Still trying to model a crack inside the geometry: fancy crack shape?

[eispiata]

Hi,

I am still trying to model a crack line in a 2D plane stress rubber membrane subjected to different states of stress (not only uniaxial or equibiaxial tension ...). Due to the loss of the symmetry i have to model the whole model, i mean i can't simplify the model into its half or quarter part. To do so, i decided to partition the whole domain in two subdomains with the crack line laying at the interface of these two subdomains (see schematic pictures: model1, 2 and 3).

The points at the interface that are outside the crack are constrained with a TIE constraint so that the stress and strain are continuous (see schematic pictures: model1, 2 and 3). The crack is modeled by releasing the points within the crack line from any constraint so that they are free to move apart from each other (see schematic pictures: model1, 2 and 3). Two surfaces are created in the interaction module to be used as slave or master surface.

The two bottom red surfaces make up the first surface and the two top red surfaces make up the second surface (see schematic pictures: model1, 2 and 3). "Adjust slave surface initial position" is on.

To get started i modeled the case of a simple uniaxial state of stress!

The problem is that whatever the gap (as sketched in the part module) between the two surfaces is, the crack doesn't look good. What i mean by doesn't look good is that instead of an elliptical shape, i get this fancy shape (see Results.jpg) with a big gap between the crack faces. I know that this is caused by the "Adjust slave surface initial position" and the fact that the crack faces are untied.

But this fancy shape distorts the elements in the vicinity of the crack and this results in a discrepancy of the field outputs. Is there a way i can have the crack closed at the beginning (crack faces would look tied even though there are not)?

Indeed i would like the crack to have an elliptical shape as it should have.

Moreover, this initial gap between the crack faces causes the crack tip not to be a crack tip. I mean that, as you can see on the picture, there is no crack tip but a gap between what is supposed to be the crack tip. It may come from the fact that to refine the mesh around the crack i sketched a partition which seems to have removed the tie constraint. But why is the TIE Constraint removed by the partition sketched in the Mesh module to refine the mesh around the crack?

So please let me know what is wrong with my model and how could i get what i expect: an elliptical crack shape with a crack tip.

I remind you my two questions:

1)Is there a way i can have the crack closed at the beginning (crack faces would look tied even though there are not)?

2)Why is the TIE Constraint removed by the partition sketched in the Mesh module to refine the mesh around the crack?


Best regards,

Malik

 

[eispiata]

Sorry i forgot to attach the schematic pictures

 

[corus]

Sorry, but from the results picture the two sides look tied to me. You can see contours and mesh which can only exist if there is material there. The displaced shape doesn't look elliptical as the mesh looks poor at the crack tips (bearing in mind that it is distorted). The top looks smooth and then jumps to the coarser mesh at the crack tips.

Sometimes though you have to be careful after defining surfaces as later partitions might renumber the surfaces. Go back and check your surface definitions in the interaction module so that they are the ones you want, after you have finished doing any additional partitioning.

corus

 

[bfillery]

eispiata

You could try to define a seam (Intereaction-Special-Crack ???). I know this functionality is avaiale in 6-7. In this case the mesher creates duplicate nodes along the seam such that the surfaces along the seam can seperate. In this way the rest of the model can be simply connected as normal and you do not have to use a tied constraint. Furthermore with some partitioning you should be able to obtain a better mesh quaility around the crack tips.

bfillery

 

[eispiata]

Hi,

Actually i defined a seam and it is definitely the best thing to do in my case.

Since i would like to apply a compressive loading to the outside boundary, i would like to preclude crack faces overlapping.

But when i apply such a loading, the crack faces overlap.

Is there a way we can preclude crack faces overlapping using "seam"?

Best regards,

Malik

 

[bfillery]

eispiata

I have done this before. You need to apply contact to the opposing seam surfaces. Although the documentation seams suggests this is not possible it is, and it works. There is one difficulty. If you are using the fracture mechanic capabilities and therefore define a crack tip singulatity (collapsed elements at the crack tip), you cannot simply select both of crack faces and apply the surface contact. Instead, you first need to define a node set containing the mid-side (or 1/4 point nodes) of the crack tip elements on say the upper crack face. The remaining elements along the top surface can then be used to define a surface for the remaining upper crack face. You can then use all the elements along the bottom crack face to define the bottom crack face surface. Two contact pairs are then defined. The first a node based contact between the node set containing the upper mid nodes (1/4 point) and the bottom crack face surface. The second a surface to surface contact for the remaining top element based surface and the bottom crack face surface.

The reason for this is because of the way in which the nodes are constrained at the crack tip. Basically you have to exclude the crack tip nodes from the contact definitions. The way above is the only way in which I found this could be successfully done. However, it does require python programming. For a better explanation have a search for the ZENCRACK documentation on the web. It provides similar descriptions as to how crack face contact is defined.

bfillery