## General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

#### Static Structural Analysis of Masonry Bridge subject to local scour

Subscriber

I am attempting to study the effect of pier settlement of unreinforced masonry arch bridges on the structural health of the bridges. I am using a macro-modelling approach as I am not interested in collapse mechanisms but rather early stages of structural deterioration.

I have modeled a bridge using different bodies with bonded contacts between the structural parts of the bridge (spandrels, arch barrels, foundations, abutments, backwalls and pier), and frictional contact between the fill and the surrounding parts.

I am aiming to get crack plots and so have used APDL commands to make use of Solid65 elements in all of the structural bits (with material properties adjusted accordingly).

I have constrained the model using fixed supports under the foundations and modeled settlement of the pier by defining a transnational and rotational displacement applied to the pier in the middle.

The problem I am facing is the model doesn't converge due to errors in element formulation; I have tried adjusting contact stiffness of contacts I identified using NR Residuals, refining the mesh, increasing steps and substeps to gradually apply the displacement and everything I could find which may help but the model doesn't converge unless I suppress the fill.

The fill is a mohr-coloumb material I defined and I suspect is the issue behind the convergence dilemma.

Any help or insight would be greatly appreciated.

Nayef

• peteroznewman
Subscriber

I was successful getting a Mohr-Coulomb material model to run in a mining simulation that a student on this site was building. The key there was to eliminate the fixed support at the bottom of the stack. A fixed support prevents motion in the plane, but the compressive forces from the pressure of material above causes a Poisson's Ratio horizontal spreading. This spreading causes tensile stresses to be created in the material above the fixed support, which Mohr-Coulomb could not handle. The solution was to replace the fixed support with three displacements supports for x=0, y=0 and z=0 on those three planes. This allowed the Poisson's Ratio spreading to occur without any constraint and so no tensile stress developed.

Can you use symmetry on your bridge? Cut it in half along the length and in half across the width, then you can use three zero displacement planes and eliminate the Fixed Support.

If you would like to save an archive of your model, I can take a look at it in ANSYS 17.2 and reply with any suggestions.  You can attach the .wbpz file archive to your post above as long as it is < 120 MB.  If it is larger than that, then Clear Generated Data on the mesh, Save As a new file name and File Archive for a smaller .wbpz file size.

Subscriber

Dear Peter,

The fixed support is applied to the foundations, the mohr-coloumb fill is in frictional contact above the foundations; so I am not sure your suggestion would work unless I misunderstood.

As for symmetry, the rotational displacement prevents applying symmetry along the z-axis, the y-axis symmetry is clearly out of the question and I may be applying a load at quarter span of one of the arches later on so that pretty much rules symmetry out.

I have attached an archive of the model, any suggestions would be great. Thank you very much.

Nayef

Subscriber

I think I've attached it successfully. If I haven't please let me know so I email it to you.

• peteroznewman
Subscriber

I have opened your archive and will reply with more details later, but looking at the Solver output, on the first increment of the solution, the solver successfully inverts the matrix, then writes out this warning:

DISP CONVERGENCE VALUE   = 0.1897      CRITERION= 0.9681E-02
EQUIL ITER   1 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.1897

*** WARNING ***                         CP =      38.953   TIME= 12:04
The material solution failed for element 93474 with material 13.

That means when the solver takes the nodal displacements and runs them through the material model, the material model cannot cope with those displacements.

Subscriber

Yes I have continuously received these warnings so I used named selections to identify the elements which fail and they're always within the fill body. I thought the problem could have been due to element formulation as that's the main reason the solution terminates. With that thinking I attempted to improve the fill mesh using Multi-zone meshing to improve warping, jacobian, aspect ratio etc... but it hasn't worked.

What I gather from what you're implying is the problem could be due to the material properties set for the fill? Should I be using a different element type ?

Nayef

• peteroznewman
Subscriber

Understand that I'm not an expert at soil modeling, so please take the information I provide as suggestions for further study.

I changed your model to have 1 step, just gravity, duplicated the Fill material and deleted the Mohr-Coulomb (MC) model so it is just a linear elastic material. I solved that and plotted the Maximum Principal stress on the Fill body and find a maximum tensile stress of 7800 Pa.

That magnitude of tensile stress causes the MC material model to warn that it has failed, which stops the solution from proceeding.

The physical process of building that bridge is that the arches are in place with gravity deforming them, then the fill is added layer-by-layer so there should be no tensile stress in the fill when it is put on the arch. After the fill is in place, the slab is poured. The ANSYS model has all those parts touching with no gravity, then the gravity is ramped on, creating non-physical tensile stress in the fill.

I am curious if there is a way to turn on gravity without the fill present, then allow the fill to be added in a second step.

• peteroznewman
Subscriber

Update: Given the result above, I modified the Fill material parameters and made a material called Fill 8000 and I changed the cohesion to 8000 Pa. Now the model will converge on load step 1 where gravity is applied.

The model is currently working on load step 2 where the movement of the pier is applied and is having some difficulties converging.

Subscriber

Thank you peter, since your previous comment I have been tinkering with cohesion and have gotten the model to run but attempting to balance getting the lowest cohesion possible while minimizing the number of substeps for the solution. Your insight has been of amazing help. Thank you peter.

• peteroznewman
Subscriber

Awesome. I will add that in step 2, for the motion of the center pier, the convergence was a lot better when the behavior of the Remote Displacement was changed from Rigid to Coupled.

Subscriber

Out of curiosity, what set up have you used for the Analysis settings?

I understand you apply the gravity in step 1 and the remote displacement in step 2, correct? How many substeps are you using and have you kept the step end time at 1 second for both steps? What solver type have you used and have you utilized any of the nonlinear controls?

In an attempt to speed up the solution, I use direct solver with stabilization (nonlinear controls) as well as changing the Newton-Raphson Option (Nonlinear Controls) to 'Unsymmetric'.

Also do you think splitting up the gravity and the remote displacement into different steps has a significant affect on the solution, both speed and percision?

Nayef

Subscriber

Hey Peter,

I have run into a new issue, every time the solver reaches 1/3 of the step where the remote displacement is applied multiple bisections occur and the model becomes increasingly difficult to converge.

I have tried applying the gravity load and remote displacement in the same step, and in different steps. I have also tried changing the displacement behavior to coupled as you have advised but the same thing happens.

Nayef

• peteroznewman
Subscriber

I almost always use the Direct solver. I have never used stabilization or changed to 'Unsymmetric' on the NR Options.

Step 1 has Program Controlled Step Control.
Here are my step controls for step 2.

The solver got to Time = 1.87 so didn't quite get to the Y = -2 mm and Rx = 0.115 degrees since it didn't converge after 26 iterations. But as I said above, this is a lot better than with the Remote Displacement as Rigid.

I like the idea that the gravity load alone converges before the pier starts moving.
You could try breaking up the Remote Displacement into two steps, one for the Y motion, and another for the Rx motion.

Peter

• peteroznewman
Subscriber

Update: by breaking step 2 into two parts, translation then rotation,

it was able to complete the old step 2 by getting to the new step 3 in fewer iterations.

Subscriber

Dear Peter,

My model is still giving me false results as I am trying to get nonlinear results through the use of solid65 element for the masonry. To test if the command I am using is working I have created the cube test attached and it has confirmed my suspicion that its the element definition causing convergence issues and false results.

Do you have any experience with APDL commands? can you take a look at the archive I've attached ?

Thank you,

Nayef

• peteroznewman
Subscriber

Dear Nayef,

I don't have much experience with APDL. Can you decode what this means?

et,matid,solid65

MP,Ex,matid,1500

MP,Prxy,matid,0.2

MP,Dens,matid,2400e-9

TB,concr,matid

tbdata,1,0.3,1,0.304,4.278

What do you expect to happen when you apply a uniaxial compressive stress to this material?

I created a "test cube" to demonstrate the behavior of a material model. That model has exactly one element, but it has three displacement BCs, one on each plane with only the normal displacement set to zero.

Regards,

Peter

Subscriber

Whenever a flexible body is created I believe Ansys sets the default element as Solid186 which doesn't support crushing and cracking. Basically, based on the type of analysis used Ansys Workbench will use the element it thinks is most suitable. A 'legacy' element called Solid65 does support crushing and cracking so I need to switch to the use of that element.

I've found out there are two ways to go about changing elements:

(1) Write input file and open model in ansys mechanical and switch element type there.

(2) Using command blocks in workbench.

I have been attempting both but since I am not at all familiar with Ansys mechanical I have little idea of what I a doing there. The command I have applied basically says the following:

ET = set element type

matid = use the material id for this body

solid65 = the element I want to use

MP = material property command

Ex = Young's modulus (set at 1500 MPA)

Prxy = Possion's Ratio (set at 0.2)

Dens = Density (set at 2400e-9 kg/mm3)

TB = Activates a data table for material properties or special element input

CONCR = material model chosen is concrete

tbdata = specify the material properties in the table (the first 1 specifies starting at the first cell of the table)

0.3 = Shear transfer coefficients for an open crack.

1 = Shear transfer coefficients for a closed crack.

0.304 = Uniaxial tensile cracking stress.

4.278 = Uniaxial crushing stress (positive).

With this test I am trying to reach a nonlinear state in the cube and see the stress progression as well as create a crack plot using the command in the solution.

see attached for the CONCR properties table.

• peteroznewman
Subscriber

Thanks for that. I have learned that whenever command snippets are used, it is critical to run the solver in the same units that were used when the command snippet was inserted since the numbers in the snippet don't have units on them.

I ran your model at 1 MPa pressure to get it to converge so I could see the output that was generated.

Subscriber

Yes, I have just figured out the units issue and am playing around with it to validate results.

The crack plot should be in the solution section under command ( only appears after solver has run).

• maurya
Subscriber

HELLO NAYEF

have you succeeded in changing element in workbench, have you you checked the element in the solution output.

i also tried                                et,matid,solsh190

keyopt,1,1

keyopt,2,1

but command haven't worked means no error during solving but in output file its shows  solid186 or 185 is used.

it override the commands.

if i am doing any mistake please correct me in codes.

thank you

Subscriber

I think my solver output confirms that solid65 is applied, a better way to check is to open the model in mechanical and check elements in there. When I did that it confirmed that I am using solid65 element. I am still suffering from the convergence problem which I believe is due mainly to solid65 element formulation.

• Rana Nasser
Subscriber

Hi everyone!

Nayef or peter could any one of you please attach the model in ansys version 15 format?

many thanks,

Rana

• peteroznewman
Subscriber

Hi Rana,

You are lucky that I installed ANSYS 15.0 on a spare computer last week. I was able to recreate Nayef's test cube for Solid65 elements including the APDL code snippets for plotting the cracks. However, that /POST code only works if the solution finishes load step 1.  It is a difficult balancing act to get some cracks to appear while also converging at time = 1.  Is there a way you can /POST to other times besides 1.0?

Attached is an ANSYS 15.0 archive, with results, but no cracking.

• Rana Nasser
Subscriber

Hi peter,

unfortunately I did not deal with APDL codes before, but I'm going to meet a professor at my university who has a good experience in APDL codes this week and I'll show him the file and ask him to help in that problem.

• R123
Subscriber
Hello everyone Can anyone help me assign concrete cube element type with solid 65, I need to know how can I write commands and is solid 65 is suitable to concrete or not.
I need help
Thanks