peteroznewman
posted this
28 March 2018

- Last edited 28 March 2018
Hello Rosario,

You must turn Large Deflection On. That is why it appears the material is entering the blocks. That change will make the solver take a lot more iterations, so you will wait longer.

That change will also make the solver want to take smaller steps, so you can change Auto Time Stepping to On and suggest Initial Substeps to 10.

You should change the Contact from Bonded to Frictional. You should add all the curved surfaces below the flat surface on the blocks. As the plastic is pushed down, it will eventually make contact with the curved surface, so you want that in the definition.

You want more elements through the thickness of the HDPE to let it easily conform to the shape without excessive element distortion.

Get ready for some difficulties getting the solver to converge. Here is an example with the changes I put in above.

The solver took 53 iterations before I hit Interrupt. The model converged 30% of the way to the full displacement of 0.3 mm so it only can show 0.09 mm of closure. Corrective action in the model is required to get it to go further. Why is the solver having difficulties finding the next equilibrium solution? You need to look at the Newton-Raphson Residual plots to see where the largest force imbalance is in the model. Sometimes more elements near there can help. But to see the plots, you have to turn them on by typing how many you want saved. I typed 6.

After Interrupting Solution, you can look at a NR Residual plot. In this case, every one of the 6 plots had the Maximum Residual occur on either the top of bottom block, and since the mesh is so coarse, I expect a finer mesh is going to help the solver to converge.

Adding a lot of elements to the blocks is going to increase the wait time on the solver. One way to reduce that time is to change the blocks from flexible to rigid behavior. Then only the surfaces that push on the HDPE have to be meshed. If the deformation of the blocks is negligible, then this will save you a lot of time.

After increasing the mesh density on the blocks and changing them to rigid bodies (a few other edits go along with that), the solver now converges to 50% of the displacement of 0.3 mm but fails to converge. The NR plots only show the Pad now since the Blocks don't need to converge. And so it goes. The gap between the blocks seems to be 1.3 mm, so was 0.3 mm just a trial?

Another way to reduce the time spent waiting for the solution to converge is to solve only a small piece of the whole assembly. Isn't the left side just a mirror image of the right side? Why solve both? Just cut the model in half and use a symmetry plane at the center.

The temperature condition causes the thermal expansion to grow the pad 14 mm longer, 4 mm wider and 0.4 mm thicker. If you want that, you should do that in step 1 before you close the blocks in step 2, but you have to leave 0.4 mm of space for it to grow in step 1.

Viscosity has no effect in the Static Structural model. Plasticity will allow the material take on a shape. Viscoelastic may be useful in a Transient model.