Reinforced concrete beam

  • 260 Views
  • Last Post 10 October 2018
  • Topic Is Solved
manuelhermanus posted this 11 April 2018

Dear all,

i am modelling the a continuous beam to analyze with frp after initial crack from loading  . I am new to ansys and dont seem to get much help on this. I keep getting various errors after always reviewing. Errors seem to be based on my support conditions and how to generate them.

Am sorry this is really silly question but how do i get around this.

Thanks Mannie

Attached Files

Order By: Standard | Newest | Votes
peteroznewman posted this 12 April 2018

Hello Mannie,

There are a few problems with your model.

You can't use no separation contact between your beam and the pressure plates on top or the blocks below because those bodies are free to slide around the face they are on since that is what no separation allows. You could bond them to the concrete, you you could simply split the face where those blocks touch and delete the blocks, fixing the three faces on the bottom and applying pressure to the two faces on the top.

The Analysis Settings only allowed one iteration per step. That is not recommended and there is a warning in the output file to that effect. I changed it to 1 step with 100 substeps.

 

I reduced the total force applied from 1,200,000 N (30 MPa on 0.04 m^2) to 20,000 N.

I put 3 elements across the thickness. I also added the code to plot the cracking.

 

You didn't say what version of ANSYS you were using. Attached is an ANSYS 19.0 archive.

 

Attached Files

manuelhermanus posted this 12 April 2018

Thank you; You have been so much helpful.

I am not sure i understand what you mean by put 3 elements across the thickness

If i were to include frp reinforcement over the maximum moment zones per span; i could use the no separation  contact as mentioned earlier if i understand you correctly ?

Do you reckon omission of shears would affect the flexural output ?

Also,how may i be able to compare stepped loading with generated strain until failure whiles observing crack behaviour ; especially when i add the frp?

 i use 18.2 version.

Thank you

 

manuelhermanus posted this 17 April 2018

Hello Peter, ,

Kindly, assist me  with the above inquiries 

Regards.

peteroznewman posted this 17 April 2018

Hello Manuel,

Sorry for the delay. You have a rectangular section, height x  thickness and that section has some length. I put 3 elements, along the thickness direction.

Explain why you want to use no separation contact?  I think it is because you want the beam to be free to "slide" or "roll" on that support. I achieved the same result by using a remote displacement, and only set the vertical DOF to be zero and left all the other DOFs Free, so I get that effect.  I don't understand how no separation contact has anything to do with frp reinforcement, please clarify that.

One way to reduce the size of your model is to put a plane of symmetry at the center of the length, that will cut your model in half and allow you to use smaller elements on the remaining half without exceeding the student limit.

I don't know what you mean by "omission of shears", please explain that.

For your last question, I think creating a multi-step analysis will allow you to plot the crack at many intermediate loads to failure.

Kind regards,
Peter

krishnadondapati posted this 10 October 2018

Hi Peter,

I tried your suggestions with the Mohr-coulomb model but it doesn't worked with my model so now i'm trying to solve using SOLID65 without reinforcement. for that, First I tried to solve the above-attached model for reference but it's not giving me the crack plot. presently I'm using Ansys 19.1.

 

Kind Regards

Krishna

Close