Submodeling Method in ABAQUS/STD 6.4 2

[jmolligan]

I am doing contact analysis between the actebaular cup and femoral head of a total hip replacement implant. Basically it's a ball and socket joint (ball is made of steel, the cup is made of polyethylene). The cup is held in place my a rigid body backing. I ran a non-linear global model with a contact pressure and frictional torque. I then cut the global model and refined the mesh for a submodel. My question is do I need to impose redundant boundary conditions for the submodel (i.e. do I need to impose the contact pressure with the ball and the rigid body backing of the cup). Or can I simply specify the driven nodes which should be the nodes on the cutting plane, the nodes on the back of the cup (which are held in place) and the nodes at the interface? This is my first real project with ABAQUS and I'm only 19, so if someone could help I would be greatly appreciative.

JM

 

[corus]

If you're using a sub model then boundary conditions come from the driven nodes. If any other prescribed displacements or loads that applied to the global model also occur within the sub model region then apply those too. You can check your sub model is working by comparing the contours of displacements at the boundary with the global model. Because of the interpolation that occurs the contours won't appear so smooth but values should in general be in line with those of the global model.

corus

 

[gwolf]

Sounds very interesting, I wish that I'd had access to ABAQUS at 19! What corus says is correct, and the displacement contour plot is a good way to ckeck that you got it right.

It sounds as though you are trying to refine the contact area between ball and cup to get better contact stresses and to cut out a lot of elements in the femoral head to save analysis time. You are submodelling across a contact boundary and although this might work there could be problems. I think that the following is the best way to model this problem:

Model most of the ball structure with a very coarse mesh and model the contact area with a fine mesh of C3D8I elements. These elements are VERY good for contact. You can either zoom the mesh from coarse to fine manually or you can mesh the ball in two zones and use a *TIED contact pair to glue the two bits together. If necessary do the same for the cup. Then run as normal.

You should also look up "Herzian Contact" which is very good at predicting stresses where two surfaces of possibly differing radius contact. I have correlated this with FE and found the results to be so good that for simple problems I would never bother with an FE model again. Not sure how friction will affect this.

When contacting metal against polymers the failure mechanism is usually sub-surface failure in the polymer.

Good luck.

gwolf.

 

[gwolf]

Sorry "Hertzian Contact"

 

[xerf]

In "Abaqus/CAE User's manual" there's a section containig a step-by-step description of how to use submodeling technique ("24.7 Submodeling") within CAE.

 

[jmolligan]

Hey guys,

Thanks for all of the information. I have actually gotten it to work in the mean time, but I do appreciate all of your responses. Gwolf, you are correct in that I am trying to refine my mesh at the contact area to save analysis time, but I should further explain my modeling situation. I am not wholly concerned with the contact stresses in the femoral head (as that is made of metal and relatively immune to wear) so I have modeled it using an analytical surface (sphere of course). For the cup I simply use second order brick elements (C3D20) and so far that is pretty much it. Would there be any advantage it making the interface elements C3D20I (if they have 2nd order interface elements that is) and the rest of the cup regular C3D20?

Jeremy

 

[gwolf]

Assuming that your rigid surface assumption for the femoral head is valid, which it isn't quite, but good enough for now.

Don't use C3D20 elements for contact, the result will be an extremely spotty stress field with huge variations in stress between corner and mid-side nodes. Model the whole of the cup with C3D8I elements. Make sure that you have some small elements through the thickness normal to the contact surface because you will most likely be looking at sub-surface stresses as a failure criterion.