Parallel FEAP results in ParaView

[TonggeWu]

Hi,

I am using parFEAP to solve some static structural problems.
After reading the FEAP manual, I tried following solving command:

Code: [Select]

BATCh
  PETSc ON
  TANGent,,1
  FORM residual
  DISPlacement ALL
  STREss ALL
  REACtions ALL
  PVIEw sample_name
END

STOP
However, parFEAP gave me one file (I had four domains solved together) named "sample_name.vtu".
And when I imported this ".vtu" file into ParaView, the software gave me some error message.

Can anyone tell me if I should modify my solving command?
Thank you so much~

[FEAP_Admin]

The

Code: [Select]

FORM residualis not needed (unless you are keen to see that the residual has converged).

Regarding PVIEw, it seems to have acquired a bug in the parallel version (the file names are incorrect so they are over writing each other).  We will investigate a fix.  Thanks for the bug report.

In the meantime, if you need to see the solution you can use the interactive plotting (makes one window per partition).  Or you can use the method described in section 3.4 of the parallel manual.

[FEAP_Admin]

One way to make it function immediately is to use

Code: [Select]

PVIEw,timeThis will name the files as P<your_problem_name>_<process_number><time_stamp>, so you do not get to name the file but now it works.

To get a merged, single image, create a collection file; see http://feap.berkeley.edu/wiki/index.php/Collection_file .

[TonggeWu]

The

Code: [Select]

PVIEw,time works and ParaView stitch several domains automatically. This is cool. Thank you so much~!

However, I do have another question about the visualization. In the ParaView, when we look at different properties (e.g. displacement, stress/strain, principal stress), there are additional options for direction or component (to my understanding). Why there are 7 components (0-6) for principal stress and 15 components (0-14) for stress and strain?

[TonggeWu]

In the ".vtu" file, there are following comments:

First:

Code: [Select]

<DataArray type="Float64" Name="Stress/Strain" NumberOfComponents="15" format="ascii">I also found the last 3 values are alwasy 0. Then I guess the first 12 variables will be stress 11 22 33 12 23 13 component, and strain 11 22 33 12 23 13 component, is this correct?
 
Second:

Code: [Select]

<DataArray type="Float64" Name="Principal Stress" NumberOfComponents=" 7" format="ascii">But I don't get it, I thought there would be only 1- 2- 3- principal stress 1- 2- 3- principal strain.

Furthermore, I found the displacement values are evaluated at nodes, how about the stress/strain and principal stress/strain? They are evaluated at gauss points, nodes or center of an element?

Thank you very much~!

[JStorm]

The stress and strains are projected in the elements to the nodes for plotting purpose. The number and order of stress/strain components depend on the used element type. But the number of components is at least 15. For user elements it is possible to active and use more than 15 components.

You are right, for 3D solid elements the order is 6x stress + 6x strain. the 15th component is not used.

[FEAP_Admin]

The quantities under principal stresses are the same as the first set of values printed by

Code: [Select]

stre,node in the Macro phase;
see http://feap.berkeley.edu/wiki/index.php/Nodal_Stresses#First_set_of_values for details of what is computed.

[TonggeWu]

Thank you, JStorm and Admin.

One last question, if I don't have

Code: [Select]

stre,node in my solving command but

Code: [Select]

stre,all (since I need stresses at gauss points for later use), the

Code: [Select]

PVIEw,time will still project the stress/strain and principal stress to node?

[FEAP_Admin]

I think that you need to issue STREss,NODE before PVIEw,time to get the stresses output to the VTU file.
STREss,NODE force the nodal projection.  (STREss,ALL only prints the Gauss point stresses.)

[JStorm]

The paraview macro do not support to provide data at the integration points. I have extended the macro to have that feature. If you are interested write me a PM and we can ask my Prof. for providing the code.

[TonggeWu]

I think I should rephrase my last question:

1)If I use "STREss,NODE + PVIEw,time", in this case, I will have nodal stresses in my Ofiles and .vtu files, right?

2)If I use "STREss,All + PRVIEw,time," in this case, I will have gauss stresses in my Ofiles and nodal stresses in my .vtu files?
(This is what I did actually, I had gauss points stress in my Ofiles, but I did not know if the stresses in .vtu files are nodal stress)

[Prof. S. Govindjee]

VTU files will always have nodal stresses.  But it is important to generate them first with either Marco> stre,node or Plot> stre.  Note, both commands will generate them for all nodes.

Macro> stre,all will write all the Gauss point stresses to the Ofile.

Macro> stre,node,x,y will write nodal stress for nodes x to y to the Ofile.  If you leave off x and y you will get the nodal stresses for the first node in the output file (but FEAP does also compute all the nodal stresses).