Error When Calculating Minimum Stable Time Increment for Bottom-up Mesh

[suz_02]

I have created a bottom-up mesh using the sweep tool for this stent. However, I am having issues with being able to calculate the minimum stable time increment, as it shows this error message when doing so. I was wondering if there is a way to solve this.

 

[FEA way]

Do you have a section with material (including density and elasticity) assigned to this part ?

 

[suz_02]

Do you have a section with material (including density and elasticity) assigned to this part ?

I realised the section was incorrectly assigned, thank you for this!. I also wanted to ask for bottom-up meshes, how do you correctly identify mesh and geometry assignment? To make sure that the mesh is properly assigned would I have to use all parts of the geometry during the control settings of the bottom up mesh? Would a good sign of proper assignment be that when assigning geometry to mesh there are no yellow dots to indicate any missing parts? It is my first time using this mesh type and so I was unsure.

 

[FEA way]

The bottom-up mesh (unlike the standard top-down mesh) doesn't follow the geometry of the part being meshed. By default, it's only associated with the parts of the geometry that you select as source, target or connecting side. But you can manually associate it with other geometrical entities. You may also use the Edit Mesh --> Project tool to manually project nodes to geometry.

When it comes to section assignment, it should be enough to assign a section to the whole part (geometry). The default light green color in the Property module will confirm the assignment. But you can also check the option to create an element set when generating bottom-up mesh and then use this set for section assignment.,

 

[suz_02]

The bottom-up mesh (unlike the standard top-down mesh) doesn't follow the geometry of the part being meshed. By default, it's only associated with the parts of the geometry that you select as source, target or connecting side. But you can manually associate it with other geometrical entities. You may also use the Edit Mesh --> Project tool to manually project nodes to geometry.

When it comes to section assignment, it should be enough to assign a section to the whole part (geometry). The default light green color in the Property module will confirm the assignment. But you can also check the option to create an element set when generating bottom-up mesh and then use this set for section assignment.,

Thank you for the response! I have adjusted it as you said and it works. Does this mean that if I have used all of the geometry in the sweep, when I apply my loads and boundary conditions then it will be as if it’s applied to the original geometry?

Additionally, I do have an issue where I am finding it difficult to properly mesh this part as there are regions of oddly shaped elements and I’m not sure how to fix this. I did suspect it’s the curvature or the thickness and have tried adjusting the design slightly but I’m not sure how to fix this to make the elements more uniform. I’ve seen in papers they’ve used 4x4 hex elements and they had a very uniform mesh and I can’t seem to figure out the mesh controls to do so without making the stable time increment too small.

Any suggestions?

 

[IceBreakerSours]

Those high quality meshes aren't recreated from medical imaging scans; they are built from 2D wire-frame designs and then mapped to 3D

 

[suz_02]

Those high quality meshes aren't recreated from medical imaging scans; they are built from 2D wire-frame designs and then mapped to 3D

How would I do this mapping? The stent I’m showing here is not an image created I made this on CAD. How do you create a 2D mesh to then map it for us on Abaqus? Is this something that Abaqus can do or another software is required.

 

[FEA way]

Does this mean that if I have used all of the geometry in the sweep, when I apply my loads and boundary conditions then it will be as if it’s applied to the original geometry?

Loads, BCs, and other analysis features defined on the geometry are transferred only to the mesh entities associated with the geometric entities.

How do you create a 2D mesh to then map it for us on Abaqus? Is this something that Abaqus can do or another software is required.

Sounds like the Wrap Mesh plug-in we talked about before. But of course, you have to design the 2D pattern first and CAD software might be better for that than Abaqus/CAE.

 

[suz_02]

Loads, BCs, and other analysis features defined on the geometry are transferred only to the mesh entities associated with the geometric entities.


Sounds like the Wrap Mesh plug-in we talked about before. But of course, you have to design the 2D pattern first and CAD software might be better for that than Abaqus/CAE.

I am not able to install the wrap mesh plugin since I do not have the proper account to do so as I did not purchase the license myself. I am currently trying to create a wireframe of my stent (1D) so that I can model it using beam elements. I am finding it difficult to extract the midlines, and since you cannot emboss a edges without adding thickness I am unsure how to only extract edges. Any advice on this?