Dear all,
I have worked out an APDL code (the code is attached) for a 3-point bending test analysis. I used SOLID186 to mesh the model and for the contact, I used CONTA175 and TARGE170 elements. the analysis is static based with 50 steps. I am facing two problems :
1- The first one is that I get the nodal displacement but unfortunately, I don't get the element's reactional force, contact pressure as well as Vanmises stress. I used OUTRES,ALL,ALL to claim the results but the same problem occurred.
2- The second problem is that I just got the last step. ansys doesn't record the results of every.
Any suggestions will be highly appreciated.
Best,
My suggestion is to exploit symmetry and to use a plane model (in plane stress) in order to reduce simulation time.
Moreover, Workbench is defintively easier than APDL in managing contact problems
Denis Benasciutti , Thank you for your suggestion, I have already performed the simulation using 2D plane elements as you proposed. Now, I am focusing on the 3D solid model with APDL in particular.
Try changing the memory use to "Shared-Memory Parallel (SMP)" in the Ansys Mechanical APDL Product Launcher.
David Alegre Gimeno Thanks, I have tried your suggestion but no luck, the same problem.
How about solving 50 loadsteps, each with just 1 substep? I'll be a bit more of code, but getting results should be less problematic.
David Alegre Gimeno I have followed your advice and used 50 Steps which results in recording just the displacements of 3 steps of i think there is a problem with results convergence.
But what confuses me is why Ansys isn't recording element reactions and stresses !!!!!
Kouider Bendine I tried to run your script, but it didn't converge. It stopped at time 0.16. If it doesn't converge you can only access to the results of nodal displacements, so in my case that was probably the reason why I couldn't retrieve other results like reactions and stresses.
David Alegre Gimeno yeah you're right I did run it and indeed it is a convergence problem as you stated. Will try to increase the mesh in the contact area and see if it converges
Kouider Bendine I found a couple of problems in the code.
First, the contact surfaces are defined as areas, but using elements CONTA175 (node-to-surface). I tried with CONTA174 (surface-to-surface) and it reaches the last substep. Here's how I defined the contact element:
ET,3,CONTA174
KEYOPT,3,2,1 ! Formulation: MPC
KEYOPT,3,4,1 ! MPC - Force-distributed constraint
KEYOPT,3,12,5 ! Bonded (always)
Then, the top cylinder was not properly contrained. I tried constraining the model like if modelling only a quarter of the system - double symmetry. For a quick test without changing the actual model I just did this:
ALLSEL
NSEL,S,LOC,Z,0
D,ALL,UZ,0
ALLSEL
ESEL,S,TYPE,,2
NSLE,S,1
NSEL,R,LOC,X,Lb/2
D,ALL,UX,0
Now the model converges and I can access the stress results in all substeps. Probably still have to adjust the contact surfaces to avoid stress concentration.
follow the below link. I explained about it. also follow Dr.Dalyo tutorials.
https://www.researchgate.net/post/Experimental_and_Simulation_Verify_of_Reinforcement_Concrete_Beam_Bending_Crack_with_Ansys_Workbench/1
Seyed Reza Jafari Many thanks for your reply , However, my main tool is APDL not workbench