FEMAP NODAL STRESS

[JohnHam]

Hi all, Please excuse that I have put this question also in the femap section, but looking at the posting dates it gets little use.

I am Pulling out what little hair I have left. Just started using Femap, can't say I am impressed on user ease. Everything seems to be listed in places you least expect. Tech support seems very slow and poor , one of those call centre type log your issue and get back etc and the manuals seem non discript compared to the abaqus manuals I am used to.
I have a simple problem. I need to take off nodal stresses and shears on node sets preferably put into a table to transfer into excel. All would be well if it was elements stresses as that seems easy to do, but nodal results seem limited to displacements and rotations etc.
What I am trying to achive is take nodal stresses through a section to linearize them for ASME codes.

Shouldn't be hard, could have done it in seconds using abaqus, cant do it in Femap and I've been looking for hours!!

Thanks in advance for a any help

John

 

[rb1957]

i'd use the .f06 file (output destination = print & post-process) and edit the executive deck (under model/analysis).

can you use element stresses ?

 

[kellnerp]

Did you ask for them before you ran the analysis? If you did you can easily get them just like any other post process quantity.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[JohnHam]

Thanks for your answers. I could use element stress but the the mesh is in such a way that I am not sure it will give me the stress reading right on the edge or not.

Did I ask for nodal stresses? No. How do I ask for nodal stresses before analysis. I have started picking off the stresses using the pointing tool and hovering over the right nodes. This is very slow , however proves the stresses are there and have been calculated I just don't know how to get to them.

John

 

[kellnerp]

What finite element code are you using with FEMAP?

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[rb1957]

how about exporting the results (since you've imported, from the analysis, the corner stresses) ?

he'd be running NASTRAN, NX probably ??

 

[kellnerp]

RB1957,

I don't assume, but it does sound like the shoe fits. It is always proper to let people on a forum know the background of the question if it cannot be gleaned directly from the question. In this case the question is about FEMAP not the solver.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[ProbaSci]

In my version of FEMAP (8.3) you can't request stresses on nodes, only elements when you set up the analysis file. All of the associated stresses are only available on elements (at least for tet meshes.

I think when you use the manual probe, you are actually getting averages calculated from the element stresses.

http://www.probasci.com

-
Implantable FEA for medical device manufacturers

 

[AndyFEMAP]

What you can do in FEMAP is "convert" the elemental stress to "nodal stresses" using the "Model, Ouput, Process" command. Once the "Process Output Data" dialog box is open, follow these steps:

1. Choose "Convert" in the options section. Choose whether you would like to convert using the "average value" at each node calculated from the element stresses or the "maximum" value.

2. In the "From" section, choose the Output Set where the appropriate stress Output Vector exists, then choose the stress output vector itself.

3. Click the "Add Operation" button, then click "OK".

A new output vector with the value "9000000..Converted Ouput Vector" should have been created in the Output set you selected. This output vector contains nodal stress output. You can now use the Data Table or an Output Listing to get the values you need and take them to excel.

Please let me know if you have any questions.