Problem with "Volume Mesh" and "Abaqus Voxel File" export

[willsenwijaya]

Hi,

I tried to export my textile model (just the tows without matrix) to ABAQUS using two options:
1. Volume mesh
Both the matrix and the dry fiber mesh are combined as a single entity of mesh when imported to ABAQUS. Is there a way to make them as separate sets?

2. Abaqus file --> abaqus voxel file
This time when I imported the voxel meshes of the tows, the different tows within my unit cell is combined as a single entity. I was expecting that the different tows will be divided into different sets and that they are not connected to each other so that I can model the relative motion of the tows in compaction simulation. Is there a way I could do this?

[louisepb]

Hi,
I'm afraid that I don't fully understand the issue here. In both the volume mesh and voxel mesh exports element sets for each yarn are created (and the matrix if that is being exported) These can be viewed in Abaqus CAE. There will be one element set created for each separate yarn in the TexGen model.
If you could give more information then I might be able to help more.
Best regards,
Louise

[willsenwijaya]

Hi Louise,

Thank you for your reply. Attached are some of the pictures of the problem that I want to ask:
1. In the picture titled "Voxel-NoPeriodicBC" I exported my textile unit cell using the ABAQUS Voxel file option with the periodic boundary condition option set to NONE. As you can see, no separate sets are created when the .inp file is opened in ABAQUS.
2. In the picture titled "VoxelMesh-ContinuumBC" I exported my textile unit cell using the ABAQUS Voxel option and chose arbitrary periodic boundary condition (which in this case I chose to be Material Continuum). As you can see, separate sets of yarns are created when the .inp file is opened in ABAQUS.
3. In the picture titled "VolumeElement-NOPeriodicMeshing" I exported my textile unit cell using the Volume Mesh option and didn't tick periodic meshing option. As you can see, no separate sets are created when the .inp file is opened in ABAQUS>
4. In the picture titled "VolumeElement-WithPeriodicMeshing" I exported my textile unit cell using the Volume Mesh option and ticked the periodic meshing option. Then I chose arbitrary periodic boundary condition (which in this case I chose to be Material Continuum). As you can see, separate sets of yarns are created when the .inp file is opened in ABAQUS.

Is this an unresolved issue in TexGen or is it intended to be like this?


Despite this issue, I still proceed with the volume mesh option using any arbitrary periodic boundary condition such that I can mesh the yarns with tetrahedron element and so that I can have the ability to choose different yarns independently. However, every time I tried to run a job using this .inp file, I keep getting the same error messages as can be referred to a picture titles "error in ABAQUS when using volume mesh export option"

Thank you very much

[willsenwijaya]

Here are the some of the remaining attachments

[louisepb]

Hi,
The element sets are created even when no PBCs are specified. If you expand the Assembly section and look under Sets then you should see the matrix and yarn sets.

If you are trying to run the .inp with the equations and PBCs as specified from TexGen from CAE this is probably the cause of the errors. The equations used as, for example the one below, use node sets with multiple nodes. In this example the equation is linking the nodes on two edges of the domain. It is a limitation of Abaqus CAE that it cannot run these sorts of equations. You need to run the job from the command line.

*Equation
4
Edge11, 2, 1.0, Edge9, 2, -1.0, ConstraintsDriver1, 1, -1.96962, ConstraintsDriver5, 1, -0.22

I hope that helps,
Louise

[willsenwijaya]

Hello Louise,

Once again thank you for the reply. Yes, I just realized that set definitions can be found under the assembly module. Thank you for pointing that out.
One more thing, I tried to run my textile compaction simulation in ABAQUS based on the "Volume mesh export option" with various seed size from coarse to very (very) fine and I kept getting common errors and warning messages as can be seen in the attached pictures. This is definitely something related to the element quality (the .inp file from TexGen) instead of the way I set my simulation. Any advice on this? Thank you very much!

[louisepb]

Hi,
You could try changing the merge tolerance. This specifies the size of gap between yarns which will be ignored, ie the yarn meshes would be created in contact with each other at distances of less than the merge size. This can avoid thin, misshapen elements between the yarns.

Best regards,
Louise