I am simulating uni-axial compression behaviour of porous materials and used multi-linear isotropic hardening material. Now I have to plot stress strain graph from simulation results in order to compare it with experimental results. I can do this in three ways:
1 - find the reaction loads of selected nodes at different displacements and convert into stress strain graph.
2 - plot of y-component of displacement versus y-component of stress at a node.
3 - plot of y-component of displacement versus von mises stresses at a node.
Which option should I use? For 2nd and 3rd options, I have to specify a particular node. Which node should I select? How can I spot the node at which stresses are maximum, because my finite element model has large number of nodes?
You have a lot of options in ansys to do so.
in /post1 you can define "paths" via the path command and then let ansys map all posible results onto this path via pdef. You might even do some methematical operations with this results via pcalc. At the end you can save such path informations either in a external file or into an array from which you can write some output via *vwrite into an external file. The only problem is that you only can define a line of interest.
If you want something more advanced, because for example the region of highest stress chainges during your calculation you might want to use *get or *vget commands to retrieve your results and then find the point of highest load.
One option that you can use is the Time history post-processor (main menu), with this option in ANSYS you can plot several variables of you model.
An about the question 3, regarding that you are using a porous material, the volume of the specimen can not be considered as constant, it mean that the hydrostatic stresses are acting on it. If we review the theory of Von Mises, we should note that is formulated under the assumption of constant volume ( it means that only the J2 stress invariant acts), so for this reason I think you shouldn't use Von Mises as a failure criterion.
In the other hand, you can sort the results of your simulation by nodes, elements, areas, etc.. After this you can set a range of values ( in this case stress) that you want to analyze, only the elements in the range will be shown
you cannot get stress-strain curve from a single or multiple nodes. you need to "cut" the specimen [by path operations as suggested by Martin, and integrate the "actual" stress [[ not Von-Moses]] in the direction of loading. I would do that in 3 distinct locations [of course it should give you similar results due to equilibrium but nice to do this to consider numerical inaccuracies] and then find similarly the average displacement at each one of these three distinct locations, then try to calculate strain from these average displacements. Von Muses is a sort of resultant stress that you don't need since you are calculating uni-directional stress behavior now.
Thank you very much Martin Hofmann, Gustavo Capilla-González and Mahmud M.S. Dwaikat. The problem had been solved with your suggestions.
- Badges
- Science topic