Hi Everyone, I hope to get some answers to clarify some abnormal post processing results with my FEA model.
Basically I have a sensor housing that sees 20 K pressure on internal walls, the base is fixed. I need to capture the axial and circumferencial stress and strain all along the length of the ID and OD. I am trying to have the output on a table/graph.
But after preliminary alanysis, I came accross this unusual post processing contour. picture below is the deform model (scaled to 2% of model). Could anyone explain to me why this midnotes are pulled towards the OD asymmetrically? I assume that is not supposed to happen. This asymmetrical condition at the base translates all the way in to the ID (as seen below).
Could someone please help me understand the results above.. Thank you.
Solved! Go to Solution.
It is difficult to say without the model. I think you used midside nodes not on surface. This can alter locally the geometry and with 20 K (barg I suppose) may cause such distorsion.
This load can also be investigated teorethically. I have used a similar model to validate femap calculation without this probelm. In my opinion is better to simplify the model taking into account of simmetry: you can use 1/4 the model and I don't agree to fix the base. In this case usually I use Sliding along a plare (and also along simmetry planes)
If you like sent the model
Thank you. I could have taken advantage of the symmetry and used a 1/4 model. I will do this again to compare the results. In my previous solid file (as you can see in above picture above), I have sliced the model along global planes. But this time I created a boundary surface and revloved the geometry and elements. The results seems to be fine this time. Please see the attached file. I don't see the unusual deformed pattern in the base anymore.
But I do have a couple more quesitons.
1 - When I changed the BC of the base to "allow sliding along surface" the run is terminated and fatal error message received. Not sure why?
2 - How could I select a portion of the model (or a plane along X-Y) to plot the circumeferencial and axial stress, strain vs X-position? Right now I am using the entire model to plot the stress, strain. But as you are aware there are too many data points and its hard to visualize or explain the results.
You have to contrain the model in all X, Y and Z direction!
I will answer you with more time tonight.
Atttached there is your model I have modified as listed below:
I have sliced your model along the global planes XY and XZ;
then I have sliced 1/4 of the model with the curve of the end of the hole so that I am able to mesh the model with Hex elements;
I have constrained the model in all 3 dimensions with "allow sliding only along surface";
Finally I have put pressure load on the hole surfaces.
To plot stress I use the FEMAP Stress Linearization Tool (see Femap forum) to analyse stress according to ASME Section VIII Division 2. Otherwise you can do a Freebody study selecting the nodes or regions you want. See also this picture and the your model modified without results due to dimensions
Dear AMinati, Thank you.
I was able to do a 1/4 model analysis and used the Stress Linearization Tool to plot the stress disctribution along the thickness of the sensor housing. This helped me a great deal. However I could not open the model you attached. I extracted the file and when I tried to open it, I keep getting the error message as seen below. my Femap version is 11.1.2.
I have opened my zip model1 file without errors, now I send to you same model but as neutral file.