How to extract Forces and Moment from Solid Tet Mesh Model in ABAQUS?

[tp701]

Hello,

I have one solid Y shape type structure model which i have modeled as assuming beam model in NASTRAN. From NASTRAN i am extracting internal loads (Nodal forces and Nodal Moments) successfully and then i am doing the strength analysis of particular section by using internal loads. Now i have model the same structure using 3D solid finite element model by assuming Tet Mesh under ABAQUS. Analysis was running perfectly in ABAQUS. Now my problem is how to extract the internal loads from the 3D solid Tet mesh model for the same section. I need help to extract the internal loads from the solid Tet mesh. Please help me i am right now stuck at this point.

Thanks in advance,

TP

 

[truckcab]

Hi,
there is an Abaqus keyword which allows you to do exactly what you are asking for. Check the *SECTION FORCE keyword in the documentation, it is quite straight forward to use this feature. I am not at work right now so I cannot give you the syntax. I remember that you need to define a surface at the section where you want the forces... just check the keyword *SECTION FORCE, you can then quite easily solve the problem.

 

[tp701]

Thanks truckcab,

I will look at that aspect.

Thanks again,

Tarun

 

[truckcab]

tp701,
my memory failed me. The keyword is *SECTION PRINT and it is quite straight forward to use.

 

[tp701]

hi truckcab,

i have look at *SECTION PRINT. It is very usful option to get internal forces anad moments. However,i have still few doubts because it has certain limitation such as section has to cut through element faces or edges but my section cuts through 10 noded tet element.

I have few doubts about relation with shape function. Is it possible to find stress in tet element for perticular point using shape function.

Thanks,

Tarun

 

[truckcab]

Hi Tarun,
I am not really sure hoe your model looks like so this might not be possible: What i should do is trying to fix the mesh in the sections where you want to compute the forces so that you can define a fairly good face there using the element faces. Depending on how your mesh looks like you might need to be rough and maybe distort the elements a bit. But since you are interested in forces and not stresses it might not play any significant role. That is waht i should do. As far as i know there is no way to automaticallt compute section forces cutting through the sides of an element in abaqus. If you want that you might need to resort to some programming yourself.

 

[tp701]

Hi Truckcab,

Thanks for your reply,

I think i should try to fix the mesh in that section.

Thanks again,

Tarun

 

[tp701]

Hi truckcab,

It is very difficult to fix the mesh on perticular section solid part because i have complex solid part. Please provide some suggestions.

I am also woundering you mention some sort of programming i have to do. It would be nice if could you explain me in detail.

Thanks,
Tarun

 

[truckcab]

Hi Taurun,
if it is not possible to make a nice and clean cut through your structure at the location where you want to know the section force then you can:

1. Do the best cut you can through the tetra mesh at the interesting location.

2. Define an element based surface on the tetra facets facing the cut (*ELEMENT, TYPE=ELEMENT etc... its all in the manual).

3. Define a local coordinate system corresponding to the Nastran system you have in your previous Nastran run) or any other system that you think is good (use *TRANSFORM), when you use *SECTION PRINT it is possible to receive section forces in that very coordinate system. It is also possible to receive the forces in an updated coordinate system i.e. if you have large deflection your local coordinate system must be updated accordingly in order to receive the proper section forces.

This is how I would do if its not possible to get a clean and tidy cut through the section.

Actually, problems receiving section forces is one drawback with solid element models.

I do, however, believe the *SECTION PRINT approach I describe will result in feasible section forces. Of course... I do not know anything about you physical application.


The programming I mentioned was to resort to the old fashioned way the elderly like me had to do in the middle ages... make your own summation of node-forces in a cut and transform them into a coordinate system that suits your application. Fortran, Matlab, awk, Perl etc. etc. I should, however, prefer the *SECTION PRINT since Abaqus will do the job instead.

Live Long And Prosper

Truckcab

 

[tp701]

Hi Truckcab,

Thanks for your reply,

I will try your suggestions and let you know.

Thanks again,

Regards,
Tarun

 

[truckcab]

Of course I mean *SURFACE, TYPE=ELEMENT etc. and nothing else... I was a bit tired writing that post.
Sorry for that.

 

[tp701]

Hi truckcab,

no problem

Thanks,

Tarun