Obtain cross-section forces 2

[AkbarAkbar]

Hello everyone,

I am trying to obtain the history of cross-section forces (forces and bending moments) from a 3D-Shell Model.

Anyone can give me some suggestion? What should I do to take out cross section forces?

Thanks in advance.

 

[Chen1]

If you mean Reaction forces and Moments, you can use Free body cut to get them, but remember you need to output NForc, which is the nodal force due to element streses.

 

[akabarten]

Hi,

For Abaqus/Standard please check:
Abaqus Analysis User's Manual, 4.1.2 Output to the data and results files, Section output from Abaqus/Standard
Abaqus Analysis User's Manual, 4.2.1 Abaqus/Standard output variable identifiers, Section variables

For Abaqus/Explicit please check:
Abaqus Analysis User's Manual, 4.1.3 Output to the output database, Integrated output in Abaqus/Explicit
Abaqus Analysis User's Manual, 4.2.2 Abaqus/Explicit output variable identifiers, Integrated variables

Regards,
Bartosz

 

[AkbarAkbar]

Thank you so much for reply.

I defined field out put for the section that I need to get force. In Visualization module, I create XY Data - ODB Out put then I get section force (SF) at integration point of the node set that I already defined. Afterward, I add these forces up to obtain the section force. But it gives a wrong value.

Could you please let me know if I am doing right thing to get the section force?

Thanks again.

 

[AkbarAkbar]

Hi Chen1,

I created a free body cut of the section, and I am able to get forces and moments for this specific section at a certain Step Time. I am wondering how I can get the history of forces and moments using free body cut, as the analysis lasts 400 Time Step to be completed?

Thanks again

 

[akabarten]

Hi,

What Abaqus do you use? Explicit or Standard?

defined field out put for the section

Integration output from Abaqus/Explicit is history output type not field output type.
You should get access to the curve with Abaqus/Viewer, Create XY Data, ODB history output.

Section output for Abaqus/Standard does not store outputs with *.odb file.
It can be stored to *.dat file and/or *.fil file.
The first one is just ASCII file, you can open it with any text editor.
The second one is old Abaqus output format.
I never used so I am not sure what software can be use to open that file.

Regards,
Bartosz

 

[AkbarAkbar]

Hi Bartosz,

Thank you for reply.

I am using ABAQUS Standard. I defined History output for NFORC (nodal force due to element stresses), and I got this output in simulation module, but working with history output in simulation module is not easy. When I open the .dat file corresponding the job that I am running I got this warning " ***WARNING: OUTPUT REQUEST NFORCSO IS NOT AVAILABLE FOR ELEMENT TYPE S4R"

Could you please help me out from this problem.
Thanks

 

[akabarten]

Hi,

I took detail look for section output from Abaqus/Standard (*SECTION FILE, *SECTION PRINT).
It looks like it can be use only with continuum elements (hexa, penta, ...).
Base on your last post I see you are using shell elements (S4R).

In this case the only choice is to use Free Body Cut with Abaqus Viewer.

1. Define NFORC field output for elements you want to cut

**
*OUTPUT, FIELD, FREQUENCY=1
*ELEMENT OUTPUT
 NFORC
**

2. Define Free Body Cut in Abaqus/Viewer
Tools -> Free Body Cut -> Create
As method choose "Elements and nodes".
First choose elements, push OK, next choose nodes (attached to selected elements) and push OK to finish cut section definition.

3. Create XY plot
Tools -> Free Body Cut -> Create -> Free Body
Choose options you need and push "Plot" button.

I am attaching simple model I used for my tests.

Regards,
Bartosz

 

[AkbarAkbar]

Hi,

I followed the steps you mentioned. I created Free body cut for the defined section. However, I do not understand no. 3. "Tools -> Free Body Cut -> Create -> Free Body" refers to step 2 again, if I am not mistaking. Should I create XYPlots using the left result tree in order to plot the history of the forces and moments of the free body cut?

Could you please clarify that.

Thanks,
Akbar

 

[akabarten]

Hi Akbar,

You are right, I see my mistake now.

In step three should be:
Tools -> XY Data -> Create -> Free Body.

Regards,
Bartosz

 

[AkbarAkbar]

Thanks again Bartosz. It worked.

Akbar

 

[mturkol]

Hi,

Just a little note on obtaining the correct cross section forces: NFORC is the element nodal force output, and gives you the corresponding internal forces at each node representing an element. NFORCSO results are computed at each element integration point and might or might not be accurate depending on the mesh sensitivity of your problem. This is a big issue especially when one tries to correctly model the fatigue behavior of welded joints. You might want to take a look at "Equilibrium Equivalent Structural Stress Method" introduced by Dr. Pingsha Dong. He published numerous papers on this, and the correct traction based structural stresses on a free-body cut can be computed in a mesh-insensitive way.