Hertz contact

[butho]

Hello everyone,
This is my first post on this forum and my english is not perfect, I hope you will understand.

Thanks to some work done and posted here, I've been able to model a hertz contact in case of ball bearings. I've tried different meshing options but this one seems to work properly even if it takes more time to solve.

My first issue is that I would like to use EFORce instead of  EDISplacement, as I know the applied compression load. (You can see that I have just use a hertz approximation in the input file below, so that I can use EDIS.) When I use EFORce, it looks like the boundary condition ligne 44 plays a key role in my problem, but I can't figure out why.

My second point is concerning the exploitation of results. I used to work on Abaqus and I was wondering if we could plot on feap the stress along a path for example. Also, I was looking for indications to add the tresca yield criterion in a script.

Finally, I was looking for how to add reference point in order to interpolate my results.

Any leads or help would be appreciated. Thank you,
Thomas

I use version 8.4.1.

[Prof. R.L. Taylor]

Let me try to answer you questions.

1 When you specify a non-zero boundary condition restraint (EBOU) then feap looks for a matching displacement condition (EDIS).  If you replace the EDIS by an EFOR then feap will ignore it if the corresponding boundary condition is still non-zero.  Thus you could have both EDIS and EFOR in a file and feap will pick the one that matches the boundary code for each dof.

2. You can display the stress along paths in 2-d problems using the PLOT SPLOt command.  You must do it in interactive mode as you need to use the mouse to pick the display line you want.  It is not as good as Abaqus because it plots on top of the mesh.  To use it: (a) enter PLOT with no arguments.  This gives a pure graphics mode. (b) enter SPLO n (n is component you want - there is a DPLO n too) (c) use the mouse to mark the A and B ends of a line (d) feap will plot the stress along the picked line.

3. I am not clear on what a "reference point" is.  TPLOt allows you to select some points and output the values at different times of the analysis.  Can you describe a bit more about what you want to perform with this?

[butho]

Thank you for your quick reply !

I understood that non-zero displacements may be specified for restrained dof's and non-zero forces for unrestrained dof's, and I understood what you said.

As I could not manage to apply these (simple) boundary conditions(*), I tried to use the AXIS SYMMetric. I changed the geometry to respect the r-z coordinates with z as the axis. It looks more coherent, but I’m still not sure how I can apply the load.

SOLUTION 1 :
Using CSUR to apply a pressure, like in the plastic example
=>I get an error. I check on the forum but this is still unclear to me.

-->Contact check
  *ERROR* Residual norm is NaN or Inf

SOLUTION 2 :
Using a Pressure MATErial tied with the ball, with TIE REGIon or TIE MATErial
=>It does not converge during CONTact CHECk. As no full convergence is obtained for the Newton solution strategy, I tried the manual option

LOOP augment a-iters
AUGMent
LOOP newton n-iters
CONTact CHECk
TANGent,,1
NEXT newton
NEXT augment

I got less warnings but a wrong solution.

SOLUTION 3 :
Using EFORce with the force in Newton applied on each node knowing that the factor 2pi is not included in any applied
loads.
=>In this case I noticed that the nodal force was not constant on each node, specially on the node located on the axis symmetric. I suppose this is due to a superposition of loads created by the symetry. (*)

I can't find where I'm wrong, any help would be appreciated.


(And thank you, TPLOt will do the trick. I need these reference points to interpolate the stress field, as I'll add inclusions distributed in the thrust washer according to a random space distribution.)

(*) I got "Internal server error" if I upload the picture

[butho]

It works now.

[butho]

Update :

Error on CSURface was due to a wrong points definition (right hand rule) seen thanks to the Ofile.
Multiple loads applied on the (0,0) node were due to the definition of the disk. It needed to be tied.