Contact problem - negative or zero pivot

[mel08]

I'm having trouble with contact pairs, using ansys classic...
I have a cube of bone, which i need to compress with a metal plated. I have constrained all the nodes on the bottom face of the bone and have created contact nodes on the elements on the top face of the bone, target elements on the plate face in contact with the bone.
Essentially the plate needs to be glued to the bone, so I have used an MPC algorithm.
The plate can only move in the z direction, so I have set keyopts for the target element as:
keyopt,3,4,000100
For the contact element i have set the keyopts as:
keyopt,4,2,2
keyopt,4,5,3
keyopt,4,9,1
keyopt,4,10,5
keyopt,4,12,5
When i enter cncheck,status I get the following output:

*** NOTE *** CP = 14.344 TIME= 13:31:24
Deformable-deformable contact pair identified by real constant set 3
and contact element type 4 has been set up.
Contact algorithm: MPC based approach
The used DOF set is UZ

*** NOTE *** CP = 14.344 TIME= 13:31:24
Contact related post- process items (ETABLE, pressure ...) are not
available.
Contact detection at: nodal point (normal to target surface)
MPC will be built internally to handle bonded contact.
Average contact surface length 0.25000
Average contact pair depth 0.25000
Default pinball region factor PINB 0.25000
The resulting pinball region 0.62500E-01
Default target edge extension factor TOLS 10.000
Auto offset used to close gap/penetration -0.24750E-01
Initial penetration/gap is excluded.
Bonded contact (always) is defined.

*** NOTE *** CP = 14.344 TIME= 13:31:24
Max. Initial penetration 2.499992188E-02 was detected between contact
element 65851 and target element 64266.
You may move entire target surface by : x= 1.385992035E-19, y=
6.249960938E-05, z= -2.499984375E-02,to reduce initial penetration.
****************************************


1 CONTACT PAIR IS SELECTED
CONTACT PAIR HAVING REAL ID = 3 IS INITIALLY CLOSED

I increased my FKN to 1.5 and FTOL to 0.2 to try to reduce this initial penetration, but it doesn't seem to work.
The only constraint of the plate is this contact.
I then apply a surface pressure to the top face of the plate and run the analysis.
I continually get a fatal error saying there is a zero or negative pivot.
I know this is due to an unconstrained model, but I don't understand why my model isn't constrained.
Could anyone tell me what i'm doing wrong or how better i can constrain my model.
Hopefully what I've written makes sense!! If it doesn't, please let me know!!
Thanks!

 

[cbrn]

Hi,
supposedly the MPC contact is acting in direction Z only (which means that contact and target nodes / elements will "follow" each other in Z direction), leaving X and Y unconstrained.
If the plate really has to displace only in Z direction, put displacement constraints in X and Y, or if you can take advantage of symmetry (if you have a cube, you should be able to use two symmetry planes).

Regards

 

[meshparts]

Hi,

looks like the contact surfaces have initial penetration. This could be the reason for non convergence.

Adapting FKN will have no effect, as the MPC contact works with CE's not with the penalty method.

Regards
Alex

 

[cbrn]

Mihaiupb:
I don't think so. Initial penetration is likely to cause convergence issues because it makes the determination of initial contact stiffness problematic. However, it does not cause a zero- or negative-pivot error, this is mathematically impossible.

Regards

 

[meshparts]

Cbrn,

if Mel08 is doing a static analysis (and I think so) then following could happen:

1. With initial penetration the MPC equation will not be computed -> unconstrained model.

2. With an unconstrained model and a statical analysis one will get in my opinion exactly that warning: ZERO PIVOT.

If I am wrong, it will be nice if you would explain, why this should be "mathematically impossible".

Regards
Alex

 

[cbrn]

Hi,
the reason I think so is in the contact diagnostics:

Contact detection at: nodal point (normal to target surface)
MPC will be built internally to handle bonded contact.
Average contact surface length 0.25000
Average contact pair depth 0.25000
Default pinball region factor PINB 0.25000
The resulting pinball region 0.62500E-01
Default target edge extension factor TOLS 10.000
Auto offset used to close gap/penetration -0.24750E-01
Initial penetration/gap is excluded.
Bonded contact (always) is defined.

You can see, the algorythm has already applied an automatic adjustment. The contact is almost surely "closed" (the O.P. doesn't post any evidence of it, but the diagnostics above tend to proove that the contact is actually active).

Regards

 

[mel08]

Thank you to both of you for your responses.
Yes it is a static analysis.
I will try placing displacement constraints onto x & y.
The bone is essentially a cube, but it has a complex geometric structure of plates and rods, so I won't can't use any sort of symmetry for the model (would be easier!!)
Thanks again,
I'll let you know how it goes.
Mel

 

[mel08]

Hi cbrn.
I followed your advice and constrained the nodes of the plate in the x & y directions. I now can get a solution, but the plate does not stay stuck to the top of the bone, instead the plate moves through the bone, so I don't think that contact is actually ever detected. I think that my initial penetration is too large and so it can't detect the contact.
Is there a way I can reduce this?
Alex seemed to think that increasing the stiffness (FKN) would have no effect. Should i jut be increasing my pinball region??
Thanks,
Mel

 

[cbrn]

Hi,
1- if the initial penetration is "real", i.e. you really have interference fit in reality, then rather than MPC try to use an Augmented Lagrangian formulation. It allows for better controls when you deal with deformable / deformable parts. In fact, in cases conceptually similar to yours, I never used MPC, rather A.L. or penalty-based
2- if, instead, you have penetration due to geometric / mesh "unwanted" effects, try to resolve them physically on your solid model so that you have very small gap/penetration (by small I mean x10^-4 or -5 or so). The remaining gap/penetration can then be resolved by "adjust to touch" or "bring to contact", I don't exactly remember how Classical calls it.
3- mmmh, yes, to be honest I never used MPC formulation together with a penetration, so Mihailupb may very well be right when he says that the contact pair is not working.
4- pinball was already bigger than the penetration. So I don't think the problem is there.

Regards

 

[meshparts]

Hello,

that's the point with the MPC formulation, the automatic gap closing is not working. At least not not for my cases

So the contact must be closed before solving.

You also do not have to worry about any penalty stiffness, because the contact is described by constraint equations.

Regards
Alex