Hi,
I have a new project to design a tank foundation. The layout will be similar to the one that I am attaching. I would like to know the following:
Thank you in advance,
Sofia
Solved! Go to Solution.
Solved by Rafal.Gaweda. Go to Solution.
- Does Robot Millennium models these kind of structures?
- If it does, which elements should I use (i.e. shells)?
As shells.
Can Robot Millennium design the foundation according to EC8 and EC2?
It can calculate reinforcement for plate and shells. You have to calcaulate is as a slab \ panel(s) on soil specifying correct kz value
As mentioned earlier, use panels to model the tank. Robot will then mesh the panels into shell elements for you. Depending on how the tank attaches to the foundation, I would model the tank seperately from the foundation. You can then save a copy of the model, create the foundation, eelete the tank, and copy the reactions from the previous tank design to your foundation model as loads. This can speed up calculation time as Robot won't have to analyze the tank each time. There are macros on this forum that help transfer loads from one model to the other. See attached example. This is an example of a tank that sits on the foundation but only has anchor bolts for uplift resistance. You will see compression only springs at the base of the tank and regular springs (representing the anchor bolts) at the bolt locations. The reactions are transfered to a foundation only model which runs much faster than when both are together.
I modeled the foundation of tank using shell elements, but when I tried to analyse it the software could not find solution due to no convergence of iteration. Is something that I can try to overcome this problem?
@Anonymous wrote:Is something that I can try to overcome this problem?
You have set up a nonlinear problem (elastic foundation/uplift) and your combinations are linear.
You have to set up nonlinear cases/combinations too and try to manipulate the non linear parameters.
Sofia,
Are you sure the base plate should be 0.01 cm thick?
Are you sure the pipes and upper plate should deflect 113 cm under selfweight?
Effect on bottom plate - "peaks" of 113 cm for sw
With 10cm base plate sw case converges smoothly
Please find attached a dwg that explains my modeling. What I did is to use this 0.01 "film" plate in order to give the subgrade modulus properties under the 60cm and 200cm shells that are forming the foundation. I did this to take into accound the right level of horizontal forces application points and also the level of the base of foundation.
In order to overcome the problem of converges, I changed the Kz properties of Film plates from Uz+ to none. I also applied a 30% of Kz as horizontal subgrade values. The result was to overcome the problem of analysis, but the results don't seem right. If you check the vertical displacements of the "film" panels, all the displacements are concetrated at the edge nodes and not uniformly to all the panel. The center of the panels have zero displacement or even possitive. I also tried to take out the Kz from the panels and put spring supports to all base nodes. The problem remains the same. Why? Do you think that if I change the film plate's thickness from 0.01cm to 10 cm will have the right result?
So every pairs of slab node and film node should be connected by this pipe bar or rigid links
example:
The values of spring supports were:
Uz= 8000kN/m3*0.1m*0.1=80kn/m were 0.1X0.1m the area of each finite element
Ux=Uy=30%*80=24kN/m
the displacement for DL1 is equal to 30.8cm wich is 100 greater than the expected: 23.4kN/m2 (DL)/8000kN/m3=0.003m=0.3cm, where 23.4kn/m2=7029kN (DL resultant reaction) / 300m2 (area of base of foundation)
I think that the displacement of 30cm refers to 80kN/m3 that I applied as spring of each support.
You mean every node of finite element on film plate to be connected to the respective node of finite element of plate of foundation? Is there any way to make this easy, because I think that will take for ever!
You mean every node of finite element on film plate to be connected to the respective node of finite element of plate of foundation?
Yes.
Is there any way to make this easy, because I think that will take for ever!
A few seconds with bars http://screencast.com/t/n5HDenB9mM
some more with rigid links http://screencast.com/t/frMjo8r2ojN
Hi, I replaced the "film" panel with a panel of 10cm thickness with Kz, Ky,Kx the same to film panel and a material which has the same properties as C30/37 but almost negligible density. The results were fine!!
I finished my foundation but I have some problems with orientation of reinforcement and the bending moments to the small direction of 200cm thick panels.
For the reinforcement of pedestal ( 200cm thk shells) I tried two different things:
The two "test" that I describe above was in my attemption to make the pedestal act as "beam". The results when I used a shell of 200cm thick as pedestal with reinforcement under bending + T/C with polar system of main reinforcement were given a greater bending moment along the small dimension of the pedestal and not along the circular perimeter of it (or I think so, because I am not sure if I understand the orientation of bending moments and reiforcement correctly). The pedestal in reality will have the main reinforcement parallel to the perimeter of the pedestal and not perpendicular to it.
What is the right way to have results like the ones that I am expecting to see? is it better if the pedestal (shell 200cm) to be modeled as a beam and to connect it with the shells of 60cm with rigid links? what model method would you propose?
I split the zip file to two parts due to large file
And one more question, that maybe will solve my problem. At the tables of detailed results of maps for the FE, there is the choise to have the results at the panel/node or in elements centers. Because I have a lot of extremes at the nodes which is a local problem and I think that the solution will not be close to reality, can I design the elements (reinforcement required module) for the results in the elements centers? Can I represend to map of results the ones from the centers of the FE only and not the nodes? When it says " element center" it means the center of the FE or the center of the shell?
The one was to determinate as main reinforcement a polar one with center the point 0,0,0 (I wanted exactly the opposite, this reinforcement to be the secondary, and the perpedicular the main, but I couldn't find how to do that).
Example: http://forums.autodesk.com/t5/Robot-Structural-Analysis/modeling-a-water-tank-shell/m-p/4726915#M196...
I am not sure if I understand the orientation of bending moments and reiforcement correctly).
http://forums.autodesk.com/t5/Robot-Structural-Analysis/circular-slab-on-springs/m-p/3615446#M7437
Because I have a lot of extremes at the nodes which is a local problem
That's why I told you to use more connectors (bars or rigid links like on my movies).
can I design the elements (reinforcement required module) for the results in the elements centers?
No.
Can I represend to map of results the ones from the centers of the FE only and not the nodes?
No.
When it says " element center" it means the center of the FE or the center of the shell?
it means the center of the FE
Can't find what you're looking for? Ask the community or share your knowledge.