Displacement not translating?

[Anonymous]

Hi all,

I'm having issues having a rubber part interact with a rigid material part.

Despite a huge pressure on the top of the rubber part, it appears like it doesn't bend far enough to interact with the rigid part despite the displacement according to the contour plot saying that it's well over the nessessary displacement. Does anyone have any suggestions on what could be wrong with my set up?

[AstroJohnPE]

You are performing a linear static stress analysis which is only accurate for small displacements. In most cases, you would not be able to see the displacement because it is so small (such as 0.001 inch), so the software automatically scales the displacement by some "magnification factor". In your case, 2E8 inch displacement scaled by a very small magnification factor makes it look as if your part is hardly moving.

You could change the "Results Contours > Displacements > Show Displaced > Settings" (or whatever the terminology is) to show a scale factor of 1 instead of the default value of 5%. But if you did that and enclosed the model, you would not be able to see your 4 inch size model on a screen 2E8 inches high!

Probably what you should do is correct your model. It is not statically stable due to the surface contact, so as described in the documentation (on the page "Perform Analyses with Gap Elements"), you need to add some weak springs to any part that is "held" only by the contact. After doing that and finding that the displacements are small, you'll better understand why the software automatically magnifies the displacements.

[Anonymous]

I understand the magnification now but I'm still confused as to where the springs should be placed to lock the flexible part to the rigid part. Is it the node where they contact or bridging a gap between a flexible part node and a rigid part node?

[AstroJohnPE]

Actually, the weak springs that I was thinking about (and discussed in the documentation) are a type of constraint that connect the node to the ground ("Setup > Constraints > 3D Spring Support"). They are not an element that connects two nodes of the model together.

In short, pick any three nodes (as long they are not in a straight line), and apply the 3D spring supports. Fix the XYZ directions. Set the stiffness to a small value. Keep in mind that these springs do transmit load from the model to the ground. That's why you set the stiffness to a "small" value so that the magnitude of the load transmitted (= displacement * stiffness) is insignificant compared to the appied load (and the accuracy of FEA in general). Give it a try!

Going a step further in the explanation, the issue with contact in a static analysis is that the solver does not know which nodes are in contact until the displacements are calculated, and it cannot calculate the displacements until it knows which nodes are in contact. So it becomes an iterative solution where it assumes some nodes are in contact, calculates the displacement, and adjusts the assumptions. The problem is that if one of those iterations has too few nodes in contact, it is possible for the part to move a large distance, and for some reason the solution is not able to recover from that situation. By imagining that the contact elements do not exist, you can determine which parts are not statically stable. By fixing 3 points (not in a straight line) in X, Y, and Z translation, you create a statically stable part (it cannot translate in X, Y, or Z, and it cannot rotate about X, Y, or Z.) Once the part is statically stable, an interation during the solution that has too few nodes in contact will result in a valid solution but with a "large" displacement. Based on the calculated result, the solver detects that some more nodes would have come into contact, and it continues to the next iteration with the additional contact. Eventually, it converges to a solution.