Hi Matthias

I have never exported the mass/stiffness matrices myself but I believe you can output the data using OUTPUT4. 

I suggest that you skip Matlab and use instead Python and PyNastran where an OUTPUT4 reader already is in place, 

For your constrained dofs - take a look at param, autospc  and turn it off. You then will not be able to run the model but, it should not constrain your dofs any longer. 

Also, have you seen that Nastran 95 now is OpenSource on Github?

https://github.com/nasa/NASTRAN-95 

http://mycosim.com/products/

This release does not have SOL103 and newer solvers but, it is still quite competent and something to consider, e.g. when you want to run massively parallell. 

And, for the more ordinary analysis types, there is MyStran

https://github.com/SteveDoyle2/MYSTRAN 

Last, if you are dead set on Matlab - take a look at CoFE

https://github.com/vtpasquale/NASTRAN_CoFE 

Hope this helps

Claes

in static state:

1- fix all nodes

2- put a unit displacement in ith degree of freedom

3- The output force vector is the ith column of the stiffness matrix

4- do it for all the degrees of freedom to extract the stiffness matrix

then use modal analysis and find all modes

having all modes and the frequency of each mode and stiffness matrix you can find mass matrix

Hi

True, you can get data this way, but the suggested procedure is a workaround. 

Here is a simple way to dump the data into a Punch file

PARAM,EXTOUT,DMIGPCH 

http://mscnastrannovice.blogspot.se/2013/04/how-to-output-stiffness-and-load.html 

If you want load information also, use

param,extout,dmigpch 

https://community.plm.automation.siemens.com/t5/3D-Simulation-Femap-Forum/The-stiffness-matrix-from-Femap/td-p/246917

Here a way to dump the matrix data into OUTPUT4

http://support.sdtools.com/gf/project/support/forum/?action=ForumBrowse&forum_id=22&_forum_action=ForumMessageBrowse&thread_id=192

And here is a way to dump it into the F06 file and read it into Python

http://scicomp.stackexchange.com/questions/7171/finite-element-nastran-dmap-how-to-print-the-differential-stiffness-matrix-in

You might want to take a look also how to create Craig Bampton 'static modes'?

https://femci.gsfc.nasa.gov/craig_bampton/

I wish I had known the above a long time ago. :)

Have fun

/Claes

Hello,

To obtain mass and stiffness matrix for all nodes ,

1. Delete the SPC card from .bdf or .dat

2. Use PARAM,EXTOUT,DMIGPCH inside begin bulk section.

3. Solve using MSC NASTRAN

This will print the entire Mass and stiffness matrix in .pch file.

My research is also in similar line. I was trying to read the Mass and stiffness matrix from .pch file using MATLAB. But I am having difficulty in coding this. Can anyone help me with this?

I read the .pch file using textscan function in matlab but i could not process this cell array into a matrix. More information on the difficulty i am facing with code generation is attached for clarity.

Any help will be appreciated.

Thank You,

Paul

Hi Paul

An explanation of the dmigpch can be found in this document

http://www.ae.metu.edu.tr/~ae464/Format%20of%20the%20Stiffness%20matrix%20and%20load%20vector%20output%20in%20Nastran%20pch%20file.doc

I ended up plotting the matrices to .op4 and reading in the FORTRAN binary code using c++ code.

My best regards

Matthias

Hello Matthias Faes,

Why the extracted stiffness matrix using the above procedure is always singular? I have plotted the stiffness matrix into punch file(.pch) and read using python code but the extracted stiffness matrix is always singular. I tried with different Finite element model but gives me a singular stiffness matrix.

I need to do some mathematical operation like inverse of this stiffness matrix. Could you please help me with this?

Attached is my FEM details.

Thank You,

Paul

Hi Paul

This is logical since your model is not constrained.

If you are sure that you don't want to add constraints to your model, you could always try to solve a slightly shifted problem (i.e. add a very small diagonal matrix to your stiffness matrix and solve that one). That's what I do for computing the eigenvectors; you'll have to work out the accuracy for the inverse of your problem yourself.

You can always contact me for more information :).

Hope this helps,

Matthias

Hello Matthias,

Thank You. It worked great.

Could you provide the reference for the small diagonal matrix addition in order to make the stiffness or mass matrix non singular?

Regards,

Paul Thomas

Hi,

I would like to export and process the matrices (e.g. model order reduction) and then import the resulting state space system back to into nastran. Has anyone done it yet? Will I need a dummy mesh? Would using a superelement help me in any way?

Best,

Thomas

Check the code I developed earlier for one project,

https://github.com/PAAW/mAEWing1/tree/master/Design/FEM/readNastranKM

Hope it works for you. Then you can remove some columns and rows based on your SPCs.

Paul Thomas and Matthias Faes , If I remove SPC card it means the structure is free-free and I can get M and K matrices for a free model. what should I do for a clamped-free model?

Kianoosh Mohammadi you'll have to figure out which DOFs are constrained in your model, where they are located in your matrices and remove those manually.

Hi,

Here is the simple C++ converter from '.pch' and '.dat' files: https://github.com/Qinterfly/PchConverter. The input files are converted into sparse structural matrices (stiffness, mass, damping), a mapping matrix and nodes coordinates. Hope it may be useful for someone.

Pavel Lakiza thank you for the script, it helped me a lot !!

I have two short questions:

1. Can your C++ script be used in Python somehow ? Can your finished script be transferred to Python ?

2. I tried to translate a larger pch.file with your script, but above a certain matrix dimension error messages appear. Unfortunately I don't know C++, so the question is: can your script be used to translate matrices with several millions ? And how long would the translation take ?

Many thanks in advance.

St Mr

1) The algorithm is quite simple, so it would not take a lot of effort to implement it in Python. However, it might work kinda slow with large files in that case.

2) I am positive that the program can be fixed so as to avoid having the mistake which you have got. Could you send me that file? I will try to find out what is wrong with it.

Dear Matthias Faes

I need to extract the stiffness and mass matrices from reduced order model in MSC Nastran. I have chosen 6 boundary nodes on the model in the free free case. I have performed the analysis and I have used "EXTSEOUT(STIF,MASS,ASMBULK,EXTBULK,EXTID=3,matop4=43)" to generate the .op4 file.

I tried with the .pch file, but since the order of the matrix is very big, I find it difficult to extract the matrices in the correct order.

Can you please tell me how to generate a code in Matlab to obtain the matrices in .csv format, so that I could use the matrices in Matlab and perform other operations.

Thanks in advance.

Goutham Sajja