Dear João Alfredo De Lazzari ,

I have used ANSYS to solve many problems with imperfections in RC & Steel structures. My PhD involves new imperfection procedure as introduced in

Article Imperfection Modeling Using Finite Element Approach with Par...

However, my cases are slightly different than yours. I know the initial imperfections before building the model. I mean, the imperfections are input and not ANSYS result as in your case.

For your case, I suggest the following

1- Make two files: File1 for the elastic buckling to get required two modes and File2 for the nonlinear analysis (Arc length) on the imperfect structure

2-Build and Run File1

2-Write & execute code (in Ansys... file ... read input from file) to sum the displacements of the two considered modes of File1. It is very easy ... You need to read slowly in the ANSYS help .... write the code and make the code creates a txt file on your PC containing the node number and its displacements. Say, you will name the result file Odis2M.txt for exmaple

Now, you are similar to my case... You know the input imperfections !

3-Build File2 provided that the nodes have the same ID(s) in both File1 & File2 (use save as when start building File2 and do not change in the geometry)

4-Write another code to apply the displacements written in the file Odis2M.txt on the nodes of model of File2. This code will re-draw every node after changing its coordinates with the new data that is read from the file Odis2M.txt. You will use the commands

"MODMSH, DETACH "

"Do" loop for the nodes (say I loop)

changing (redrawing) the nodes using the new coordinates by reading them first from Odis2M.txt and applying them on File2 model using the command "N"

N, I, newXcoord, newYcoord, newZcoord

5-execute your imperfection code (in Ansys... file ... read input from file) or copy and paste it in the command bar

6-Congratulations! Run File2 for your target nonlinear analysis

Hint:

A-Try to build the attached simple example to apply imperfections on a plate (attachment: Imperfections Ex. Numcmp - deatch - N commads & example.pdf)

B-Try to read and practice the examples found in Chapter 10 of the book "The Finite Element Method and Applications in Engineering Using ANSYS" in order to learn how to write small easy codes for similar prolems

Additional information..

What is about the available data (either industrial, experimental, ....etc) on the imperfection shape of your problem..

You may skip the elastic buckling step ... and apply the imperfections (based on the available data) on your nonlinear model.

--------------

Also,

In my opinion, I think that the random imperfection procedure is the correct choice because it does not enforce the model towards certain deformation. Please check the random imperfection procedure in

Article Imperfection Modeling Using Finite Element Approach with Par...

Thank you so much Ahmed M. El-Kholy .

Right now I don't have available data to compare. But in the future I will make some lab experiment. But from what has on the articles I have seen, they have done some numerical modelling on this case, and I can expect what shape I want.

As you said, I came up with the idea of skipping the elastic buckling step on ANSYS, instead, I run a Finite Strip Method (on MATLAB) as pre-analysis, and from there, I can get the deformed shape in different modes. So, I sum the modes I want, and I generate an APDL with KEYPOINTS that has the coordinates of the deformed shape. In this case, I have to discretize points on each section and along the longitudinal length of the structural element. By then, I am able to put the imperfections I want, just like the similar case you have.

The only problem I am having now, It is how to generate the areas to connect the KEYPOINTS, since with the deformed shape, the areas are not planned when you connect 4 points. For this case, I am using SHELL281 (I was using SHELL181 before), and forming my areas with triangular shapes (3 points). In this case, using quadratic elements it might form some triangular elements, and the SHELL281 is a better option of SHELL when use triangular element. My dilemma now is which type of SHELL should I use, since people that have done research on this particular structural element, have been always used SHELL181.

Ahmed M. El-Kholy I would like your opinion about the idea of getting the imperfections from my pre-analysis, Finite Strip Method, and inserting as KEYPOINTS on ANSYS.

The random imperfection procedure might be a interesting idea for my problem. I will talk to people on my lab, and see what they tell about about it. Maybe, the random imperfection can be applied more specific for my case, because the structural element I am working with come from a industrial production, where the imperfections come from. Cold Formed Steel Lipped Channel can be manufactured by folding and continuous procedure. Probably on the folding is where it gets more imperfections.

Thank you so far.

Thank you

Please build the ideal model completely including the shells without any imperfections

Then

Write the code to move the nodes NOT the keypoints to the new imperfect coordinates

Then

Execute the code

You will find that

The ANSYS modify the shells because they are connected with the Joints (nodes not keypoints)... Just move the nodes using N commad

I hope that you find it useful

Best wishes

Thanks, it is very useful!

Should I use NMODIF, NODE, X, Y, Z, THXY, THYZ, THZX , instead of the command N to move an existing node?

hi i am doing a similiar work as to you can you share your solution with me and tell how you put imperfections in the non linear analysis

Dear S Prasanna Swasthik Saxena ,

Unfortunately I came up with a different solution. I programmed my own elastic buckling analysis using the Finite Strip Method, in a MATLAB code, and with that, I have the freedom to sum up the buckling modes I want. In the end, I insert the two buckling modes as initial geometric imperfections, with KEYPOINTS.

However, according to Ahmed M. El-Kholy, updating the perfect structure with KEYPOINTS is not recommended. He said that it is better update the nodes, with the command N.

If you want to inset an initial geometric imperfection from a single elastic buckling analysis, it is not that hard. You have just to perform the buckling analysis before, and update the current perfect column, with the buckling mode from the buckling analysis. If you want, I can share with you an APDL I have, so you have an Idea of what I am saying.

Best regards

Joao Alfredo De Lazzari

yes please can you do that it will help me

thanks for your help have you also used inistate command before in your work do you know how to use the inistate commands

João Alfredo De Lazzari I am also trying to include initial geometric imperfection in my cold-formed steel beams. But I am struggling how to get the two buckling modes and update my model?

can you please share your APDL or advise me how to do it. Thank you

@ dheeraj karki

@ Dheeraj Karki

https://www.researchgate.net/publication/339363721_Finite_Element_Simulation_for_Steel_Tubular_Members_Strengthened_with_FRP_under_Compression