Composite curved bridge
Hi,
I was looking at your original post over the weekend and I did compose a reply regarding some recommended practices, but you made a second post before I actually posted my response and it just disappeared and I couldn't retrieve it.
My response basically suggested that the best approach for a curved composite deck was the FE web approach - as you seem to have adopted anyway - as this allowed explicit modelling of the bracing which, due to the interaction between transverse bending and torsion of, plays a major part in the global behaviour of the deck. However, I did warn about the size of the model, even for a single span, that this may make analysis times unworkable (especially if load optimisation and dynamics was required). My recommendation was still to use this approach but to be as economic as possible with the fineness of the mesh.
I have examined your model which you kindly attached to your second post, which is very detailed, and I cannot see anything wrong with what you have done, but the number of elements in each of the webs is quite large which seems to have made the model large enough to fail in the analysis. I have tried various tricks that I have used in the past such as renumbering the joints, adjusting the memory parameters in the "Options menu" but cannot get a solution for a single load case.
I will continue to try to find a solution, as this is quite unusual, and I have created models like this in the past and not had the same problem. This is a screenshot of a five span FE web composite deck I have created where the only real difference to your model is that I only used two elements in the depth of the web. I can appreciate that you may need a few more as your bracing is not at the level of the flanges but I believe these could be minimised to get your model to work (you can provide non uniform spacing to suit your needs).
Sorry I can’t be more help at this stage, but I will continue to investigate for a short while to see if I can find a workaround.
Kind regards
Dave Geeves
Accepted solution
Hi,
Since my last reply I have done further research by reducing the number of elements in the depth of the webs to 4 rather than 14 with relative spacing 0, 0.1, 0.5, 0.88, 1.0 so that the nodes coincided with the nodes of the bracing. I also made adjustments to the default torsion calculation grid size for the design sections to 20 by 20 as the large numbers you had set were affecting the analysis time quite considerably. In addition I set the memory management parameters to 250 and 250 to ensure a reasonable size for this model.
This gave me a good solution with the three dead load cases analysing and returning all results in about 30 seconds. I created influence surfaces for all points along virtual member 1 which took about 15 minutes with subsequent load optimisation for sagging moment using LM5 taking about 1 minute which generated about 120 load cases and 99 load combinations. It took 12 minutes to solve all these load cases and return the results, which on an initial inspection looked as how I would expect them to.
I hope this has helped to get your analysis solved and if it has please mark my reply as a solution so that others may benefit. Thanks
Kind regards
Dave Geeves
Hi,
Good news, I think I may have a solution to your problem in solving the normal modes analysis for your curved composite deck.
Following my previous thoughts that the matrix bandwidth was the problem I decided to renumber all the joints and elements in the model so that there was a general progression along the span. This isn't going to reduce the final bandwidth of the problem, as the program tries to optimize the starting bandwidth, based upon the node and element numbering by internally renumbering. I believe the root of our problem is that the starting bandwidth was so large that the memory required to optimise it was too much. Hence, by optimising a starting point the memory required would be less.
So to summarise I first of all renumbered the joint using the joint details form by sorting the joints first by "longitudinal beam" then by X coordinate, then by Y coordinate and finally by Z coordinate. I then renumbered the joints from 1 in the sorted order.
I did the same in the member details form by sorting the elements using the first node reference and then renumbering this sorted order from 1.
Finally I set the memory parameters from the options menu and I was able to get a solution for ten mode shapes.
From this I did notice that the vertical positions of the joint in the web of one of the girders was not the same as the others and the diagonal bracing was not connecting to this web. So these will need correcting before the renumbering takes place.
You will also notice that the steel webs are very flexible as they have no stiffeners modelled and many of the modes generated are just vibrations of the webs or other flexible components. I think web stiffeners should stiffen up the response.
I hope this helps. Please mark this post as a solution if it has helped solve your problem so that others may benefit. Thanks
Kind regards
Dave Geeves
Dear Gave,
Thank you for your support, I appreciate it.
I follow all your steps and the dynamic analysis now works.
I also put the transverse web stiffeners but I realize that the period/frequency doesn't change and the steel webs still seem very flexible in the deflected mode. This makes me wonder if I put the web stiffeners correctly in the model.
Could you have a look at the model now?
Thank you Dave
Accepted solution
Hi,
The web stiffeners define in the design beams do not automatically get created in the analysis model and are used for web design checks in the actual beam design. You will need to manually create the vertical web stiffeners and assign appropriate section properties within the structural model.
I manually added vertical members at each location in the "Bottom Bracing" sub model as shown (I did this by creating a single beam going from top flange to bottom flange and then using the "Split members" facility in the sub model members form and selecting to split at crossing nodes to form the four vertical members at each location. I created a new section made up from four of the angles you previously used and assigned this to the new members.
The dynamic solution still worked so there was no need to renumber as before. The mode shapes created now seemed a lot more as I would expect, with the main bending mode at about 4 hertz and the second bending mode at about 10 hertz (shown here) with a lot of the local modes of the flexible webs now not existing in the first 10 modes
I hope this helps.
Kind regards
Dave Geeves