I have a simple model with contact between a bolt and a bolt hole. The component with the hole in it is fixed at the bottom, and a force load is applied to the bolt. See image below (model in Mecway).
As you can see in images below, the displacement of the bolt seems to change direction towards the end of the load step. The displacement of various nodes have been plotted versus the applied load. I have run three different analyses, one with 10 kN, one with 100 kN and one with 1000 kN. In all three the same behavior is seen.
Does anyone have a good explanation for this phenomenon?
I have also included some of my input below (with 100 kN of applied force).
Can you share the whole input file (paste it here) so that we could run some tests ? If not, please provide more details about this model. For example, what are the remaining boundary conditions, how is the load applied, what are the contact properties and so on.
Take a closer look at and animate the deformed shape of the model before and after this change in displacement. You should notice what happens with each part.
I have looked closely at the deformed model, and in the last few increments the bolt part seems to change direction and move downwards again, in opposite direction to the load applied to it. I have not be able to identify the reason for why this happens.
I examined the deformed shape of your model with various scale factors and it doesn’t look bad. There’s a small (but visible) penetration in contact first and then there’s a sort of rebound when this penetration is reduced as the bolt moves out of it slightly. It happens around the 23rd increment and can be observed as a drop on your plots. You could try changing contact properties and using displacement control to eliminate this behavior.
Hi @jbr ! As the load is incremented linearly and a linear-elastic material is used, I would expect the bolt part to move upwards throughout the entire step.
By increasing the contact stiffness, by quite a lot, the curves shown in the original post flatten out and become almost linear. However, this is only a simplified version of my actual problem, and in the actual model a contact stiffness this high leads to some convergence problems.
So I still haven’t been able to understand why this happens.
From my point of view there is something inconsistent on those results. If that result were a non-intuitive but correct result , the reversal on the displacement should appear at the same Force[N] value . In this case, It seems to happen at an 80% of the overall load no matter the load.
I have done the same calculation but following some suggestions from the manual:
The surface with the larger area should be the master. If the master is not the largest surface area there is no warranty that there is always projection support for the slave nodes.(bolt). I have swap MASTER (bolt) /SLAVE (Plate).
The surface with the coarser mesh should be the master. The node densities seem too similar . I have refined the slave by changing the plate to second order.
I have also considered :
Additional plane of symmetry for shorter computation time.
Initial 1mm clearance to make first step easier to converge.
I have redone the calculation considering this , with and without friction, and I don’t see that strange behavior.
