Transient Structural Analysis: Steel- Concrete beam

  • 698 Views
  • Last Post 07 January 2019
  • Topic Is Solved
hgsdvd posted this 16 November 2018

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,

 

Order By: Standard | Newest | Votes
SandeepMedikonda posted this 19 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

  • Liked by
  • hgsdvd
hgsdvd posted this 19 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

 

 

SandeepMedikonda posted this 20 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

  • Liked by
  • hgsdvd
hgsdvd posted this 20 November 2018

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,

 

SandeepMedikonda posted this 20 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

  • Liked by
  • hgsdvd
hgsdvd posted this 25 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

 

 

 

hgsdvd posted this 27 November 2018

I would really appreciate any suggestion that may help.

 

Best Wishes

Muha, 

SandeepMedikonda posted this 27 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

  • Liked by
  • hgsdvd
hgsdvd posted this 05 December 2018

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

 

SandeepMedikonda posted this 05 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

  • Liked by
  • hgsdvd
hgsdvd posted this 05 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,

SandeepMedikonda posted this 13 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

  • Liked by
  • hgsdvd
hgsdvd posted this 14 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,

SandeepMedikonda posted this 14 December 2018

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

Regards,
Sandeep

  • Liked by
  • hgsdvd
hgsdvd posted this 15 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

SandeepMedikonda posted this 15 December 2018

@peteroznewman

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

Regards,
Sandeep

  • Liked by
  • hgsdvd
peteroznewman posted this 15 December 2018

Dear Muha and Sandeep,

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

Regards,
Peter

  • Liked by
  • hgsdvd
hgsdvd posted this 15 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

peteroznewman posted this 16 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

 

  • Liked by
  • SandeepMedikonda
  • hgsdvd
hgsdvd posted this 16 December 2018

peteroznewman posted this 17 December 2018

1) Okay, then Bonded is acceptable, although you should include debonding failure for this interface as the bond strength between concrete and steel is fairly weak.

5) Cut the geometry off at the point where the supports were in the experiment and use those edges as the supports.

6) A welded connection has equal strength to the parent metal so it would be reasonable to unite the plates to the beam.

7) Send a new file when this is fixed.

8) You can only use shell elements on surface bodies, that is why you need to create the midsurface.

10) You might need a pad on top of the concrete to distribute the load to avoid that error. The pad would not have any failure criteria like the concrete but would smooth out the load before the concrete sees it.

  • Liked by
  • hgsdvd
hgsdvd posted this 17 December 2018

Dear Peter, 

Thank you so much for your response. 

I will modify my model according to your suggestions, and will let you know when it is done. However, If I may:

(10) I used a pad on top of the concrete during my attempts to solve this error. what I did was setting the type of the contact definition as a No Separation, and from the advanced list, the formulation was an MPC to ensure that there would not be any gaps or sliding. As a results, the pad got merged into the concrete slab as an error, which I interpreted it as a too much load on those small areas then I had to choose a different way to apply the load whether by distributing the load to the faces as you saw, or applying the load to the entire surface either as a force or a pressure. Any suggestion, Peter?

Thank you so much for you time, 

Muha,

peteroznewman posted this 17 December 2018

10) Leave the point load faces in and we will see if they are still a problem. Most nonlinear problems are best solved with a displacement input and not a force input because then the solution can proceed to the negative slope of the force-displacement curve. The best way to apply a displacement to a small face is with a remote displacement because then there is a single point and the face is free to tilt and flex about a center point.

In a model that loads a beam to failure, you will often have a model that fails to converge. That is not a problem. All you need is for the model to converge past the point when the force-displacement curve goes negative. Then you have determined the ultimate load capacity of the structure. If the model fails to converge shortly after that point, it doesn't matter. You could input a new limit on the displacement that stops the solution just before the point when the convergence failed, but it's not necessary.

  • Liked by
  • hgsdvd
hgsdvd posted this 18 December 2018

Dear Peter,

Please find the attached file after making some changes according to your suggestions.

Here are what I have done: 

1- I united all the stiffeners plates to the steel beam by using Boolean feature.

2- I cut my geometry off at the points where my supports were and used those edges as new supports. 

3- I used a midsurface to convert the beam into shell element and used SHELL181 element instead of the previous one SOLID185

4- I changed the element for the concrete from SOLID65 to SOLID185 to avoid some warnings shown in regards to material nonlinearity. Would you agree with that?

5-  FYI, the simulation goes well if the force is reduced. Does that means I need to refine the mesh better?

6- My last concern besides the above is that there are some triangle elements in the beam although I tried to use Automatic mesh > Hex and Face meshing but I received error. The reason why I am concern about this, is that I need to match the type and size of the mesh in the Static model with the one in the CFX to avoid any mismatching when it comes to the temperature mapping. What do you think?

Thank you so much for your time 

 

Best Wishes,

Muha 

 

 

peteroznewman posted this 19 December 2018

Dear Muha,

Some nice improvements there.

(4) You must use SOLID65 if you want to use the CONCRETE material model since they each require the other. The SOLID65 element has the ability to record cracking and crushing behavior of the CONCRETE material model.

You can switch to the Microplane material model for concrete. That does not track individual cracks, instead it uses Plasticity to model the softening behavior of concrete as it fails.

(5) You can't easily refine the mesh because you are using node merge to connect the rebar to the slab, and when you change the mesh, the rebar is not near a slab node any more.

To fix that, change the slab body into a multibody part. Slice the solid horizontally through the rebars and vertically through each rebar. Then Form New Part with the 16 pieces of slab. You should make the element size on the slab and rebar equal. Now a rebar node will always be at a slab node.

I advise changing from Force to Remote Displacement.

(6) Don't be concerned about triangle elements. ANSYS has sophisticated mapping algorithms that take results on one mesh and accurately map them to another mesh. You don't need nodes to be in the same place on both meshes.

Another suggestion: You could put a plane in the center of the beam and add a Symmetry BC to cut the model size in half.  Leave the roller constraint to support the remaining edge as the Z direction will be taken care of by the Symmetry BC.

Regards,
Peter

  • Liked by
  • hgsdvd
  • SandeepMedikonda
peteroznewman posted this 22 December 2018

Dear Muha,

Yes, when you use Symmetry, it doesn't work on the line bodies. You can edit them to half the length and apply the Symmetry BC to the vertex on the center plane.

I have sliced the slab into 6 pieces by making a horizontal slice through the plane of the rebars and two vertical slices through the left two rebars.

If I make five more planes and five more slices, I will have all the rebar on the edge of a body that makes up the slab. Putting all the slab pieces into one multibody part will make sure the mesh holds the bodies together without any need for contact and the mesh on the slab and rebar can easily be made congruent so the Mesh Merge will work. Why can't you do that?

Add mesh controls to make smaller elements at the base of the steel at the support. Don't worry about trying to keep the same mesh on this model that you had on the Thermal model. I already explained that ANSYS has mapping capabilities to map results from one mesh to another. You have to make smaller elements on the Structural model so it will converge. Below I have added a Coordinate system to the vertex on the base. I have added a Body Sizing mesh control with a Sphere of Influence using that Coordinate system and a 100 mm radius with an 8 mm element size, while the global element size is 25 mm.

Regards,
Peter

  • Liked by
  • hgsdvd
hgsdvd posted this 24 December 2018

Dear Peter, 

Hope you are having a good holiday. I would like to thank you for your time in answering my concerns.

I followed your suggestions and here are what I have done: 

I used the Sphere of Influence method at the both ends to select smaller elements. I went to 1 mm as an element size in those area , but I still get the same error at the same area. What do you think the reason could be?

So desperately, I used the default mesh size, and surprisingly, the model got converged without any error and with an expected deformation as well. So my concerns now are:

1-  Computationally, can I trust on the default size to proceed with my simulation? If no, what steps am I missing here?

2- If yes, I moved on toward my last step which is mapping the temperature on the bodies. Hence, I received so many errors in the areas where the temperatures mapped even though I picked smaller elements size for those areas. Any suggestions Mr. Peter?

Acknowledgment:

Thank you so much for your great helps and suggestions that I have been given. I feel like I am getting close to the end of this drawback in my research because of you guys so thank you. Also, I apologies for making this thread longer than what it is supposed to be. However, I am pretty sure that someone will find it so beneficial as I do because of your great suggestions guys. 

Best Wishes

Muha,

 

peteroznewman posted this 25 December 2018

Dear Muha,

Real beams often have an extra thickness of material welded on at the point where the beam interfaces with the support. In this model, I think the reason the web fails right above the support is because in fact, the web fails right above the support. If you don't want that to fail, then add some more material to the web at the supports.

The reason a very large element will converge when smaller elements fail to converge is because the large element is missing the peak stress at the support. If you are only interested in failure at the center of the beam and are not interested in failure at the support, it is perfectly acceptable to have large elements that converge at the support, as long as you are aware that there is another failure mode that probably occurs before the concrete failure.

2- I don't know what errors you are getting from the temperature mapping. You will have to explain more.

Kind regards,
Peter

  • Liked by
  • hgsdvd
hgsdvd posted this 27 December 2018

Dear Peter, 

  Thank you so much for your reply. The issue of the failure at the supports has been solved. I added stiffener plates at both ends, and it worked.

  2) I have attached my archive file and screenshots of the analysis details. Kindly, would you mind having a look at it and then feed me back? Since the wbpj. file has both the CFX and the static model, the file is too large to be attached, so as a test, I inserted a thermal condition with 700 C to one of the surface bodies to simulate the temperature I have from the CFX model. 

   I have used different types of element (Hex, Triangle, and Tet), used solid model instead of the shell one, identified elements violation, and NR forces but none of which gave me a clear explanation on how to move on. Most of the errors I get when I run my model with the temperature load is either Element # is turning inside out, or has highly distorted. Therefore, I used smaller elements size but I noticed that smaller element size I pick, more errors I get. Apparently, the reason is as you explained in the previous post.

I would really appreciate any insights or comments. 

Thank you so much.

Muha,

 

 

 

 

 

 

peteroznewman posted this 27 December 2018

Dear Muha,

For Concrete, a Multilinear Plasticity model is used, but the first cell for stress should be the yield strength. 

Why are you putting such a small value in that cell?

In the Thermal Condition, why only put it on the web and not on the flanges?

Kind regards,
Peter

  • Liked by
  • hgsdvd
Show More Posts
Close