Problem with rocking wall modeling 1

[IRSHADQUR]

Hello Everybody

Can somebody guide me to how to model the unbonded PT tensioning in a rocking wall. (Shown in Figure)
1) One of the problem that i am facing is that i cant use a truss member for this purpose (Error which says missing property definitions)
Using a beam member and allowing all the rotations does not help either. (Results shows curvature of the bar with bending rather than showing axial behavior).

2) Its a contact problem as shown in figure, i am wondering that which kind of contact i should use for this particular problem.
Now i am using surface to surface contact but the message file shows some weird messages like Max penetration error, solution did not cnverge withing permissible limits, discontinuous points and sometimes negative eigenvalues problem.

Thx in advance and kindly suggest me some way to handle this as i have just started using abaqus and does,nt know much abt it.
Regards
Irshad

 

[burningDiesel]

I don't see why you can't use a truss member. Missing property definitions is not an analysis error, but a pre-processing one. Are you sure you defined your properties right? If possible, can you upload the .inp file which gives this error.

Concerning contact, you have many options. Most involve a trade-off between convergence and surface pressure/stress.
If you are not really interested in exact contact output, you can think of using penalty contact to make convergence easier.
In your specific case, it might help to, along with surface to contact, define "edge to surface" contact for those edges at the side of your wall.

Relevant things in manual:
benchmark manual: 1.1.11 The Hertz contact problem
user manual: 38.1 Resolving contact difficulties in Abaqus/Standard

 

[IRSHADQUR]

Thx alot for replying.

U can find the .inp file from the link given below

http://www.filedropper.com/6march

In this file i just placed the PT strand inside the wall and foundation without providing any interaction between wall and PT. However i also tried to make holes in the wall and providing PT tendon inside and providing contact behavior between wall and PT. But by both techniques it gives the same error. (Missing property definitions)
Thx alot again for reply.

 

[burningDiesel]

In the input file you sent, you didn't assign truss properties?
See attachment, I did nothing more than assign truss properties (in part) and changed mesh to T3D2.
Simulation runs, with negative eigenvalues in prestress step & first step of loading. This does not have to be a problem, but it's not good either. Doublecheck your boundary conditions, negative eigenvalues disappear after contact has been made, so again, it is not a problem per sé.

 

[IRSHADQUR]

Thx alot Dear Sdebock.

Yes its working fine now. I just have one more question.

My PT steel is supposed to remain elastic during my loading history. But an initial post-tensioning has to be applied in the model.
I have searched through abaqus forums and i found out that Initial conditions cant be specified in CAE and i need to apply initial stress by some other ways which could not understand (I am just a beginner in abaqus). Now what i have done is that since my PT will remain elastic so i just applied a vertical force over the wall equal to pre-stressing force and did not give any prestressing in bar. Do u think this technique can be used effectively in my problem if not kindly can u explain me that how can i apply pre-stressing or give me some link where it has been explained.

Thx for ur time

 

[burningDiesel]

First try to edit the keywords. The .inp file you uploaded is just a selection of keywords and data, written by the CAE.

use *INITIAL CONDITIONS, TYPE=STRESS to specify initial conditions. Check the keyword manual for correct format etc.
Read the section in the user manual on 33.2.1 Initial conditions in Abaqus/Standard and Abaqus/Explicit

As a workaround, you can use change in temperature to prestress your material.

 

[IRSHADQUR]

ok i will try it and will let u know if i feel any other problem
Thx again

 

[IRSHADQUR]

Hello

I am trying to apply the initial conditions for my Post-tensioning steel. As you referred me to see the user manual for applying initial stress, all i can find in that is

" Initial values of stress can also be defined for rebars within elements (see “Defining rebar as an element property,” Section 2.2.4).

Input File Usage:
*INITIAL CONDITIONS, TYPE=STRESS, REBAR

Abaqus/CAE Usage: Initial stress is not supported in Abaqus/CAE."

It does not tells us that how to select the elements and how to specify the stress value. Plz kindly help me out to apply this condition. Actually i am just a beginner in abaqus so i just have some basic questions. I found my input file in the temp folder which i sent to u. Do i need to change that file to apply initial conditions. After applying these conditions can i run this file in CAE?. You have my input file so i would really appreciate it if u write the required lines with some assumed values in the file as the input file looks very confusing to me because i am just working on CAE.

Thx alot

 

[burningDiesel]

You can do it from CAE
predefined field -> create predefined field -> stress

or in the keyword input file, put
*Initial Conditions, type=STRESS
"PT Steel-1".PT, 50., 0., 0.,
before the first step.

 

[IRSHADQUR]

Dear Sdebock
I am using abaqus 6.10 and when i go to create predefined field it does not give option for stress. Do i need to install some latest version to use this option in CAE. Secondly if i input the initial conditions in .inp file then how to run it. Do i have to import this file in CAE as a model and run the analysis or i have to do it some other way to run the analysis. (My questions might be stupid but bear with me as i am just a beginner in abaqus)
Thx alot

 

[burningDiesel]

Could be it wasn't implemented in 6.10.
You can run it by (in manual 3.2.2 Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution)

abaqus job=jobname

in terminal (linux) or cmd (windows) from the same location your jobname.inp is.

 

[IRSHADQUR]

Hello Sdebock
I have installed Abaqus 6.12 and now i am able to apply initial stress and everything is working fine thx to your support.
Now i have another thing to do and again i need your help in this. I want to apply earthquake excitation to my structure but i dont know how to do it.
So could u kindly guide me in this regard also.
Thx alot and regards
Irshad

 

[burningDiesel]

I guess you should look into your regions building code to see what accelerations and/or displacements you have to apply to the base of your structure.
Possibly this involvs a modal analysis (eigenfrequency extraction) and a response spectrum, with displacement/acceleration for different frequencies.
Or, do a dynamic analysis.

Anyway, never done it, so can't really help you.

 

[IRSHADQUR]

Dear Sdebock
Actually I have the excitation to be applied on the structure in terms of acceleration time history. From the manuals i came to know that i have to apply acceleration on the base nodes as a Boundary condition. The value of acceleration will be 'g' and i will change the amplitude of this acceleration in very small intervals of time. This amplitude has to be in an external file and it will be like
Time Amplitude
0.00 0.00
0.01 0.1 (means 0.1g)
0.02 0.15
0.03 -0.05 (there will be thousand values of a 10 sec time history)
So i know that it will be done in this way. All i want to know is that how can i attach an external file with my abaqus CAE for amplitude. What should be the file format and how abaqus will call that file during dynamic analysis.
Thx alot again for ur consideration and time

 

[burningDiesel]

oh, that's easy.

You can either do:

In CAE:
Abaqus/CAE Usage:

Load or Interaction module: Create Amplitude: any type: click mouse button 3 (in my case it was right click though) while holding the cursor over the data table, and select Read from File.

or in input file:
*AMPLITUDE, NAME=name, INPUT=file_name

But I guess you haven't managed to work with the input file yet.

 

[IRSHADQUR]

Thx alot man. Its working.

 

[IRSHADQUR]

Dear Sdebock

Now i am able to model the rocking wall correctly for quasi-static loading. Now my next step is to apply earthquake excitation to this structure.
Since my model involves contact and high frequency phenomenon so i figured that abaqus implicit cant handle this problem. So now i started to work on abaqus explicit but i am facing some problem and need your guidance.
I need to apply prestress and gravity load on the wall and have to keep it constant in the next steps but when i apply self weight and prestress it tends to increase and decrease like a sine wave and does not remain constant. Similarly EQ excitation is giving weird results. Would u guide me in this regard that how to stable the system.

Thanks and regards

 

[burningDiesel]

Things that might help to remove unwanted oscillations:
- recheck all units
- applying the load using a "smooth step" amplitude
- increase the time of loading

for the EQ excitation, you can only recheck your units. If they are correct, I guess it's a matter of finding the correct damping, which is always a tricky thing to do. Also, what are the 'wierd' results?

About stability, the explicit calculations are stable by design. What you might get though, is aliasing in the output.

 

[IRSHADQUR]

Dear Sdebock
I am getting these error messages in my explicit analysis.

"The option *boundary,type=displacement has been used; check status file between steps for warnings on any jumps prescribed across the steps in displacement values of translational dof. For rotational dof make sure that there are no such jumps. All jumps in displacements across steps are ignored

The rigid bodies with refernce nodes in node set WarnNodeRefNodeNoMass have extremely small mass. It is recommended that the analysis be run in double precision."

I have checked the units, used the smooth type amplitude and increased the type of loading but still when i apply gravity loading the reaction forces varies in a sine wave form. Kindly suggest me some way to fix it. Is it possible for you to take a look of the CAE file and suggest me some way to fix this.

Thanks and regards