Abaqus meshing internal crack in cylinder

[DKEngineer]

Hi,
I am trying to model an internal crack in a cylinder as seen on "Image_001". I am using the Abaqus contour integral method to model the crack in a 3D model. First I will verify the model by comparing the results of a penny shaped crack obtained in Abaqus to analytical solutions. Next I will model irregular shaped internal cracks. But the meshing seems to cause problems.

I am trying to partition the crack front with contours around it using shell sweep and then merge it into my solid cylinder. "Image_002", "Image_003" and "Image_004" shows that this is feasable for a cylinder cut in half (using double symmetry model). But as soon as I try to model the same penny-shaped crack in the cylinder using only symmetry in the crack plane, problems occur, which is seen in "Image_005" and "Image_006".
1) Why am I not able to mesh the cells around the crack front in this model?

Next I will model an irregular shaped internal crack. The only method I could come up with was partitioning only vertical lines around the crack front through the whole cylinder as shown on "Image_009". Then I am using seeds on the lines marked with red to obtain mesh contours for the contour integral. But I like the partition used for the first model better.
2) Are there any suggestions for a meshing strategy for my problem?

Best regards

Image_001

Image_002

Image_003 (Red edge is crack front)

Image_004

Image_005

Image_006

Image_007

Image_008

Image_009

 

[FEA way]

Regarding the problem with meshing the second model (Image_006), you would have to take a closer look at the unmeshable orange region - make a view cut or replace this region using display group tools. Additional partitions or different approach to partitioning might be necessary.

 

[DKEngineer]

Hi FEA way, thanks for your quick reply.

I use the same partition ("Section Sketch" for sweep shell) in the first and second model. Therefore, I cant figure out why the cells around the crack are unmeshable in the second model.

Yes partition is key, but I am having a hard time figuring out a proper partioning. I have seen videos on youtube on the topic. But i cant find anyone modelling internal cracks in a 3d body. And not for irregular crack fronts at all.

 

[FEA way]

What if you partition that model with unmeshable region as if you were cutting it in half (like in the case of the double symmetry model) ?

 

[DKEngineer]

That works! And it also works for an irregular shaped crack. But I wonder why this works?

And thanks for the tip FEA way!

 

[FEA way]

Abaqus sometimes needs additional partitions because the regions are too complex to be meshed with hex elements and require further simplification. In this case, cutting in half seemed to be the most natural way but in other cases, there might be different ways. You should take a close look at unmeshable regions to determine the best way to add more partitions.

 

[DKEngineer]

Just found this information on the Abaqus documentation website:
"If a part was created by sweeping a cross-section along a sweep path that is composed of a closed spline, the resulting part is meshable only if it is split into two or more regions."

https://classes.engineering.wustl.e...s/usi/default.htm?startat=pt03ch17s10s03.html

So the solution is to split the sweep cells into two or more cells.