problems with displacement during friction 2

[WayneKagawa]

To test out friction in ABAQUS, I tried to model the interaction between two blocks in 3D, the smaller one(1x1x5)resting on the Larger one (10x10x10) with both having a mass density of 1000 kg/m3.
The interaction was defined as follows:
Tangential Behaviour - 0.7 (friction coefficient using the penalty method).
Normal Behaviour - Hard, Default.
Master surface was the base of the smaller block and the slave surface was the upper surface of the larger block.

To test friction, I applied an incremental load using concentrated load with a tabular amplitude starting from 10KN to 0.7x49.05 = 34.335KN to bring about slip at the base on the bottom-most node of the smaller block.
In addition I applied a gravity load.

I expected the smaller block to move after it hits the critical load but it is being displaced as soon as it hits the first load i.e 10KN.

I am extremely confused by this behaviour. Please help.

 

[Mustaine3]

Read the users manual regarding penalty friction and elastic slip. That explains the behavior you're seeing.

As an alternative the lagrange friction might be interesting for you.

 

[cooken]

Can you upload your input file?

First thing to check is your loading sequence. Are both loads applied in the same step, and if so, are you staggering them with amplitude definitions? Without an amplitude given for gravity it will start from zero and ramp up linearly with step time, so your normal force might be too low. You can request additional contact output to see what the normal force on the contact interface is.

Second thing to check is your element size and elastic slip. The penalty method allows some relative motion in the sticking region, and it is based on the element size. So if your elements are fairly large relative to the size of your block, you will have quite a bit of movement even though the blocks are "stuck" together. You can modify the default relative slip (*friction, slip tolerance=X) or change it to an absolute distance (*friction, elastic slip=X).

Also at first glance, your choice of master/slave looks odd. Typically the larger object will also have larger elements relative to the smaller one, and so should be assigned master. This is not true in all cases, and may not matter for your analysis but it is good practice.

 

[WayneKagawa]

Hi
Thank you Mustaine3 and Cooken.

I had a look through the manual and read the part regarding penalty method, lagrange method and elastic slip quite thoroughly.
I inferred from the text as well as from Cooken's observation that Abaqus assumes a certain elastic slip during the penalty method to undergo analysis via the stiffness method. The plot of the shear stress and total slip has a finite slope which is a graphical representation of this phenomenon of a default slip even in situations where the overall environment of the model is of slipping. I would appreciate if you could tell me where it is useful though.

For infinite slope between shear stress and slip i.e sticking, Abaqus recommends the usage of the Lagrange Method.

I tested the model again,the first time with a load lower than the critical load and in the second experiment with the previously defined incremental load.

The first model shows a very slight displacement (1.32*e-5, way lower than what I got previously. I still don't know if this is correct. Maybe if I refine the mesh a little more it will become even lower. Is it possible that it would come down to zero or nearby?

The second model also shows the same pattern. The relative displacement of the upper and lower blocks is very near to each other until it is nearby the critical load at which the displacement between the two increases substantially enough to simulate slipping.

Also, cooken I checked the application of gravity load. The amplitude was 'instantaneous' so I presume it is not ramping linearly. Please correct me if I'm wrong. And also, I chose the smaller block's base as master as I applied the load at that point itself. Is that not correct in this situation?

Many thanks for your help. I have attached the input file incase anyone wants to have a look.

 

[cooken]

The elastic slip region is there primarily for convergence, however can be quite useful in many applications (simple soil models for example).

I didn`t realize you were running a dynamic analysis, so yes, in that case the full gravity is applied right away. But then you also need to be careful about oscillations and/or damping, not to mention inertial forces. You are applying 30kN in 0.3s, which is rather quick. Is this the intent, or is it supposed to be quasi-static?

I would still choose the larger block as master, and given the dynamics involved, use a finer mesh on the smaller one. If it was static the decision would probably be arbitrary.

The relative displacement of the upper and lower blocks is very near to each other until it is nearby the critical load at which the displacement between the two increases substantially enough to simulate slipping.

Is this not the expected behaviour? If you're not convinced about the small initial slip, try doing this with rigid bodies first - simplify until you are confident in what Abaqus is telling you. You can even start with an analytical rigid surface and a single node (lumped mass). Remember you have strain happening in there as well, and complicated element formulations, and a point load. Look at the contact shear/slip in the X direction at the perimeter of the top block, what does that tell you?

For knowing whether or not your FE results are correct...welcome to numerical analysis. Try many things, and do your best to collect, process and plot your results in a meaningful way in order to understand what is going on. If possible compare to analytical solutions.

 

[WayneKagawa]

Hi
The intent was to check the load where it slips and to reduce computational time. Hence I gave a large increment.

The behavior was as expected. I'm just a little curious as to why it has to slip even by that little amount before the critical load. I'll work on your suggestion of using a simpler model.

Thank you again!