Analysis of bridge girder (how to model)

[Anonymous]

Hello.

i am modeling a bridge in Robot, and have used "user defined section" to make the bridge girder for global analysis.
But i also want to do a lokal analysis. how do i approach this? 

the bridge deck is built up of the cross section i have posted. length of each section (between trans stiffener) is 5 meters.

So maybe someone have a good explanation or a link to a video that show this type of modeling and analysis?

Regards Espen

[StefanoPasquini6790]

Hi @Anonymous 

The best way to model your bridge is to find the section with high buckling risk, and model this part with shell elements, even to evaluate the stress diffusion in the cross section.

This process require a big use of rigid links (to connect the beam elements and the shell elements) and a good skill in modeling ...

Let us know if you need more specs!!!

Good luck

[StefanoPasquini6790]

Hi,

only for example, you can see this picture to understand my suggestion:

I use this kind of modeling trick when I have to investigate unusual steel connection, or other detailed analysis.

[Anonymous]

thank you for your answer. 

but i think i would need a video to get the full understanding of how to model this to get correct behavior. 

[Rafacascudo]

On the picture Stefano posted , The purple I shapes are bar elements . So they just have one of its nodes as a rigid link  master node  which is connected (fully rigid) to all  FE Model nodes that are on the frontier between I profile bar element- I profile FE object

[StefanoPasquini6790]

Hi @Anonymous 

As brilliantly @Rafacascudo said, it's a mixed modeled structure, where using rigid links to connect beam elements and shell elements and simulate the behaviour in tension or buckling problems for complex structures or detailed connection analysis.

Share here your robot model, indicating the section in which you want the shell model, and the acad profile of the cross section, in some minutes I'll reply with the mixed model.

[Anonymous]

thank you for your reply.

i see now that this can be a bit complicated for my cross section. i can possible make some simplifications.

[StefanoPasquini6790]

hi @Anonymous ,

attach here your robot model (specify the version!!!!) and the cad file of the cross section, I'll try to give you quickly the meshed model.

Robot is a very powerful tool, try to reach the limit of the complexity before you change path!!!

Cheers

[Anonymous]

Hello. And thank you for your help.

Here are my model and cad file of cross section.

[StefanoPasquini6790]

hi @Anonymous ,

which Robot version do you have?

[Anonymous]

sorry, forgot to write that. i have 2018

[StefanoPasquini6790 · Accepted solution]

Hi @Anonymous ,

Here attached your model, where I've added the Center Element made of shell elements, according to the cross section file that you sent.

The model is in 2018 version, and I've no evaluated the analysis and the results, the load has been transferred to the shell elements using a "dummy" bar placed in the midline of the section.

Sorry for the duration of my modeling, but I had a long lunch.

Let me know, cheers.

[Anonymous]

thank you 🙂 i think that was fast!!!
i will try to replicate this my self.

[Anonymous]

OK. so now i really want to learn this my self.
so i am wondering how you got the points from the cad file into robot so you could trase up the surfaces? 

hope you have time to explain.

[StefanoPasquini6790]

hi @Anonymous 

Here you can find the worflow I used in your case, that represent a complex one. Keep in mind that for standard section you can do the same in seconds using the "sectiontopanel" API, that you can find for free in the free API resource in the forum.

Well, let's start with the workflow:

1. Open the cross section ACAD file and draw a line in the midline of the elements. To do this you have to be as precise as possible. In your case I've divided in centerline the cross section and drawn half section. I drawn the arcs as lines and I had the foresight to break the lines at all intersections (you can find the attached file "1. Cross section.dwg") [10-15 minutes];
2. Starting from your Robot model, I exported the dxf file, to keep the perfect coordinate of all the elements in the model [2 seconds];
3. In the cross section cad file I've placed the elements so that the center of gravity in the point "0,0,0", and then selected all the lines and copied with reference point [2 seconds];
4. Open the cad model created in point 2, align the UCS with "zero" in the point where you want to place the cross section (keep in mind to the plane orientation and to use the same units in both files)....(you can find the attached file exported "4.1 base coordinate.dxf" and the file where I've done the cross section placing"4.2 gdl.dxf" where I've deleted all the unnecessary elements) [2-3 minutes];
5. Import in Robot the 4.2 gdl.dxf file, selected all the elements (CTRL+A), excluding the main centerline, and then copy all the elements with the "drag" option activated, and then copy along the main centerline [2-3 minutes];
6. Now, select all the bar elements and copy the selection text, open the "panel" command and paste the selection in the object field (see the attached picture) [1-2 minutes] 
7. Erase all the unnecessary panels, and set the correct tichness for the panels (you can find the "7. shell-section.rtd") then, select all (CTRL+A), then copy (CTRL+C) then open the main model file, keep in mind that you have to save the file you have created. [1-2 minutes];
8. In the main model, now, press CTRL+V, and the shell elements will appear in your model in the perfect coordiante you need....[1-2 minutes];
9. Now, mesh the panel elements, setting correctly all the parameters (there is a very good webinar with this topic), and then create the rigid links at the ends of the bar elements in both sides of the panels....[1-2 minutes]
10. Now you have to make some little adjustment in robot (tendons position, loads, etc....)[10-15 minutes];
11. Run an only self weight analysis and watch for the deformed shape and thension distribution, then run modal analysis (if you need to investigate dynamic behaviour) and take a look in the modal shapes....
12. if everything it's ok, your model is ready in about 40 minutes...

I believe that it's easier to do it instead of write it....you you have some problem in this workflow, don't hesitate to contact me privately.

Good luck

[Anonymous]

hello. i forgot to reply to you!
Thank you for your answer and that you took your time to help me!

[StefanoPasquini6790]

Don't worry @Anonymous , you are welcome.

Keep us updated with your model and your results.

Cheers

[ukohanietie]

Good day all, I have followed this thread and I could not help but wondered if the same idea applied to voided deck slab? and how you would approach this model I have idealized .