To mimic loading and unloading phenomenon using Abaqus I have tried applying load (as displacement, say from 0 to 1mm) in 1st step then in 2nd step I have changed it gradually to its initial value (zero). But, I am not getting expected result in terms of load vs deflection plot. I am getting some amount of residual reaction force at the end of analysis, but I want to free the model from it. Also, when the load is decreasing from its peak value (1mm), for the first increment (decrease in terms of displacement) the reaction force is increasing surprisingly. Please suggest me any procedure to get exact result. Thanks.
Dear Mandal,
I have a very simple suggestion to the problem.
Is it not possible to use a single step? From my point of view, it would be possible in ABAQUS to define a function of load i.e. a table of force versus time etc. In the same step you can start from a load of 0 units, increase it to the required value and then decrease it back to 0 units. Please update if you still get the problems.
regards,
Hamad
Please post more information about your model:
What is the geometry, what is the material model used, what is the element type and mesh, what is the Abaqus procedure (step definition), what are the results exactly, what is the increase in reaction force you observe?
Without more detailed information, there are too many possibilities to give a clear answer.
It sounds as thought you might have included plasticity in your material model and that your prescribed displacements are loading the plate into the plastic region. If this is the case then you would probably not expect zero reactions even if you go back to the original state. If you loaded your model with prescribed forces rather than displacements then you would obtain zero reactions but there might be a residual, self-balancing, stress field within your plate.
Thanks Baeker Sir and Ramsay Sir.
- This is a simple plate problem. Plate is made of laminated composite material. One shorter side of the plate is fixed and an axial displacement has been provided on the other end i.e. like a simple tensile test.
- I have integrated a material model using UMAT considering Hashin failure model in 3D.
- I have used 3D brick element C3D8R (tried C3D8I also). I have done mesh convergence study and mesh size is okay.
- The analysis steps are static, general with initial increment size 0.025 and maximum 0.1.
- The residual reaction force I am getting is very less compared to its maximum value. Like, maximum reaction force is 28.65 kN and residual amount is 11.4 N. But, I am getting a jump in reaction force to 32 kN when I am decreasing the load (in terms of displacement). The plot is attached.
- I have not considered any plasticity in my material model. As Ramsay Sir said I can use force rather than displacement but then convergence problem may come.
I want to know any standard procedure to this type of problem. Thanks.
Here are a few things to check:
Did you test your model with simple linear elasticity, to make sure that it works correctly?
"I have not considered any plasticity in my material model." However, a failure model (where different elements in the end have different stiffnesses) may lead to similar effects, I think.
Are there residual stresses at the end in the model that explain the non-zero force?
What happens if you reduce the size of the time increments? Do the effects change?
If you look at the first unloading increment, what happens with the stresses? Is there a stress increase somewhere in the model? What about the energy balance of the model - make a plot of ALLWK, ETOTAL and other relevant energies.
Dear Mandal,
I have a very simple suggestion to the problem.
Is it not possible to use a single step? From my point of view, it would be possible in ABAQUS to define a function of load i.e. a table of force versus time etc. In the same step you can start from a load of 0 units, increase it to the required value and then decrease it back to 0 units. Please update if you still get the problems.
regards,
Hamad
It is a good suggestion to run the model without the failure model to see that all is working properly. The graph you provided indicates zero force then the model returns to the original state but it returns down a line with a different gradient to that on loading. So your structure has become stiffer for some reason. It all seems most curious! By the way you should not experience a convergence issue when loading with force provided the structure retains some stiffness.
Thanks Baeker Sir and Ramsay Sir.
Thank you Mr. Hamad for your excellent suggestion. Its working perfectly and I am very happy.
I have tested my model for a lower load like 0.5mm (in terms of displacement) where there is no failure and the model works perfectly. The loading and unloading both curves are linear and in same way as shown in attached figure.
For higher load also now it's working well using the method suggested by Mr. Hamad. The new Reaction force vs. Displacement curve is attached for displacement upto 1mm. There is no jump in reaction force during 1st unloading time and also residual reaction force amount has also decreased from 11.4N to 3.5N which is very less compared to the maximum reaction force.
Thank you once again all of you.
Thank you Mr Hamad, your suggestion was very helpful. Much regards
- Badges
- Science topic