Hi Samuel,

I guess you can not print global stiffness matrices. But you can use 

*output option (check documentation, both mass and stiffness matrices 

could be outputed) to save all the element stiffness matrices to .mtx 

file. So you can assemble them and add loading & boundary offline. 

You can pretty much do this. There are two ways that I am aware of 

1. Use *element matrix output 

2. Use substructure (see below) 

*STEP 

*SUBSTRUCTURE GENERATE, TYPE=Z0002 

*SUBSTRUCTURE MATRIX OUTPUT,FILE NAME=outputfilename, STIFFNESS=YES 

*RETAINED NODAL DOFS 

 outputNSET, 

*END STEP 

You need to create outputNSET; Read manual for each card defintion and 

more options and understanding. 

Good Luck! 

It's possible to output the global matrices - I do it by creating the MATRIX GENERATE step in the inp file as follows:

*STEP, name=whatever

*MATRIX GENERATE, MASS, STIFFNESS

*MATRIX OUTPUT, MASS, STIFFNESS, FORMAT=MATRIX INPUT

*END STEP

Hope this helps

Check the Last FIVE LINES of the file i attached.

https://www.youtube.com/watch?v=LxTzYAkUkNA

Hi,

I tried your introduction but when I imported an inp. file added, the program warned as below, How can the problem be fixed? Thank you!

WARNING: The following keywords/parameters are not yet supported by the input file reader:

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

*MATRIXGENERATE

*MATRIXOUTPUT

Quy Thue Nguyen

Please use:

*MATRIX GENERATE

*MATRIX OUTPUT

Best,

Victor

Hello Victor Flores Terrazas,

I used the above-mentioned method to generate mass and stiffness matrices. For cross verification, I just added all the elements for the mass matrix but found that the sum is not matching with the mass that is being shown in Abaqus.

I verified analytically using density*volume formula, and obtained the results same as Abaqus one, but not the one from the matrix.

Can you please, help me with this aspect?

Thank you,

Dheeraj Kulkarni add only diagonal elements of Mass matrix.

Hi

Thank you for your response. Sorry, i didn't specify, but i got diagonal matrix. So, I added only diagonal elements. But I'm unable to get it

Dheeraj Kulkarni , how much different from each other are those computations?

Victor Flores Terrazas, the difference is huge. Like some 2-3 times in some cases, and 4 to 6 times in some other cases. I tried the same for different varieties of problems. But, the answers are different.

I'm attaching obtained mass matrix and input file.

Thank you

Dheeraj Kulkarni I am not quite sure what the problem might be, as I am not an expert in the subject. What I can tell you, though, is that I have had problems with structural matrices generated by Abaqus for beam elements, where I got negative values for the node numbers. Have you tried using a different type of element, just to make sure?

Hi Victor Flores,

Actually I was getting mass and stiffness matrices without boundary conditions. So, when i applied BCs to the stiffness and mass matrix, then I obtained the exact results.

Thank you for your kind response.

Dheeraj Kulkarni Good to hear. Just from experience from my own model, if you want to perform modal analysis with the matrices extracted from Abaqus, the only way I got the same natural frequencies in Matlab and Abaqus is by extracting the matrices WITHOUT the BC's and enforcing them in Matlab manually.

All the best.

Hello everyone,

I am having trouble in using the extracted stiffness matrix. I am doing modal analysis so I wanted to cross check the eigenvalues I found in abaqus and the extracted stiffness and mass matrix and using 'eig' in matlab. But the problem is even though I arrange the stiffness and mass matrix I don't get same result.

Kadidja mohamed Barkat have you tried my suggestion of extracting the matrices without boundary conditions and enforcing the boundary conditions in Matlab before your modal analysis?

Kadidja mohamed Barkat what format did you use for the matrices? How did you arrange in matlab? I am also trying to verify my results.

Hello Victor,

I saw your above responses and hence asking you this question.

I am trying to extract the stiffness matrix of a loaded structure (after the static general step has been performed) WITHOUT boundary conditions. I can extract the stiffness matrix with boundary conditions but I want to extract it without Boundary conditions. I need to match the results from the Frequency analysis where I removed the boundary conditions with the results from this K matrix (without BC). Please let me know if you have any thoughts.

Thanks in advance.

Hi Nidish,

The way I did this was to insert the matrix extraction step in the INP file, BEFORE the Modal Analysis step. I have also performed a static load case analysis, but this I did separately from the modal analysis.

The extracted structural matrices will have no boundary conditions, as they will be applied during the Modal Analysis (frequency) step in abaqus. You can then apply the boundary conditions to these "unbounded" matrices in what I assume is a numerical simulation program such as Matlab, or just perform a modal analysis with the unbounded matrices, as you see fit.

Hope that helps.

Hello Victor,

Thanks for the prompt reply.

I understand what you are saying. But I need stiffness matrix of a deformed geometry (without BC) rather an undeformed one. I ran static general step after which I got some deformed shape. I need to find stiffness matrix of this new deformed shape.

I hope this clears my question.

Hello Victor,

I can add this after the static general step in the input file.

** ----------------------------------------------------------------

** Output Global Stiffness Matrix

*Step, name=Global_Stiffness_Matrix

*MATRIX GENERATE, STIFFNESS, MASS

*MATRIX OUTPUT, STIFFNESS, MASS, FORMAT=COORDINATE

*End Step

** ----------------------------------------------------------------

But it will give me a stiffness matrix with boundary conditions. I want a global stiffness matrix without boundary conditions. Like the way, we do frequency analysis (by removing BC in this step) after performing static general analysis.

Hi Nidish,

I understand your question now. I have not tried to do this, and I would *think* that you might want to try then inserting the matrix extraction code as a step after the loading case step. Although in this case, I believe that the boundary conditions will carry over to the next step.

Are you performing non-linear analyses? Otherwise, I would think that the direct stiffness method is used in Abaqus for static load cases, in which case I don't think the stiffness nor mass matrices will change after deflection under loading (also assuming an LTI system).

rgrds

Hello Victor,

Yes I am performing nonlinear analysis. In Abaqus documentation it says that you can modify BC in matrix generation step. So I am adding this line in the inp file. *Boundary, OP=NEW (to remove BC). But the simulation does not run.

Regards,