User login


You are here

Modeling post-tensioned concrete in ABAQUS

Hi All,

 I want to model post-tensioning tendons embedded with concrete structure. Both ends of tendons are anchored. Can anyone inform me what kind of element most suitable to model the tendons and concrete structure in ABAQUS? I tried solid part for both items, yet as the tendon diameter is very small if compared to the concrete dimension, the resulting number of mesh on the concrete structure is very large.

I generate a box-like concrete and use the cut extrusion function in ABAQUS to create the ducts at which the tendons are to be located in the Assembly module. The diameter of duct is equal to the diameter of tendon, hence small instances are seeded at the edge of duct end before generating mesh.  

Can anyone suggest on how to model this post-tensioned concrete?



elabbasi's picture

You should look into the Embedded Elements feature in Abaqus. It's a simplification, but in many cases the sacrifice in accuracy is minimal compared to the reduction in model size (I believe there is good info in the Abaqus manuals on when this simplification is reasonable). For the geometry you described, you would again model a box-like concrete block, and a line or thin cylinder for the tendons. Instead of extruding you would just specify that the line/cylinder is embedded in the box, and mesh both geometries with regular meshes not affected by the diameter of the tendons.


Nagi Elabbasi 

Thank you very much for your suggestion. The tendon will be used to connect two adjacent box-like concrete blocks. Between these two concrete blocks, a space of gap is given (i.e. the two concrete blocks' faces won't coincide) and a rubber ring is located in the gap. The connecting tendon will pass trough the hole of the rubber ring. For this case, modeling the tendon as a solid element might be more suitable than as a line (i.e. beam or truss element). Hence, I will need to apply a solid element (tendon) embedded in a solid element, which is the concrete block. But then my question is that, is it still necessary to define rebar function in Abaqus to model the tendon? I believe there is no rebar layer definition for solid element using Abaus CAE, but maybe scripting in an input file is possible? The second thing is that do I still need to model the concrete-tendon interface using contact pair in Abaqus if I already use embedded element? I would really appreciate your suggestion. Thanking you in anticipation.


elabbasi's picture

Solid element can be used as embedded elements but not as rebars. That restriction is from Abaqus itself not its CAE. If you use embedded elements you cannot have contact at the interface between the embedded element and the host. The embedded elements are automatically constrained to the host. If you only want to capture the global behavior due to the tendons imbedded in the concrete this may be fine. However, from what you just described, it seems that you want to capture the local deformation close to the concrete-tendon interface as well. If that is true you should not use embedded elements.

Really thank you for your valuable comments. I need to analyze the global behaviour due to the tendons. I use intial stress condition to define the prestress of the tendons. From Abaqus documentation, it is written that for the structure given initial stress condition, the structure must be brough to a state of equilibrium before it is actively loaded. But, I dont understand which Abaqus keyword I need to use. I understand the keyword should belong to the step though. Do you know about this?

And also, for prestressed condition, I will need to include *prestress hold in my input file to avoid prestress loss in my model (correct me if I am wrong). But, can I also apply this prestress hold for the case of tendon modeled as solid element? It seems that Abaqus only recommends this feature for rebar. Would really appreciate your comments and thank you.

am working on post-tensioned element as well and am having problem in the interaction module (contact pair)am geting an overclosure error but i cannot find how to solve it however, am sure  that all steps  are ok. any suggestions? in addition do we have to add any constraint at the end of the tendon to simulate the anchorage?

I really appreciate any feedback

hello...i need help...i'm modeling post-tension also...

i don't know how model anchorage or model without anchorage....


please send me

hi, can you send me your cae file .. i need help in modelling of post-tensioned concrete


Subscribe to Comments for "Modeling post-tensioned concrete in ABAQUS"

Recent comments

More comments


Subscribe to Syndicate