contact between reinforcement and concrete 2

[PhDCivEng]

Hi!
I have to model a composite steel-concrete shear wall but I can't make to work the contact between reinforcement(including steel profiles) and concrete.Reinforcement and steel profile is modeled with LINK8 and concrete with SOLID65.
Thank's!

 

[ansysfreak]

Hi

You can do it by modelling the rebar element with use of the Concrete nodes. Also yo can use combin39 elements to connect the rebar nodes with the concrete nodes.
There is also the option in the Solid65 element to model the rebar as a real constant for this element.
Hope this helps.

 

[PhDCivEng]

I think that is a problem to do what you recommend me because the concrete element is meshed automaticaly and my rebars have a fix position by coordinates. I don't know now how to model the concrete element by reinforcement nodes.
If i use what you recommend me the contact is all aver the reinforcement surface or just in contact nodes?
About modeling reinforcement in solid 65 element, i made once this but I have some convergence problems!
Thank's for your answers.
I'm a novice in using Ansys and between my friend's nobody know's this program and that for I use this forum. I put this question also on others forums but I didn't received any answer!

 

[ansysfreak]

Hi

If you sliced your model at the location where the rebar is located you could make sure you have corresponding nodes for the concrete and rebar. The combin element needs to be applied in the ux, uy and uz direction of each rebar node, connected to three concrete nodes.
It doesn't really matter which methode you use the convergence troubles will always be there.

 

[PhDCivEng]

I will try to apply your recommendations and hope that works but I have a problem in viewing components of the model sepparately although I make two componets. one from vertical an d horizontal rebars and one from stell profiles. Which is your opinion about my model? It is to complicated? . One more question if it is posible: the load is in 70 steps as follows: from step 1 to 40 the value of the load is 400 N, from 40 to 50 the value of the load is 250N ...etc. When I look at the results I see that the program doesn't sume the step loads and gives the result's from every step load separatelly. I look in the guide and I think I have to make combinations between steps to have the result's from the sume off all step's. Is that correct?
Thank's a lot for your answers! Sorry for my english, i hope you understand my questions!

 

[skjoex]

Hi,

i am going to write the settings which i use. The time and number of substebs must be set correctly. Also i prefer do not leave solution-procesor between loadsteps and put command to tell the ansys to sum the loads:

FINISH
/PREP7
...
FINISH
/SOL

TIME , 40
NSUBST, ...
F,NODE, FZ, -400

SOLVE

TIME , 50
NSUBST, ...
FCUM , ADD !!! THIS TELLS TO ANSYS TO CUMMULATE THE LOAD
F,NODE, FZ, -250

SOLVE

 

[ansysfreak]

Hi

When You apply a load of -400N and after solve change this load to 250N it becomes -250N. So apply a load of 400N in the fist 40 steps then change the value to 650N. This way the load in step 40 = -400N and in 50 -650N.
You don't need to use the FCUM commando.

 

[PhDCivEng]

Hi,
Where from is this sign changing (from 250 to -250)?
If I do what you recommend me, can I view at the end of the analyse the value of stesses, displacements... in all substeps, or just in last one?
Thank's!