how to data for a surface 1

[iwb]

Hi,

I'd like to have the values for the stress components
for a cut through a body analog to a path in 2d. Is this
possible an how does it work.

Thanks

 

[xerf]

Visualization Module->Menu->Tools->View Cut->Create.

 

[iwb]

I don't need the graphical representation in the CAE.
What I need is a list of values that I can further process
with python. I try to do it with the xxx.getSubset(...) but
I thought there would be a more convenient way.

thanks for your help.

 

[xerf]

I am not aware of any ABAQUS Scripting Interface, that would output data for arbitrary cutting planes (or other surfaces).

The difficulty comes from the fact the values are computed either at nodes or at integration points.

Since the cutting surface can be arbitrary, first, a plotting algorithm has to figure out the values for the data it needs based on the available information at nodes and integration points. The structure of the data necessary for the plotting algorithm might be different then the typical ABAQUS data storage (i.e. related to nodes/integration points/centroid etc). Therefore
FieldOutput.getSubset(...) might not work. You can see actually that .getSubset(...) returns a FieldOutput object. That means the data structure underlying the FieldOutput is conserved when .getSubset(...) method is used.

A simple trick would be to create a partions of your 3 model before running the analysis along the cutting planes. This way, ABAQUS will generate nodes on the partion faces.
Further, you can create Sets based on the inner partion faces.

Then run the analysis.

In the end you can use FieldOutput.getSubset(...) to extract the data for the sets you created along the cutting planes.

Also, you might be interested in using VTK. (

http://www.vtk.org)

VTK is avalaible for Python language, you can try to write code to convert the ABAQUS data into VTK data and then use VTK algorithms to obtain the data along cutting surfaces.

Brep might be able to provide useful info if he reads this thread.

Best.

 

[brep]

If you're using Explicit you can use a method of creating a partition, an internal surface and then request "integrated section output". See section 14.13.1 in the /CAE Users' Manual (and other references)

In Standard you could try a method like xerf suggests. Create a set on the internal face from the partition and request NFORC or whatever from that set. You'll at least have some data to start playing with in your python script.

I'm not sure using vtk will help here, although I am still playing with it for other purposes...

 

[Yoman228]

I never use VTK before, Is it easy to learn and what is the use of it that viewer can not do?

 

[xerf]

1. VTK is a FREE library available for C++/Python/Java/TCL which you can integrate it in your own code.

2. It incorporates useful algorithms for data visualization.

3. See

http://www.vtk.org

for details.

 

[brep]

No it is not "easy to use", unless you are a reasonably experience programmer familiar with object oriented languages. (VTK takes a heavily object oriented approach).

However it contains a huge range of objects/methods that you could piece together to do just about anything that is related to meshing/visualization. For example you can take a cloud of points (e.g. a scan) and then perform a delaunay triangulation on them. Using this you could construct an ABAQUS mesh, do some field to field mapping, whatever.

There is no built in geometry (nurbs etc) though, so if you needed that you'd have to look at incorporating something like OpenCascade, and if you are doing that then you are essentially building your own CAD system or pre/postprocessor - goodluck, and hope someone is paying you or you have a lot of spare time...

 

[iwb]

The suggestions with the partition worked very well.
Thanks again! But actually I was not able to get the coordinates for the respective integration points. Do I have to compute those coordinates by hand or is it possible to get it from the odb?

I considered VTK for other purposes, but did not see the value for FE-postprocessing. I will try it.

 

[xerf]

For the integration points the situation is complicated since the they are not in the cutting surface, if you use the partion approach.

If you need a field which is stored at the integration points then you should need to obtain the field in terms of its nodal values.

I think you can do that by something like

nodalFieldOutput=myfieldOutput.getSubset(position=ELEMENT_NODAL)

Then use nodalFieldOutput.getSubset() again to obtain to extract those values on the cutting surface set.