Crack modeling in steel part: How to choose the mesh size?

[Mohamed Zied]

I am assessing the effect of cracks in steel bridges. I chose the mesh size of 50mm for the whole bridge. When I modeled the crack (Cut in the shell element), I made the mesh smaller in the cracked part.

But I had different maximum tensile stress values in the cracked part with different mesh sizes ranging from 169 MPa for 50 mm to 273 MPa for 10 mm.
I am wondering how to decide about the result to consider? Should I keep the same mesh size to compare with the intact state?
Thank you in advance.

 

[FEA way]

Mesh around the crack should be properly refined. To avoid crack-tip singularities (like the one that seems to occur here) you should define the crack via Special --> Crack --> Assign Seam. There you can choose various options to account for singularity. If you are also interested in J integral evaluation then you should add concentric layers of elements around the crack tip.

Another option is to use XFEM approach which is less problematic in terms of required mesh refinement.

Generally, this model may not be suitable for fracture mechanics study since it consists of the large part of the whole structure. Instead you may want to narrow it down to smaller region of interest (for example using sumbodeling technique).

 

[Mohamed Zied]

Thank you for your answer.

I found that XFEM can not be used for 3D shell parts.
Is it possible to simulate cracks in 3D sell parts using seams(Special --> Crack --> Assign Seam)?

Thanks

 

[FEA way]

No, seams can be used only with two-dimensional (plane stress/ztrain) or 3D solid parts.

 

[Mohamed Zied]

So, you mean that there is no way to simulate this for my model (3D shell elements)?

In my case, I am assessing the effect of damages on the whole structure (Live load deflection, Maximum stresses in main members ...). The first case of damages was corrosion in different locations. Now, I have to model cracks for the same bridges to compare with the intact structure. There is no special focus on the crack itself.
What do you think about modeling cracks as a cut in the material?

 

[FEA way]

Actually, there are other ways to perform fracture mechanics analysis with shell elements. You can run crack propagation simulation without XFEM. And it seems that it’s also possible to use contour integral evaluation with shells (there are even special elements called line spring to model part-through cracks in shells).