Transient Structural Analysis: Steel- Concrete beam

Hello Guys, 

I am working on a project where I am modelling a steel bridge beam. I imported body temperatures from a CFD model, where I studied the effect of the temperature to the beam with respect to time (55 min).

In the transient structural, I defined the structural and thermal materials of the steel and concrete including the Stress- Strain plot in the Engineering Data ( Attached 1).

The issue I get is when I run the structural model, I got this error:

*** ERROR ***                           CP =       1.125   TIME= 20:20:18
 The number of temperature specifications exceeds the maximum of 11 for 

 material number 1.  The TBTEMP command is ignored

 

Any idea will be much appreciated. 

Thanks 

Muha,

 

«1

Comments

  • edited November 2018

    Muha, you can't use hyper-elastic experimental data. That is used for Hyper-elastic curve fitting purposes only. You would have to use Multilinear plasticity (MISO) for the experimental data you show.

    Regards,
    Sandeep

  • hgsdvdhgsdvd Member
    edited November 2018

    Dear Sandeep, 

    Thank you so much for your comment. I overcame this issue by writing APDL commands under each material ( Steel, Concrete, and Steel reinforcement bars)

    I have selected the elements of SHELL181, SOLID65, and LINK180 for Steel, Concrete, and Steel reinforcement bars respectively. The issue I am facing now is that I am getting the error below:

     

    *** ERROR ***                           CP =       1.234   TIME= 21:28:08
     Element type 1 is not the same shape as SHELL181.  Switching to a      
     different shape is not allowed while elements of type 1 exist.

    I have changed the element to BEAM188 and BEAM189, but I am getting the same error. Kindly, below are the commands for the steel.

     Would you tell me where is the problem?

     

    Thanks

    Muha,

     

    Commands

    ET,MATID,SHELL181

    MP,PRXY,MATID,0.36 

     

    R,MATID,0,0,0,0,0,0

    RMORE,0,0,0,0,0

     

    !Density (C) and (kg m^-3)=========

    MPTEMP,,,,,,,,  

    MPTEMP,1,20  

    MPDATA,DENS,1,,7850

     

    !Modulus of Elasticity (C) and (MPa)==========

    MPTEMP,,,,,,,,

    MPTEMP,1,20

    MPTEMP,2,100

    MPTEMP,3,200

    MPTEMP,4,300

    MPTEMP,5,400

    MPTEMP,6,500

    MPTEMP,7,600

    MPTEMP,8,700

    MPTEMP,9,800

    MPTEMP,10,900

    MPTEMP,11,1000

    MPTEMP,12,1100

    MPTEMP,13,1200

    MPDATA,EX,1,,240000

    MPDATA,EX,1,,240000

    MPDATA,EX,1,,216000

    MPDATA,EX,1,,192000

    MPDATA,EX,1,,168000

    MPDATA,EX,1,,144000

    MPDATA,EX,1,,74400

    MPDATA,EX,1,,31200

    MPDATA,EX,1,,21600

    MPDATA,EX,1,,16200

    MPDATA,EX,1,,10800

    MPDATA,EX,1,,5400

    MPDATA,EX,1,,0

     

     

  • edited November 2018

    Muha, I don't see what analysis( 3D, 2D?) you are doing or what geometry you are using?

    Multilinear plasticity will use TBPT data for each command. Please see this post. I recommend you to use Engineering Data to proceed with the definitions. This way mechanical will correctly determine the compatible element for your analysis.

    Regards,
    Sandeep

  • hgsdvdhgsdvd Member
    edited January 2019

    Thanks Sandeep for you reply.

    Below is my 3D geometry(Attached).I saw the post you mentioned and was really helpful. Thus, this leads me to a few questions if you may. I am trying to define the structural properties(Density, Modulus of Elasticity, and Strain- Stress curve) of the model which consists of a beam(Steel), Slab deck (Concrete), and  reinforcement bars(Steel) with respect to the temperature (10-12 temperatures). I will use the Engineering Data for the steel materials as you discussed in the mentioned post. 

    The reasons why I shifted from the Engineering data to the Mechanical commands are first, I wanted to define the stress-strain curves of the materials with respect to the temperature (Attached). Second, I wanted to pick an element (Solid65) that would suit for concrete.

    So now i will follow you suggestion in the mentioned post which was using the Multilinear model to define a such curve for the steel, and will post  in a short while. Would that be my best option, knowing that I still need to define the Modulus of Elasticity with respect to the temperature? I would assume that I cannot use both platforms ( Engineering Data and Mechanical) together, then how can i define the Modulus of Elasticity?  

    Thanks a lot

    Muha,

     

  • edited November 2018

    Muha,

      Just curious, have you seen DrDalyos tutorial on this?

     

    You can define temperature-dependent elastic properties from Engineering data:

    This would write out something similar to what you had:

    MPTEMP,1,20
    MPTEMP,2,40
    MPTEMP,3,60
    MPTEMP,4,80
    MPDATA,EX,1, ,200000,150000,140000,120000, ! tonne s^-2 mm^-1

    I don't think this is the problem in your case. What are you referring to Element type 1 above? Check for that? See if this post helps?

    Is your simulation even starting?

    Regards,
    Sandeep

  • hgsdvdhgsdvd Member
    edited November 2018

    Dear Sandeep, 

     

    Thank you so much for your constructive comments on my post, and I apologies for the delay in getting back to you. Here is what I have been doing; I defined the material properties of steel by using the Engineering Data as you mentioned and I added the multilienear model as you suggested to define the stress strain curve of steel with respect to temperature. As a result, it worked and defined well. For the concrete, I used the Engineering Data too to define its properties as well as APDL commands to select the proper element (Solid65). Finally, for the steel rebars, I did the same as the concrete. However, I selected Link180 element for it. Then, I joined the concrete with the rebars by writing some mechanical commands ( Attached). 

    Now, what I am trying to do here is to run the model till deflection failure. For your information, I already performed an experiment and have its data, so I am expecting the failure to occur within an hour after loading the model with a constant load (800 KN). Initially,I was using Transient Workbench until a friend of mine who advised me to shift to Static workbench since I have a constant load.Hence, I did it.

    Here is the thing now, I have ran the model just for 5 seconds (Simulation Time) as a test, and it takes at least 2 hours and eventually, I keep receiving an error, either (The Element has been highly distorted) or(The element ''Solid185'' is turning inside out). So, I have refined the mesh(Attached), checked the contact pairs, and still receiving the same errors. 

    My questions now are, can I really use the Static Workbench instead of the Transient Workbench for my simulation since the Static is a bit faster? If so, how can I set the analysis to be ran for an hour or till failure? FYI, I used just one step and set the end time as 3600 sec (1 hr) (Attached)

    2- How can I overcome these errors and if there are more solutions that I can do further, please suggest. 

     

    Thank you so much for your help and it is really appreciated

    Muha,

     

    Concrete Commands:

    ET,MATID,SOLID65

    R,MATID,0,0,0,0,0,0

    RMORE,0,0,0,0,0

     

     

    TB,CONCR,MATID,2,9

    TBTEMP,20

    TBDATA,,0.2,0.8,3,30

    Rebars Commands:

    ET,MATID,LINK180

    R,MATID,6,,0

    Connecting the concrete and the steel rebars together commands:

    /PREP7

    /NERR,200,99999999,,0,0

    ESEL,S,ENAME,,65

    ESEL,A,ENAME,,180

    ALLSEL,BELOW,ELEM

    CEINTF,0.00001,

    ALLSEL,ALL

    /SOLU

    OUTRES,ALL,ALL

     

     

     

  • hgsdvdhgsdvd Member
    edited November 2018

    I would really appreciate any suggestion that may help.

     

    Best Wishes

    Muha, 

  • edited November 2018

    Muha,

      If it is that long a simulation and it doesn't look like you have any dynamic or inertial effects, yes do a static analysis.

      Turn on auto time stepping. Above you are asking the solver to achieve convergence in 1 go or using the default substeps which is usually not enough. See here. Peter has provided numerous solved examples on the forum. See these for example:

    Discussion 1

    Discussion 2

    Regards,
    Sandeep
    Guidelines on the Student Community

  • hgsdvdhgsdvd Member
    edited January 2019

    Dear Sandeep, 

     

    Thank you so much for your time in replying my questions. 

     

    I did what you suggested. I am still getting errors (Element highly distorted) and ( Solid185 is turning inside out). I have constrained the model using fixed supports at one end and roller support from the other end. I have tried adjusting contact stiffness of contacts I identified using NR Residuals, refining the mesh, increasing steps and sub-steps to gradually apply the displacement and everything I could find which may help but the model doesn't converge. I am coupling the model with ANSYS-CFX to import the temperature I got into the Static Structural Model. 

    My questions now are: 

    1- How can I get the model converged 

    2- As a test, I did not assign any loads to the slab. However, my model still deforms at the area where i am supposed to assign these loads to. What would be the problem.

    3-  It appears that there is no bound at all between the concrete and the reinforcements although I used the commands below( Attached).

    4- I have tried to attach an archive file to kindly if you have time, look at it , but the issue is that the file has the CFX model which makes it too large to be attached. Is there any way that you can  have a look at it if you may?

    5- Lastly, the running time is taking forever although i reduced the No. of nodes and elements but still longer than usual. For example, to run 10 s , it takes couple of hours and eventually, I receive an error. Any Idea? 

     

    Thank you so much Dear Sandeep. Frankly, your comments have been so helpful and will appreciate any comments or insights. 

    Muha 

     

    Connecting the concrete and the steel rebars together commands:

    /PREP7

    /NERR,200,99999999,,0,0

    ESEL,S,ENAME,,65

    ESEL,A,ENAME,,180

    ALLSEL,BELOW,ELEM

    CEINTF,0.00001,

    ALLSEL,ALL

    /SOLU

     

  • edited December 2018

    Muha,

      What you are specifying for the time stepping is not reasonable. Change Define Time by to Steps, Change Initial Substeps and minimum substeps to 50, Max Substeps 500 and give that a try.

    You are also removing the Force Convergence, I wouldn't recommend doing that, Change Displacement Convergence to the defaults. Also, try a case with Line search and see if that works.

      Just try getting the solid model to converge and complete first before coupling with CFX?

    Regards,
    Sandeep

  • hgsdvdhgsdvd Member
    edited December 2018

    Dear Sandeep, 

       Certainly, I will give your suggestions a try. The reason why I used these time steps is that I ran the CFX model with a time step of 1s for 3600s as a running time. So, to avoid any problems in the convergence, I set the structural model with the same time steps. Secondly, I want to run the structural model for an hour (3600s) so I thought that by setting the definition of the time step as substeps, would take ages to be solved. As a result, I chose time with a 1s instead of substeps. However, I guess I misunderstand the time steps concept but surely will give it a shot. 

       For the Force Convergence, I deleted all the convergence criteria except the Displacement one since I am interested only in getting the Time- Displacement Curve from this simulation. So, I thought by doing so, it would solve faster but again I will do some modifications according to your suggestions and will be back to you.

    Thank you Sir for your time. 

    Best Wishes

    Muha,

  • edited December 2018

    Muha,

      I am glad you are making progress. However, I have to say that I don't have much confidence in these results if you remove force convergence. It is extremely important to understand how FEA works and how numerical algorithms approximate this.

    " If your model contains non-linearity it cannot be solved directly, so must be found by iteration. Although you cannot find an exact solution, you know you have something close when the energy you put into the model through loads roughly equals the energy output of the model through reactions.  The convergence criteria defines how close to this exact balance is acceptable."

    Please see the following discussions to get a better understanding.

    Discussion 1

    Discussion 2

     

    I think the above-mentioned reason is your bigger problem. However, for the elements turning inside out, have you tried using quadratic elements ( keep mid-side nodes on / program controlled)? This should help.

    Regards,
    Sandeep

  • hgsdvdhgsdvd Member
    edited December 2018

    Dear Sandeep,

     

    Thank you so much for your reply. I attached my archive file. Would you mind having a look at it and tell me what I am missing?

     

    Thank you Sir,

    Muha,

  • edited December 2018

    Unfortunately, I am not allowed to Muha. Maybe someone else on the community with permissions can.

    Regards,
    Sandeep

  • hgsdvdhgsdvd Member
    edited December 2018

    Dear Sandeep, 

    Thank you so much for your reply. So, would you mind tagging or mentioning someone who has a permission to look at my file? I am pretty sure that I am missing something but I do not what it is. 

     

    Best Wishes, 

    Muha

  • edited December 2018

    @peteroznewman

    I know it's the holiday season but if you have time can you help Muha here?

    Regards,
    Sandeep

  • peteroznewmanpeteroznewman Member
    edited December 2018

    Dear Muha and Sandeep,

    I will take a look at the attached model and reply, but probably not till tomorrow.

    Regards,
    Peter

  • hgsdvdhgsdvd Member
    edited December 2018

    Dear Peter and Sandeep, 

    Thank you so much both for your time. Please feel free whenever it is convenient for you. I just updated the archive file according to recent changes.

     

    Best Wishes,

    Muha

  • peteroznewmanpeteroznewman Member
    edited December 2018

    Dear Muha,

    I opened the archive attached to the previous post and have a few comments.

    1. I question why the concrete is bonded to the steel beam. Was the concrete cast over the beam?  It seems more likely that the slab was cast separately and was later placed on top of the steel beam. Therefore, I would suggest a frictional contact between the concrete and the steel, not a bonded contact.

    2. Why do you want to prevent lateral buckling? If the steel beam is going to buckle, wouldn't you want to know that?

    3. The displacement BC "Bracing for Lateral Buckling" which sets a zero X displacement along the entire steel flange edge on one side only is inappropriate. I don't believe this represents an actual brace in the experiment. I recommend it be suppressed.

    4. With the Bracing gone, something else is needed to constrain the X displacement. It should be added to the two nodal displacements.

    5. The Nodal Displacements are not robust against mesh edits. It is better to apply BCs to Geometry not Nodes. Why not just use the end of the beam?

    6. I recommend a Boolean to unite all the stiffening plates to the beam solid so there is no need for bonded contact.

    7. Is there a reason why the steel beam plates don't line up at each end (they do line up in the middle)?

    8. I recommend you convert the steel beam to a midsurface shell model to reduce node count. I tried to do that but item #7 prevented a clean midsurface model.

    9. I believe the mesh on the concrete and rebar is too coarse. Increase density by a factor of 3 or 4.

    10. The small faces on the top of the concrete are not being used. Delete them.

    Make some changes to your model and reply with a new archive attached.

    Regards,
    Peter

     

  • hgsdvdhgsdvd Member
    edited December 2018
Sign In or Register to comment.