Community
Hi All,
I have a project which is an enormous diaphragm wall. The panels are 3m in width. The reinforcement does not extend into the adjacent panels, therefore the correct way to model is to apply a linear release to the edges. After trying that i noticed that moment was still being transferred to the adjacent panels. Therefore we decided to model the panels with a 20mm gap and connect them with a linking beam to reduce the differential displacement.
The problem is, some link beams have high tension on them, which is incorrect. Looking at the nodal displacements and the forces, there shouldnt be any tension on these beams.
I have attached screenshots to show this
"The problem is, some link beams have high tension on them, which is incorrect. Looking at the nodal displacements and the forces, there shouldnt be any tension on these beams. "
Not really . If you look carefully the nodal Ux displacements are perfectly compatible with the bar tension forces. Having a closer look at the bar of your picture which shows a 803 kN axial force , we have
following the formulas for Stress and strain below
Doing the math we have
Epsilon(strain) = Delta L/ L= (0,633596477-0,632966383)/20 =0,000031505
P/A(Axial stress) = E x Epsilon
P = A x E x Epsilon
P = 750000 x 34000 N/mm2(MPa) x0,000031505 =803377 N = 803,4 kN
, which is exactly the value you will get if you increase the decimals for force results in RSA
The linking bars you chose are very stiff and even very little displacement induces high axial forces in these bars and they are also transmitting moments as there are no releases on these bars
Have you tried linking these walls only with a single Ux rigid link??
Rafael Medeiros
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
Then , you have to link them with truss "compression only" bars which will make the analysis nonlinear
Rafael Medeiros
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
Yes ,
Use regular bars and then use bar releases and on the unidirectional tab set the diection Ux+ or Ux- that will allow only compression on these bars.
Don't forget to fully release your moments ( Ry and Rz) on both bar end nodes
I didn't understand why you are using 2 bars. I would use just 1 bar to simplify the model
Rafael Medeiros
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
so if i wanted to release it in tension and keep it compression only, to do this in the image below
and in the member tab, release the rotation??
Normally you will need to release the unidirecional Ux just in one of the bar ends. Ux+ or Ux- will depend to where the bar Local X axis is pointing. Just make sure all bars have the exact same local axes , so you can assign the same release label type to all your bars. You can adjust the Local x direction on Geometry/properties/Local member direction.
And then , just try with Uz+ or Uz- and check if the model behaves the way you want(compression only)
For the rotation , yes ,on the member tab on the nodes close to the both walls
Rafael Medeiros
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
Some remarks on your model .
1- You cannot ignore some warnings and never ignore an error(red text) . There was a warning I never had , " finite elements do not belong to any panel" . I selected them , selected their nodes and deleted them all. With that the inchorerent mesh error also disappeared.
2- As soon as you get a mesh you are satisfied , freeze it !!! Otherwise RSA will always rebuild the mesh again and again wasting analysis time every time you run the model
3- Your mesh in the upper part of the strucuture was not good. I changed the meshing method and some parameters to give me always square FEs.
4- As I told you before Unidirectional Ux release is needed only in one of the bar ends .Setting it on both ends was causing an instability warning on Ux direction
5- In a nonlinear analysis only self weight load case and the combinations are important as the other single cases like , wind , water , soil will never occur alone. And in your case ,as it is and underground structure , even the self weight will never occur alone . So I set all the single cases to be auxiliary. I ran the model only for the 2 combinations
6- I used the nonlinear settings below to make it converge . Sometimes it is better to set just 1 increment(Official support advice)
7- In job preferences , Structure analysis always leave the method on automatic , because some of the methods do not report all the instabilities that may occur ( also from official support)
Model attached
Rafael Medeiros
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
I am not with computer but meshing options are
Coons
Squares on square contour
FEs quadrilateral
All these 3 settings set to " forced" option.
Mesh the 3 perpendicular walls 1st . Then mesh all panels of the large front wall. And do not forget to freeze them all.
I will send the model later.
Rafael Medeiros
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
That is correct , if both sides are moment released , then there can be no shear on the beam if there are no loads on the span
Model attached
Rafael Medeiros
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
Bars with zero are those where their end nodes are translating on opposite direction and therefore they would be in tension if Ux had not been released unidirectionally on one of its nodes
Rafael Medeiros
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
Forums Links
Can't find what you're looking for? Ask the community or share your knowledge.
Post to forums
