Mesh a complex part with voids

[saraalaw]

Hello,
I have a part made up of 3 layers, a top and bottom rectangular plate and a layer in between that is shown in the screenshot (

https://files.engineering.com/getfi...-4d93-90b2-f4bb59a83615&file=2020-03-16.png).

The three layers are merged together like this (

https://files.engineering.com/getfi...4-b53a-58c0be8a2aae&file=2020-03-16_(1).png).

I am trying to mesh the whole part with hex mesh (siz 0.5 or 1 ), however, it is not working due to the complications in the part. I tried to partition each layer alone as shown in the picture but it is still not working because of the middle layer. I also tried tet elements but there were many distortions so the Job analysis wasn't running.
Any suggestions on how to do this?

 

[FEA way]

Meshing this middle part (grid) would require very small element size and lots of partitions. I think that you should consider simplifying your model and using beam elements instead of solids for the grid. Outer layers could be modeled with shell elements.

 

[saraalaw]

I tried decreasing the element size up to 0.2 but it still didn't work.
I am new to abaqus so can you please explain more about the beam elemnts and shell elements?

 

[FEA way]

You would have to redraw the middle part. You can do it in Abaqus - just create 3D wire-type part and sketch this frame. Then assign beam section with proper profile. For outer layers you could use midsurface modeling to create shell part directly from solid. However these layers are so simple that you can create shell-type parts from scratch.

 

[saraalaw]

I did it as a beam element and the top and bottom layers as solids. I merged all the parts together and tried to submit the Job. Now i am getting this error:
In step 1, some contact edge thicknesses for general contact were reduced from the parent element or specified values due to a large thickness compared to edge dimensions. The most significant thickness scaling factor was 1.66732E-06 for an edge on parent element 175900 of instance TOTAL-1. An element set named "WarnElemGContThickReduce" has been created to locate the regions of reduced thickness.

 

[FEA way]

Merging is not a good idea in this case. It would be best to leave these layers as separate parts and then use general contact. Try with explicit solver if it fails to converge with standard.

 

[saraalaw]

I layered the 3 parts on top of each other. I did general contact. Now i am getting this:
For 1525 beam elements either the average curvature about the local 1-direction differs by more than 0.1 degrees per unit length as compared to the default curvature or the approximate integrated curvature for the entire beam differs by more than 5 degrees as compared to the approximate integrated default curvature. This may be due to a user-specified normal or due to the nodal averaging routine used by Abaqus. This difference may cause unexpected behavior of the beam and you may want to verify that the beam normals are correct for your problem. The elements have been identified in element set WarnBeamCurvature1.

 

[FEA way]

It’s a warning not error, right ? These can often be ignored but you should check them. You can query beam orientations in Property module.

Also remember that this frame (middle layer) should be offset from outer layers to account for beam profile thickness.