I am getting a deflection of 0.6 mm in ansys apdl. Where as the experimental result have shown a deflection of 8-9mm. Kindly help in solving the FE analysis in ANSYS 19.1.
Following are model description.
Load - 2 point load
Support - Roller(Right) and Hinge(Left)
Load step - 1
Substep - 50
Mesh size- 20mm
Steel 8 mm diameter and concrete 150X150mm
You can try to solve it activating large displacements (NLGEOM, ON). This activates nonlinear solvers.
If this doesn't work, the differences can be due to material properties, boundary conditions, mesh size...
In my opinion, you should check your BC that has an effect on deflection.
Hello David and Hoang
I have tried with all the possible BC and cross checked with material properties. But couldn't able to get any change in the result with that variations. Initially there was problem in completing the analysis, now the analysis is completing and issue with the result.
Thank you
David and Hoang
Softwares give elastic deflection. It ignores deflection due to creep and shrinkage
Greetings Ravindra Ramanad,
Is there any valid Creep and co efficient values available in code ? So that it can be incorporated in the FE analysis?
Ansys doesn't account the nonlinearity such as cracks. Such a case has to be analyzed using fracture mechanics principles.
- In the experimental test did you use LVDTs to accurately measure the deflection.
- In ansys did you check your boundary conditions, concrete, steel and the combination between them. also the units for the values input.
- did you check the concrete material model you used and the failure criteria.
- did you apply any type of symmetry on your model.
- In general it's tricky to get SOLID65 element to converge with both cracking and crushing activated, the load (displacement controlled) should be applied at a very slow rate with a fine mesh. If the concrete cracks are not important in your analysis then you can try the newly developed Microplane model using SOLID185 with damage elasticity/plasticity or with CPT215 coupled damage.
@Ahmed Mirghani
1. In experimental setup deflection is measured using analog dial gauge and also obtained through UTM software. However, dial gauge reading is considered for sturdy.
2. After inspecting boundary condition, concrete material model and cracking and crushing one thing which gave some varied results are meshing and rate of application of load.
3. However, it is taking long duration for the analysis and some of the internal elements failed due to large strain. Still unable to solve that failure of internal elements and continue the analysis.
- SOLID65 element has a well known relation with concrete material in ansys APDL/workbench (through commands). however the convergence issues associated with SOLID65 element and the mesh sensitivity of the CONCRETE/SOLID65 combination was one of the motivations for moving to the Micro-plane model that tracks the softening behavior of the concrete as it fails, without having to track individual cracks.
- Load should be applied as a displacement controlled loading instead of force controlled to get pass the necking in the stress-strain (load-deflection) graph. Load controlled analysis will fetch you with the maximum load v/s displacement. If you need to get the deflection after maximum load then you need to perform displacement analysis.
- you can drop your force convergence and only consider the displacement convergence in the non linear stage that is from first crack or simply for the whole analysis you can drop your force convergence, or you can use force convergence upto linear stage only, only non linear starts then drop force convergence.
- you can get use of symmetry to save solution computational time. for example if you model a quarter of the beam then the solution will take 1/4 the time required for the full model (if the mesh and other parameters are the same)
- Did you activate the Keyopt. for solid65 element specially the stress relaxation
keyopt,matid,3,2 !Suppress mass and applied loads, warning message and apply consistent Newton-Raphson load vector.
keyopt,matid,7,1 !Include stress relaxation
keyopt,matid,8,1 !Suppress warning message for totally crushed un-reinforced element
- you can try the SOLID185 element with microplane model as its by far more accurate and easier to converge than the solid65. just to check the deflection and compare it with the experimental. the only drawback of the SOLID185 with microplane model is that you can not view the concrete cracks as SOLID65 element.
@Ahmed Mirghani I have not tried any of your added points. I will try them.
Thank you
Hi Sachin Vijaykumar. Have you tried hand calculations for this?What deflection do you get by beam calculations? I feel that would be an easy way to check if the sanity of the FEA results since this seems to be a simple beam problem.
Sachin Vijaykumar
Have you found a solution for your problem? because I am facing the same problem as yours and I don't know how to solve it
You need to study non-linear fracture mechanics of concrete. During bending, there is bridging between steel bars and concrete, also between agregate and matrix. So the beam is bending nonlinear. This phenomenon is impossible shown by software.
Hi dear,
You may try with fck=-1, as uniaxial crushing stress, instead of giving cube strength fck. And consider open and closed shear constants as 0.3&0.5respectively. Still not happen, change your convergence criterias of force =0.1 or displacement criteria with disp=0.1.
- Badges
- Science topic