Compression test on a complex geometry 2

[mdama]

I am trying to do a compression test on a macrostructure (about 20cm) such that the structure includes two parts, one with pores (

https://www.dropbox.com/s/j7ummlx3j9es88e/part1.PNG?dl=0)

which has a height and the other one as you see here(

https://www.dropbox.com/s/xmaq39nsdxmm53w/part2.PNG?dl=0),

covers the height of the first one (part2). You can see the assembled one here (

https://www.dropbox.com/s/udon5o7sca4oueg/whole structure.PNG?dl=0).

I used a cylindrical indenter to apply displacement to the structure. Here is the details:
1) I used a very high elastic modulus for the indenter and considered a rigid body for it with reference point
2) I used elastic-plastic materials data for the part with pores
3) I used only elastic properties the same as part 1 for part 2
4) In order to connect part 1 with part 2, I used tie constraint where the surfaces of part 1 (part with pores) that are in touch with part 2 were considered to be slave. Surface to surface discretization method was also used
5) In order to mesh part 1, I create a partition such that surface that contains pores become separate (wedge element) and the rest as tet shape mesh.
6) The indenter was considered as master and the structure underneath was slave
7) The surface below the indenter was meshed finer to get more accuracy
8) Surface to surface interaction between indenter and the structure was assumed with normal behavior
9) I considered the whole surfaces of the indenter as master and only the top surface of the structure (here part2) was assumed to be slave
10) The bottom surface of the structure was constrained only in loading direction (u2)
All is in static general. I used 1E-25and the initial time step and 1E-30 as the minimum time step. Also IA as 50 (number of iterations).
I get an error:
Time Increment required is less than the minimum specified,
What is the solution to this?
You can also see mesh here (

https://www.dropbox.com/s/8u1b02pyuns7bo4/mesh.PNG?dl=0)

Any suggestion on this process would be appreciated. Also what do you say about the tie constraint?

Thanks

 

[FEA way]

This error indicates convergence issues that may have various causes. Try decreasing minimum increment size though I doubt it will help. In your case I guess the model is underconstrained and there are so called rigid body motions which can’t exist in static analysis. Instead of constraining the structure only in the loading direction apply encastre constraint to it (you can do it through kinematic coupling if you want). Also how is the indenter constrained ? Its motion should be fixed in all directions apart from the enforced one (movememt towards the structure). In this case apply BC to reference point.

 

[mdama]

Thanks
Still the same issue, any comment on the Tie constraint?

 

[FEA way]

You can try with contact instead of tie (so that these surfaces can separate) but the latter should work too. I suggest increasing mesh density. Outer layer part should have at least 3 elements per thickness.

Explicit dynamics analysis may be better in this case but first read all warnings from that failed static simulation and make sure there are no unconnected regions apart from contact before initialization. Make the indenter touch the structure from the beginning and experiment with settings of this contact interaction. Try with stabilization on. And assign mass to the reference point of rigid body.

Can you share a picture with all boundary conditions ?

 

[Mustaine3]

A better mesh + A/Explicit + General Contact + some tests on the Mass Scaling settings and the topic would be done really fast.

 

[Mustaine3]

And it seems that there are two symmetry planes possible for simulation, so just running a quarter region.

 

[mdama]

The structure that you saw, is already half. The other half is on the other side which I used symmetry boundary condition for z surface instead.
Since, I used symmetry BC, should I also draw half cylindrical indenter? (what I used:

https://www.dropbox.com/s/icdb9ush63hx668/Capture5.PNG?dl=0)

I deleted the Tie constraint and used tangential and normal properties between the surfaces of part1 and part2, still getting error.

 

[mdama]

I used these two interaction:
(

https://www.dropbox.com/s/vdal0d5dl6cyuq1/interaction1.PNG?dl=0)

and
(

https://www.dropbox.com/s/t1fvu906g6ztay8/int2.PNG?dl=0)

 

[FEA way]

Yes, cut the indenter in half too along with the structure since the symmetry plane goes through both parts.

This contact interaction between indenter and structure may be problematic because in the same definition there is a cylinder base initially touching the structure and cylindrical face not touching it.