at the level of the beams. Mind that panels have got no real thickness and beam no real sizes and are just flat surfaces and lines with corresponding properties being their attributes only.

In addition as cables cannot transfer bending you shouldn't apply releases to them.

I corrected the model and set the large displacement analysis type - all load cases and combinations converge to the reasonable (at the first glance) results. see the attached model.

If I managed to answer your question(s) press the Accept as Solution button please. This will help other users to find solution(s) much faster. Thank you.

[Rafacascudo]

  I have never done a suspension bridge , but I suspect , You cannot do it perfecly using RSA . There´s something called " Form finding" which is an iterative

method to find the forces for the initial configuration of all cables , mainly to withstand bridge´s dead weight, keeping it´s idealized shape/geometry.

https://biblio.ugent.be/publication/8521629/file/8521631.pdf

If you manage to do that using Robot or another method/software outside Robot , then maybe it will be feasable using RSA.

[Anonymous]

Hi Rafascudo,

I am curious.... 

just and idea, what you think about phase option.

Model is nonlinear and principle of superposition it is not valid.

Then just for each phase we can check all regarding limit states (deformability and ultimate).

In Robot Structural Analysis 2018 Help: Non-linear Static Analysis

Large displacements analysis

This analysis considers third-order effects, such as the additional lateral rigidity and stresses resulting from deformation or rotation. This effect considers additional forces arising in a deformed structure such as a beam with fixed supports on both ends, loaded by a vertical load, longitudinal forces arise and the deflection decreases.

Large displacements option is actually form finding solution- for that phase.

Or even for each model, if we have several cables.

Regards

[Rafacascudo]

Could work.

I never studied this method (form finding) that is used in almost all tensile structures like suspension bridges and membrane shells.

Maybe someone who has already done a suspension bridge ( @alfredmx  ???) can give us some tips on how to do it on a non dedicated bridge program like Robot.

For sure some dedicated programs can do it automatically.

[Simau]

Hi @Anonymous

Never studied a suspension bridge.

But here some comments, after looking at

[Simau]

Try a UX UZ free support

[alfredmx]

Hello friends,

I’ve never participated in a suspension bridge project. However, in cable stayed bridges, you need to find influence matrix of structure (related to stays) in order to find forces that will give you desired profile and stresses in beams (usually as if deck was a continuous beam over elastic supports). You can do it in Robot, but it takes some work. Basically you have to find a matrix that tells you how structure responds when you pull certain pair of stays. Then by imposing certain constrains to such matrix, you solve the system of equations that will give you required stay forces. Finally with backward analysis according to defined construction stages, you will find pull forces for all stays at each stage. Some specialized bridge software offer you this “form finding” algorithms. Regarding non-linearity of stays, it is easier to make them “linear” by using methods such as Podolny equivalent stiffness. Some software use this approach. Please mind that Robot phases is very limited and not suitable for this type of analysis. You would have to do staged analysis outside Robot.

Regards,

[Anonymous]

Hi aflredmx,

I didn't have chance to design cable stayed bridges or roof structures but I am expecting to do it in future.....

Ok, for structures with many cables we can not provide phases in Robot. Also, most important Robot can not model in case of several phases, for each phase its final deformed configuration as initial in next phase (as it is possible I think in SAP 2000....).   

Generally, in this type of cable stay structures material non-linearity is not highlighted, only geometrical non-linearity (cables are tensile structures, with no flexural stiffness). Robot have large displacement implemented theory implemented and works fine, which means that equations of system in the current phase (only one phase, because doesn't support more phases in this case) are based on modified geometry using incremental-iterative procedure of solution (geometrical nonlinearity -known as Lagrange theory, solution of equation and convergence using -Newton Raphson method...).

So I wondering for just this type of structure as it is in this post, could we use Robot to calculate the forces in cables and provide code checking. 

By my opinion in this example is just one phase. If Robot can calculate this type of structure with adequate safety that is OK...)

And this topic is very important for future Robot development, hope this will be implemented in next versions. 

Regards

[Anonymous]

Hi @Artur.Kosakowski!

Thank you for your answer and for correcting my file. I've adden some other loads and tried to correct the structure so that the supports are right, but i keep getting errors and warnings about "instability in the nodes along the main cable and "no convergens of nonlinear problem". How do i solve this?

best regards

Simon

[Anonymous]

Hi @Anonymous!

Do you have any experience  with SAP2000? And is it possible to convert a ROBOT-file til SAP format? at least the geometry?

best regards

Simon

[Anonymous]

Hi Simenp,

Sorry, I don't have experience with SAP2000. But, I still think you can model it in Robot.

The only problem is probably initial geometry of structure if you hvae several cable, but in your case there are only two of them and they are constructing in the same time,

I am just thinking, perhaps in your model can calculate just for characteristic combinations as it is for self weight of structure+prestressing force in cables (I assume you are planning to prestress them) , and 2. combinations self weigth+prestressing +live load.

Looses of prestressing force can took aproximate in all combinations.

Then compare deformations and forces in cables.

What you think about that?

Regards

[alfredmx]

Hello rm-rsa,

I’m assuming that in suspension bridges at some point you would also need to find pull force in main cable to achieve desire profile under working loads. Since structure by nature is highly non-linear, you would definitely have to use cable elements. As far as I know, structure can be studied using Robot considering “assembly case” including all acting loads. However, I’m not sure how to correctly simulate pull force in main cable (not sure if you apply elongation only to back spans or all main cables segments). Also, since main cable goes from one side to the other, above top supports you would expect to see behavior similar to a pulley. Don’t know if releasing longitudinal displacement on top supports is the correct way to model such behavior. Maybe Artur/Rafal/Pawel can give some suggestions.

Regards,

[Anonymous]

Hi alfredmx,

I agree with you. How to model top support is good question ?  There we have longitudinal force from cable which can in each case be divided into two components, vertical and horizontal. If we consider FEM node compatibility, then in that node we probably need to use something as rigid links and release horizontal displacement. Vertical downward force have to go into column……

Definitely, question for Robot Artur/Rafal/Pawel/Rafascudo …..

There are programs that are specialized for this, but I have a robot and I hope that together we can find a way to calculate this…. I was thinking about the phases and also agreed with you. What you think to simplify the calculation and do next:

Phase 1 (assembly case) – MODEL 1 – cables + self weight. In this phase we need to manually vary prestressing force (or stress which produce force, probably elongation is impossible to define) in cable as long as the first stage does not satisfy serviceability and ultimate limit state. This is iterative procedure and it takes some time.

Phase 2 (final phase) – MODEL 2 – cables with prestressing force from phase 1 (reduced for predicted losses by relaxation) + self weight + dead load + live load. In this phase we calculate deflections and forces in cables.

Then, as simplification (because Robot can not update geometry through phases), summarized deflections from phase 1 and 2. The sum is total/final deflection. And the force in cable is total force for cable design.

During construction it is probably impossible to measure elongation, but pressure on prestressing machine is possible (also vertical deflection of complete structure as control parameter).

If deflections in this phase are not satisfied, we need to get back in 1 phase and increase prestressing force or even increase the cable diameter and prestressing force.

For this kind of bridge analysis of vertical vibrations is also very important, I am not familiar that we can do this type of analysis in Robot.

Regards

[Artur.Kosakowski · Accepted solution]

Hi @Anonymous

I'm not an expert in the cable bridges and IMHO the assembly is usually done by a specialized company but my understanding is that the cable assembly is made in the SEQUENTIAL way:

1/ one group of cables is assembled with some pre-tensions and if required tension forces are obtained these cables (cable lengths) are fixed

2/ then another group of cables is assembled with some pre-tensions and if required tension forces are obtained these cables (cable lengths) are fixed too. Usually the assembling of the second group results in changing tension forces in cables of the first group comparing to their original tension forces (from point 1).  So it is different than simultaneous assembling of all cables

3/ then another group of cables is assembled ...

The practical approach may be sequential creation of the model like below:

a/ adding cables corresponding to step 1/ above  defined by tensions and running analysis

b/  checking regulations of cables added in step a/  (see the description of cable regulation in help) and replacing tensions in definitions of these cables by their regulations (input as positive or negative absolute elongations)

c/ adding cables corresponding to step 2/ above  defined by tensions and running analysis

d/ checking regulations of cables added in step c/  and replacing tensions in definitions of these cables by their regulations (input as positive or negative absolute elongations)

e/  adding cables corresponding to step 3/ above ...

... 

In the final model only the last assembled group of cables would be defined by tensions - all the previously assembled would be defined by elongations but these elongations would correspond to tensions from previous stages of assembling.

If one or more of these posts answered your question, please click Accept as Solution on the posts that helped you so others in the community can find them easily.

[Artur.Kosakowski · Accepted solution]

Hi @Anonymous

I have altered the parameters of the load cases and combinations and all of them converge now. See the attached file.

If one or more of these posts answered your question, please click Accept as Solution on the posts that helped you so others in the community can find them easily.

[Anonymous]

Hi Artur,

I think you have explained this very well and that is exactly procedure by my opinion needed for this kind of structures (in case of cable stayed bridge with many phases I am not sure can we do this, but in case of a model in post yes !).

Looking at the results of model you attached, deflections demand are not satisfied (if we took limit v=L/250=9300cm/250=37cm and for combination 7 you have 100cm, with a note that I am not familiar what is exactly Eurocode demand regarding deflections limit for this type of structures).

I want to say that some prestressing is necessary to decrease vertical deflections.

''In the final model only the last assembled group of cables would be defined by tensions - all the previously assembled would be defined by elongations but these elongations would correspond to tensions from previous stages of assembling.''

So, just to clear modelling in Robot, because I generally understand what you said but I am not 100% sure how to do that in Robot.

1. Are we agreed that we can model this structure in Robot as you proposed, with sufficient accuracy ?

In that case we need two models and following procedure will probably be:

2.  Phase 2. / model 2. - is final phase. In this model we don't play with prestressing force in cables, we just need to calculate additional elongation of cable. When we have elongation then we can calculate additional force in that cable and we can estimate initial available prestressing force in cables that we can use for phase 1/model 1 (assembly stage). Also where to find a value of additional elongation of cable?

3. Phase 1. / model 1. - is assembly phase. Model of structure which includes self weight + prestressing force (available prestressing force which can be defined as cable resistance force (with safety factor) minus additional tensile force caused by relative elongation in model 2). In this phase we calculate deflections, and of course check all other elements. Using prestressing in assembly phase we will probably get upwards deflections!

4. Then final deflection is equal  = deflection from model 1 (probably upwards) + deflection from model 2 (probably downwards).

Regards

[Artur.Kosakowski]

Hi @Anonymous

Looking at the results of model you attached, deflections demand are not satisfied (if we took limit v=L/250=9300cm/250=37cm and for combination 7 you have 100cm, with a note that I am not familiar what is exactly Eurocode demand regarding deflections limit for this type of structures).

I want to say that some prestressing is necessary to decrease vertical deflections.

I'm not designing this bridge. I was only helping in converging the analysis for a model as it was attached

To  be honest I don't think I have enough expertise in this area to comment on your points and I'd rather leave this to somebody with the bridge design background. 

[Anonymous]

Hi Artur,

I am not also expert in this structure, but I learned something from this discussion about Robot possibilities.... 

Only I can say that Robot is excellent tool, hope Autodesk will continue to develop it.

Thanks 

Regards

[Anonymous]

Hi, Artur.

The model seems pretty good except for the negative (green) moment at every combination. I dont know why it is such high value.  It seems to be something wrong with the support at the end. 

Can you please help if you understand it? 🙂