hello every one
i m working on delamination buckling analysis in abaqus 6.14...
now i want to add geometric imperfection in my model while i m using general static step for buckling analysis ,,,
can any one help me how i can add geometric imperfection in my model
i don't perform eigen value analysis because i dont need different modes and their buckling load..
i just apply axial displacemnt on two parts joined by cohesive element with delamination between them....but now i want to add imperfection to it too..i have studied in the abaqus documentation how to add imperfection but that require eigen value analysis,,which i dont want
i just need to know if there is any other way to add imperfection to my model since i m using general static step..
thank u
best regards
Hello,
what kind of defects do you want to apply ? geometrical, material ?
what do you want to model ?
best regards
Baranger, E., Guidault, P. A., & Cluzel, C. (2011). Numerical modeling of the geometrical defects of an origami-like sandwich core. Composite Structures, 93(10), 2504-2510.
I assume you may have some known geometric imperfection, which could be explicitly expressed for each node point of the Finite Element model.
In this case, I think you can modify the keyword input file directly!
That means, you can add the nodal geometry imperfection to the node coordinates of the perfect structure geometry model.
thank u sir Emmanuel Baranger for ur response
i want to add geometric imperfection factor .05 , .5 into my model ..
i want to model delamination buckling in composite shell with cutouts using cohesive elements,,,now beside cutouts i also want to add some geometric imperfection in to my model.. i would be glad if u could tell me how to do it,,,i can not/dont want to use that method of calling of result file from another model..
thank u
best regards
may be I am wrong but I think you have to move your nodes either by using a python script either directly in the inp file.
best regards
thank u for ur response Yining Lv
can u elaborate how will i do that
it would be great
thank u
the simplest way to do is to generate the inp file and then to modify the table of the points coordinates using a script (python, matlab...).
regards
I think you can do an independent calculation for each initial imperfection case. For each case, you can follow the procedure below:
(1)in your prepared .inp text file, find the *node part and copy this part into an Excel spreadsheet.
(2)for each node, you have initial imperfection of a prescribed factor;
(3) add this imperfection to the coordinates of *Node segment manually in the Excel spreadsheet.
(4) copy this updated *node segment to revise the original .inp file.
Now, it'll be ok to run this .inp file.
Actually this is the same procedure as the last shown by Emmanuel Baranger with only one sentence.
Hope this can be some help for you!
Babak Keykhosro Kiani · 2.50 · International Institute of Earthquake Engineering and Seismology
its not necessary for eigenvalue buckling analysis and your main analysis to have same BCs or applied loads or even shell thicknesses.
How do I include geometric imperfection in a model? - ResearchGate. Available from: https://www.researchgate.net/post/How_do_I_include_geometric_imperfection_in_a_model [accessed Jul 27, 2016]..............
more please?
Hi there,
I know this post is a bit dated, but for anyone still looking at it, there are 2 ways that I found to add an imperfection. They have different levels of effectiveness
Method #1:
Apply a imperfection directly to your geometry. I did this via a python script and this worked fairly well. However, it is very hard to get convergence past the point of buckling unless damping or a very "nice" mesh is used. This doesn't mean a high element count, but potentially using non-linear geometry mode (activated in step dialog box) and a quadratic mesh instead of a linear one.
Method #2:
Apply imperfection using *IMPERFECTION keyword directly in your input file. This requires that you have the eigenvalue buckling analysis completed for the same mesh, and you have the FIL file from that previous analysis (requires you to add another 2 lines near the end of your eigenvalue buckling analysis input file). I only realized the part about the FIL part later and I don't know how to get that extracted without redoing the analysis again.
I used Method #1 with elastic buckling analysis and #2 for plastic/inelastic buckling analysis. I would recommend #2 so long as you get it working for your case.
Hope this helps some people!
:) :D
Hi Bharat Bhaga can you please elaborate more?
I am designing a cold-formed steel beam, modeled as SHELL element. So, how can I include geometric imperfection in the case?
Thank you in advance.
Regards,
Dheeraj
I have created here a youtube channel with many different ABAQUS-tutorials videos on shell buckling:
https://www.youtube.com/channel/UCU3dmUB40wf5RCEGp9UMtbA/videos
Dear Ronald Heinz Norbert Wagner,
Do you know any ways that we can create a general static step after static, riks step in Abaqus?
and Can we use the *Imperfection command for static, general step ?
Best regards,
Dear Sir,
If we have 2 steps in a job, the first step is a static, general analysis and the second is static, Riks. so how can we apply the imperfection for only the second step in this job? Thank you for your help!
Dear Eko Charnius Ilman,
Could you tell me how to read and modify the node coordinate by using Python or do you have any simple example can share with me, please?
Thanks!
For those looking to input imperfection directly to node/s of mesh BEAM element via Python. Below is how you can do it using Python. As you can tell, this is the code output from the .jnl file. You just need to modify it accordingly and stick it into your script. Here myColNode_Mid is the imperfection I want for the node located at the middle of my mesh. Please take note, when I say node I meant the node of the meshed element (i.e in the *Mesh module), not the node you see in your *Part/*Assembly modules. For my case, I just need these few lines of code to add imperfection to all the columns in the model as all the column instances were added as an independent instance (i.e. link to the original column in *Part module.)
myColNode_Mid = mdb.models[myModel].rootAssembly.instances[myModule+'_'+myColName+'-1'].nodes.getClosest( coordinates=(((0, 0.5*float(modHeight), 0)),)) mdb.models[myModel].rootAssembly.editNode(nodes= myColNode_Mid, offset1=-500) mdb.models[myModel].rootAssembly.regenerate()
- Badges
- Science topic