Learning Forum

[Rizwan_ul_Haq]

Hi. I am doing simulation of compression testing of a spring.My experimental and simulation results are same in the linear region. I have tried the simulation with all types of contact behavior even with pin ball at different radius with linear and non linear material properties with large deflection on/off. The graph is different when all helix are in contact with each other.The following graph shows my results. I will be grateful if anyone can suggest any solution to simulate the encircled curve.

[peteroznewman]

Array nYou are showing compression as a positive value.nIf compression is along the X axis, that means the right end of the spring is fixed, while the left end of the spring moves to the right along the positive X axis.nPlease mark the blue curves with arrows or a legend to show compression and release. For example, use an arrow pointing to the right on the branch of the blue curve that was traced when the left end of the spring was moving to the right and the spring was being compressed. Use an arrow pointing to the left on the branch of the blue curve that was traced when the left end of the spring was moving to the left and the spring was being released.nDoes your material include plasticity? I expect you will need that to get a large nonlinear behavior.nYou say The graph is different when all helix are in contact with each other. Please show that graph.nPlease reply with images of the geometry and the mesh.n

[Rizwan_ul_Haq]

Please find below the images as give your valuable suggestions.There is no plastic deformation but i tried simulation with non linear data as well but could not get close to experimentation result.nn

[peteroznewman]

Make sure Large Deflection is On,.nYou need the contact to be present to increase the slope as the coils begin to collapse on each other.nYou need to get this behavior first. Attach a zip file with your project archive and I will take a look.nYou need Plasticity to have the slope change when the unloading occurs.nGo to the Engineering Data cell in Workbench, and from the Toolbox, expand the Plasticity category.nDrag and Drop Bilinear Kinematic Hardening onto your material. On the Yield Strength cell, pay attention to the units when enter a value. Type a 0 into the Tangent Modulus.nNow rerun your model.nn

[Rizwan_ul_Haq]

I have tried the recommendations but still struggling to get the required results. Please find the attached Archive file of my structure for further recommendations. I would like to mention that the non linear data is actually extracted by using extensometer and used in this simulation.I have to delete the results and solution data from the attached file due to size of the file. I ave used 0.5-1 mm mesh size with 26 mm displacement. So your valuable recommendations will be highly appreciated.nn

[peteroznewman]

When I said Contact, I should have been more specific and said Frictional Contact. Your model is using Bonded Contact, which doesn't pick up new contact as the structure deforms.nYou will have some trouble with frictional contact because your stack of washers is not precisely assembled. There is significant interference. Fix that before you start.nThere are five waves in each washer. Make two planes, and cut through the washers where they touch, then apply symmetry on those planes and the model that will solve much faster.n