You are here
ABAQUS shell element stress output
Mon, 2008-10-06 12:05 - PJtree23
Hello,
I am running ABAQUS EXPLICIT to simulate aortic valve function. I created a model using hex shell elements. When the simulation is complete the output contours are in U,Magnitude, in the list of primary variables to show; there are a few other options, put they are all of kinematic/dynamic nature, there are no options for material stresses or strains.
I realize that U,Magnitude is displacment, but how can I visualize the von mises stress contours? Von mises stress is selected in the Field Output criterium. I am completely out of ideas and very frustrated, please make comments or let me know where to look for a solution, please!
Thanks in advance,
PJ
Forums:
Free Tags:
So nobody knows the
So nobody knows the answer? I am guess it is impossible for ABAQUS to report the stress or strains of a shell element....can anyone please tell me what is going on here?
PJ
Re: impossible for ABAQUS to report the stress or strains ...
".. guess it is impossible for ABAQUS to report the stress or strains of a shell element".
I took that as a challenge and decided to pursue the matter. I don't use ABAQUS at present nor have I used it extensively in the past.
If searched the web an found an Abaqus manual at http://www.hlrs.de/v6.6/books/exa/default.htm. After reading TFM I found an example at http://www.hlrs.de/v6.6/books/eif/pressfueltank_uniformthick.inp
There I saw the following string of commands
*NODE PRINT,FREQUENCY=0
*EL PRINT,FREQUENCY=0
*EL FILE,ELSET=SAMPLE
STH,
SINV,
*OUTPUT,FIELD,VAR=PRESELECT,FREQ=10
*ELEMENT OUTPUT
STH,
*OUTPUT,FIELD
*ELEMENT OUTPUT,ELSET=SAMPLE
STH,
SINV,
*OUTPUT,HISTORY
*ELEMENT OUTPUT,ELSET=SAMPLE
STH,
SINV,
Then I tracked down the Abaqus keywords manual (at http://www.hlrs.de/v6.6/books/key/default.htm) and searched TFM for *element output. The help page said that this command determined which variables were to be saved. A little more of searching pointed out that STH means section thickness and SINV means stress invariants.
I presume that if you save these quantities you should be able to plot the von Mises stresses. The exercise took me less than 15 minutes.
-- Biswajit
It worked, thank you so much
It worked, thank you so much Biswajit!
For my simulation I was running into errors with the S4R element however, in the example you posted the S3R element was used. I am now using the S3R element for all of my models with good success. I was curious about why this worked.
Could it be that the SR4 element is numerically "less sophisticated" than the SR3 element for curved surface modeling? Just a thought.
Anyway, another question about interpreting the von Mises stress plots, for the position selection I am selecting "Unique Nodal" and the graph contains two sets of data :
S, Mises (Avg: 75%) SP:1 PR:SHELLCBAV_SM-1 N:16_1
S, Mises (Avg: 75%) SP:5 PR:SHELLCBAV_SM-1 N:16_1
What do the terms SP:1 and SP:5 correspond to? (in bold)
Are they the outer and inner surfaces of the shell element?
Thanks,
PJ
I have the same problem,
I have the same problem, There are two available outputs for von mises stress, what do they mean?
S, Mises (Avg: 75%) SP:1 PR:SHELLCBAV_SM-1 N:16_1
S, Mises (Avg: 75%) SP:5 PR:SHELLCBAV_SM-1 N:16_1
What do the terms SP:1 and SP:5 correspond to? (in bold)
Are they the outer and inner surfaces of the shell element?
Setion points
SP stands for 'Section point'. These exist in beam and shell elements and provide the spatial resolution through the thickness. See User's Manual on 'Elements'.
Note that the output for non-default section points has to be requested explicitly; see Keyword manual on 'Element output'.
Good luck
Frank