Crack inside the geometry: how to partition and use the TIE constraint 1

[eispiata]

Hi,

I am trying to model a crack inside the geometry. Due to the loading applied to the outside boundary of the model i can't simplify the model into its half or even quarter part. I definitely want to model a crack line inside the geometry.

I have been told that i can do it through the TIE constraint.
I read up on that but i still have a few questions.

1) First of all, to partition the geometry how should i do?
Should i create two separate instances in the part (see attached file) or should i create one instance and partition it in the middle (see attached file) so that the crack faces = doubles nodes with the same coordinates?

2) When i want to use the TIE constraint. There are different options: Analysis default, node to surface, surface to surface. Which one is the most appropriate in my case.

3) In the TIE constraint you can specify a distance for the position tolerance. Does it means that all the nodes within that tolerance will be tied to the master surface even though they do not belong to the slave surface?

4) Since the TIE constraint stands for two glued surfaces i hope that the two tied surface will always have exactly the same shape?

Thanks,

Malik

 

[eispiata]

Hi,

I ran a simple uniaxial tension model with two separate instances. As you can see on the pictures i tied the top and bottom surfaces, the top surface being the master surface.

As you can see in the results, the crack line doesn't remain exactly horizontal but is slightly waving along the horizontal line. Why ? It supposed to remain straight even after deformation...

Maybe i should rather create a crack surface with doubled nodes with the same coordinates but how can i do that?

Thanks for your help,

Malik

 

[xerf]

A slave node is tied to a master node only if it is at less than a certain maximum distance from the master node.

Your mesh looks bad. You should use similar seeding approaches for both matching edges.

 

[corus]

If the surfaces were tied then the displacements would be the same on either edges. Clearly they're not in your case. The mesh looks like you've thrown some automatic mesh generator at it. I'd create a circle around each crack tip, where the peak stress is, mesh that finely and then graduate the mesh away from that region. A smooth graduating mesh will give you much better results than one that is haphazard and where there are large changes in element size in close proximity.

corus

 

[eispiata]

Hi,

You were right Xerf. I used similar seeding approaches for both matching edges and i got something nicer with the expected results. Actually it is even a requirement to make it work properly.

Corus: as you told me to do i created a circle around each crack tip and it worked great. Definitely the computed results clearly match the theoretical results.

But as you can see on the . ODB file that i attached to this reply, due to the "adjust slave surface initial position", the crack has not a symmetric deformed shape and thus its half bottom shape doesn't look really nice compared with the half top one. And i think that besides the mesh itself, this "fill the gap" may cause a loss of accuracy in the results.

So how can i do to get a symmetric shape? Should i inactivate the "adjust slave surface initial position" option?

Moreover i noticed in the results that when you want to compute the strain energy of the whole model the volume of the initial gap is actually included in the computation.

So how can i take advantage of that "adjust slave surface initial position" and at the same time get a symmetric crack shape and a computed strain energy that includes only the volume of the model at the very beginning.

Thanks for your help,

Malik

 

[xerf]

The countour plots do not look symmetric because the mesh is not symmetric and because the plotting algorithm which extrapolates the values from the integration points to nodes before plotting.

You can create a rectangular partition encompassing the crack and use a structured mesh inside this partition.

 

[eispiata]

Hi Xerf,

I am going to try it. Actually i used a symmetric contour and i seeded this contour by number but in the mesh control, i used a free mesh thinking that Abaqus could create a symmetric mesh on both sides but apparently i was wrong.

Actually i can't use a structured mesh: only the Free mesh is activated. I am using a "mesh on instance". Do you think that i'd better use a mesh on part?

Thanks,

Malik

 

[xerf]

If you partition a part, then you can assign different meshing algorithms to different regions (partitions) of the same part.

For example, if you partion a part by a rectangle (using partition by sketch) you can mesh the rectangle with a structured mesh.

Best.

 

[corus]

You won't have a structured mesh as you have two points on the edge. I think you need to have at least a four sided region for a structured mesh. You could simply partition each region by drawing a vertical line from the crack tip. That would give you 3 four sided regions in each part. Personally though I'd still opt for a half circle around each crack tip and then partition the regions remaining to give you a structured mesh.

corus

 

[corus]

Here's an example of a mesh at a crack tip I found on the web.



corus

 

[eispiata]

Thanks