Challenges with Orphan Mesh Drop Test in Abaqus 1

[TwiceYTPL]

Hi everyone,

I'm fairly new to Abaqus and I'm facing a bit of a challenge. I've been trying to simulate a drop test where an object falls onto a rigid plate. I successfully completed a similar simulation with two solid balls interacting with the plate, and the contact definition worked perfectly.

However, I'm now working with an orphan mesh instead of a solid object. I've searched online and in the Abaqus documentation, but I haven't been able to find clear instructions on how to handle this scenario.
How would I go about defining the material properties, assigning a section, and setting up the contact interaction for the orphan mesh? I've tried assigning a "surface shell" section to the orphan mesh. This allows the part to fall, but it somehow disintegrates upon contact with the plate. Also the interaction with the solid balls in unrealistic. The orphan mesh part doesn't roll at all and just falls straight to the ground and deforms the solid balls massively upon contact. So my question is, how do I work properly with orphan meshes? Is it even possible to simulate a drop test with an orphan mesh, or is a 3D volume element strictly required?

Thanks for the Help

 

[FEA way]

So it’s a surface orphan mesh representing thin-walled hollow sphere ? Orphan meshes can also consist of solid elements, it depends on how they were created. But if it’s a thin-walled part then you should assign a shell section and the rest should work normally.

 

[TwiceYTPL]

yes its a thin-walled surface orphan mesh. However if I assign a homogenous surface section to it I get the following error message:
Error in job impactexplicit: 4028 elements have missing property definitions. The elements have been identified in element set ErrElemMissingSection.
But I assigned a section to the part. I also made sure that that I didn't leave out any element. And if I click on the part I can see that the section has been assigned.

 

[FEA way]

By surface section do you mean Create Section --> Shell --> Surface ? If so, don't use it. Choose Create Section --> Shell --> Homogeneous instead. Also, check the type of surface elements in this mesh.

 

[TwiceYTPL]

I get the error message exactly when I use the homogeneous shell. When I instead use surface, the simulations runs but has the problems I mentioned earlier. From the input file I can see the element type as:

Element, type=SFM3D3. For the section I have this entry:

*Elset, elset=_PickedSet4, internal, generate
1, 4028, 1
** Section: Section-3
*Shell Section, elset=_PickedSet4, material=alumm
0.01, 5
*End Part.

There u can also see the 4028 elements that supposedly miss a section assignment

 

[FEA way]

SFM3D3 is a surface-type element. Those elements (with their associated surface sections) have no stiffness. Change the element type (using the Assign Element Type button) to Shell.

 

[TwiceYTPL]

You're a lifesaver! Thank you very much!