Unloading in Riks 1

[Shahrukh_Islam]

Hi everyone,

I am trying to analyse a beam by loading it to a certain point using a displacement controlled parameter. In this case I need to know the postbuckling behaviour, so I am using Static Riks. My question is how to unload after a certain point during the application of displacement? Firstly, is it even possible using Riks? Secondly, if it is not possible, then how can I extract the final state data from the results and then input it to create a new model and then unload it?

I really would appreciate the help.

Thanks in Advance!

 

[FEA way]

You can use the restart functionality to add non-Riks step with unloading. This approach is described in the documentation chapter "Unstable Collapse and Postbuckling Analysis", paragraph "Obtaining a Solution at a Particular Load or Displacement Value".

 

[Shahrukh_Islam]

But Riks doesn't allow a step to be added after it has been added. How can I do it? Is there a procedure to do it using scripting? If so, what's the process?

 

[FEA way]

It doesn’t matter for restart. It’s a separate analysis, just continuing from where Riks finished. Check its description in the documentation.

 

[Shahrukh_Islam]

So, there is one issue now. I am trying to do another Riks to unload it but it is not working. How can I do the unload from the previous Riks analysis? I could get the restart out but no step can be added after the Riks? Could you help me out? I am getting this error message!

 

[FEA way]

The second step, added in restart analysis, should be non-Riks step (like general static) to simulate unloading.

 

[Shahrukh_Islam]

Thanks for the advice. I had another question. The CAE interface does not allow me to add another step in the steps menu. So, how can I do it? Does it have to be through scripting?

 

[FEA way]

You can do it outside of Abaqus/CAE, using a new input deck for the second analysis. For example:

*RESTART, READ
*STEP, NAME=UNLOADING, NLGEOM=YES
*STATIC
...
*CLOAD, OP=NEW
...
*END STEP

 

[Shahrukh_Islam]

Do you have a process or a thread or an example? That would be really appreciated. Another thing, so, do I do it using text editor and what files do I modify or alter to do this?

Thanks again for all the help

 

[FEA way]

Any text editor will be fine. You can paste this template and adjust it to your case. Keyword syntax is covered in the Keywords documentation guide.

 

[Shahrukh_Islam]

Which file should I edit?

 

[FEA way]

Create a new file with .inp extension, paste that syntax, modify it accordingly and run the analysis from the command line:

abaqus job=first_job_name oldjob=second_job_name

 

[Shahrukh_Islam]

I am sorry again. But do you have a specific guide to do this step by step? I am new to this process. How do I create the file? Is it using just text editor?

I have tried making a file with the following:

*Restart, read, step=last
**
** STEP: Unloading
*Step, name=Unloading, nlgeom=YES, inc=100
*Static
** BOUNDARY CONDITIONS from Step-1 remain
*Boundary
Set-9, 1, 1
Set-10, 1, 1
Set-10, 2, 2
Set-10, 3, 3
Set-11, 1, 1
Set-11, 6, 6
Set-12, 1, 1
Set-12, 2, 2
Set-12, 3, 3
Set-12, 5, 5
Set-12, 6, 6
Set-14, 1, 1
** Reverse the displacement for unloading in Set-16
Set-16, 2, 2, -1.5
**
** OUTPUT REQUESTS
*Restart, write, number interval=1
*Output, field, variable=PRESELECT
*Output, history, variable=PRESELECT
*End Step

This is the original file:

** ----------------------------------------------------------------
*Imperfection,
file=me8_eig, step=1
2, -0.058
**
** STEP: Step-1
**
*Step, name=Step-1, nlgeom=YES, inc=1000
*Static, riks
0.01, 1., 1e-05, 0.1, , Set-11, 2, 1.005
**
** BOUNDARY CONDITIONS
**
** Name: BC-1 Type: Displacement/Rotation
*Boundary, op=NEW
Set-9, 1, 1
** Name: BC-2 Type: Displacement/Rotation
*Boundary, op=NEW
Set-10, 1, 1
Set-10, 2, 2
Set-10, 3, 3
** Name: BC-3 Type: Displacement/Rotation
*Boundary, op=NEW
Set-11, 1, 1
Set-11, 6, 6
** Name: BC-4 Type: Displacement/Rotation
*Boundary, op=NEW
Set-12, 1, 1
Set-12, 2, 2
Set-12, 3, 3
Set-12, 5, 5
Set-12, 6, 6
** Name: BC-5 Type: Displacement/Rotation
*Boundary, op=NEW
Set-14, 1, 1
** Name: BC-6 Type: Displacement/Rotation
*Boundary, op=NEW
Set-16, 2, 2, 1.5
**
** OUTPUT REQUESTS
**
*Restart, write, overlay, frequency=1
**
** FIELD OUTPUT: F-Output-1
**
*Output, field
*Node Output, variable=PRESELECT
*Element Output, directions=YES, variable=PRESELECT
1, 2, 3, 4, 5
**
** HISTORY OUTPUT: H-Output-1
**
*Output, history, variable=PRESELECT
*End Step


Do you think my commands are wrong?

I used this command : abaqus job=Riks_unload oldjob=Riks_4 input=Riks_post.inp

But it says I have syntax error