Sap2000 tunnel and friction

[Ashoknanyang]

Hi All,

I am checking the tunnel stress and internal element stress due to settlement. Can we model the soil and tunnel in sap2000?
Also I need to model to different materials, Can we model the friction between two different element in 3D solids?

Kindly help on this.

Thank you,
Regards,
ASVA

 

[stressed]

You could model the soil as a boundary condition using linear springs, frequency dependent links, or multi-linear plastic link for nonlinear soil P-Y T-Z. You could also define solid elements with the properties of soil. If the settlement is known, you would assign joint restraints and assign imposed displacements for settlement.

Friction can be modeled between different elements as joint friction between joints using a 2 point link for friction isolator. Use of joint constraints would allow you to "spread" the link across multiple joints along a surface.

 

[Ashoknanyang]

Dear "Stressed",

Sorry for the late reply. Thanks a lot for the valuable reply. I am going to model soil as 3d Solid and tunnel as well.
But do I need to assign any links or friction values between the tunnel solid and soil soilid joints?

Thanks a lot.

 

[stressed]

Ashoknanyang, I don't have experience modeling soil using solid finite elements, but this link gives some explanation on how to apply that approach

http://www.edwilson.org/BOOK-Wilson/16-SSI.pdf

Dr. Wilson does not make any mention of modeling friction links between soil element joints and joints on the structure being supported.

 

[Ashoknanyang]

Dear Stressed,

Thanks a lot for the help.

Kindly give me your valuable advise on the query below(See attachment also)
The track bed should not act together with tunnel bending after some limits(As shown in attachment|) any idea how to model this?

Thanks
Asva

 

[stressed]

Ashoknanyang, please don't create multiple posts for the same question. Your mesh does not look good at all. Adjacent areas or solids need to share common joints in order to have connectivity.

Use of edge constraints here isn't a good idea either because joints are too far apart. Please modify your mesh for tunnel and trackbed concrete such that they share common joints.

I'm guessing that you used the "general" mesh tool for the trackbed judging by the look of the mesh. You might try other meshing options such as mesh by gridlines after adding cylindrical gridlines (see attached screenshot) or mesh by selected points.

Regarding lack of contact after a certain level of tension, try defining and drawing a two-point multi-linear plastic link in which link stiffness drops to low stiffness or zero after your tension level is reached. Local axis 1 is the axial direction for a two-point link.

If your trackbed and tunnel are modeled adjacent to one another, you will need to select joints and Edit>Edit points>Disconnect in order create space between joints to draw the link. Otherwise you will need to model the areas/solids with a small gap between them wherever you need to model links.

 

[Ashoknanyang]

Dear stressed,

Sorry about the seperate post. Thanks a lot for your suggestions.
Regarding the mesh,in the photo I attached have not meshed yet.( I need to mesh later). The mesh shown in the picture is automatically divided solid element when I converted it from Shell. This is also one thing I cannot control the no of divided solid particularly when converting from shell element.

Regarding Multi linear plasitc link, (the clouded area in the attachment),for example my tension spring stiffness is 50KN/mm and compression spring stiffness is 1456KN/mm .Hence I should key in for tension
F= -50KN D= -1KN and compressionF=1456KN D=1mm Right?. But for effective spring stiffness shown above the clouded portion in the attachment not sure what should key in. Any advise ?


How about using Hook ? specify 0.1mm in link and stiffness will be zero after attaining 0.1mm crack.is that refelect true behaviour?
Sorry for disturbance.
Thank you,
Regards,
Ashok.

 

[stressed]

Ashok, your attached screenshot shows identical stiffness in both directions which you don't want to do. Tension and compression directions depend on how you draw the 2-point link, which determines the +1 local direction. Use set display menu to activate display of link local axis in order to view local axis directions and you will see.

Change units to KN, mm and input into the plastic link the parameters you describe above, except that you wrote earlier that tension direction has a limit.. and that limit can be specified in the plastic link.

A hook won't work because a hook, like a gap link, has a constant stiffness in each direction after the hook becomes active. A multi-linear plastic link is needed to model what you describe where you have a build-up force and then a break-away force causes the stiffness to reduce to zero or near-zero.

Regarding meshing, the key to meshing solid elements is to first mesh the shell elements the way you want them before extruding the areas into solids. There are many more mesh options for shell elements than for solid elements, which have fewer mesh options. Mesh by gridlines, for example, which I described above attaching a screenshot is very powerful, but can be used for meshing areas only, not solid elements. Mesh first with shell areas, then extrude into solids.

 

[Ashoknanyang]

Dear Stressed,

Sorry for the late reply

Thanks a lot for your help and time


Regards,
Ashok.