Learning Forum

[peteroznewman]

The global size function is set to Adaptive gives this mesh.

When the global size function is set to Proximity, the default is to put 3 elements across the gap. A different value could be input.

 

[Jimmyhan]

I dont understand, why not use size to make the thin part mesh?

[peteroznewman]

A single solid element across a wall thickness does not provide a sufficient number of nodes to capture gradients through the wall thickness. That is the point of this meshing tip.

When you say "thin part mesh" do you mean a shell mesh?  Shell elements are very good at capturing bending of thin structures and would be an alternative to this solid element model, however, there is work to be done in a geometry editor to create the sheet body to replace the solid body.

[Jimmyhan]

I dont have more experience on this kind of meshing. I just want to show my idea to you. from my opinion in this kind of situation I will cut out the small parts and size their edges firstly, and generated others after that. As you know in size setting you can set what a portable mesh you like.

[RHauck]

Hi peteroznewman, now there are some updates and new releases are available.

Where is the size function now located, in ANSYS 219 R2?

Thank you!

[peteroznewman]

[RHauck]

 Ok, thank you! It works if the part is a solid. How does it work if misdsurface is using?!

[peteroznewman]

Shell elements on a midsurface are assigned a thickness. A shell element has equations incorporated into its formulation to account for bending without needing multiple layers.  Solid elements do not, which is why you need multiple layers of solid elements to accurately represent bending in thin walled parts.

[rgarcia60]

Hi Peter,

I'm struggling to get at least 2 elements in the through-thickness direction while maintaining hex elements in the pipe shown below. Currently I have 1 element in the thickness direction. When I use proximity either in the global mesh size or in local mesh size I can never get 2 elements or more in the through-thickness direction (mesh settings image shows proximity off but I have tried it on many times). The inside face of the pipe has a shared topology with the inside body (fluid). Any other techniques to achieve this?

Warm regards,

Richard

[peteroznewman]

For a sweepable body such as a pipe, apply a sweep method and pick only one body. Select a Source face in the Sweep details. Then right click on the Sweep and select Inflate this Method. Now you can pick a boundary edge of the face you just picked, either the inner or outer or both. In the Inflation details, you can request 1 or 2 inflation layers.

[Emad64]

Hi Peter,

I'm modelling a T shape steel profile embedded in concrete with 4.2 mm thickness. I use shell mesh for embedded steel. But I have a problem with the connection between the shell mesh and solid element. I followed your instruction according to this post. I considered half shell thickness distance to eliminate additional mass, I also split the surface body to achive good meshing. But still struggling with node matching! I am wondering if I have to change the sell mesh to solid element to achieve node match? I would appreciate if you could advise me.

Thank you in advance.

Kind Regards,

Emad

[peteroznewman]

Did you change the behavior from Soft to Hard on the Edge Sizing mesh controls?

[Emad64]

Hi Peter,

Thanks for your reply. It works and I achieved nice mesh.

Kind regards,

Emad

 

[rgarcia60]

Hi Peter,

When I try inflating the sweep method, the inflate method is automatically invalidated with a cross. I believe this happens because I specified the sweep method as automatic thin.

The reason I used automatic thin is that I couldn't manage to successfully mesh the pipe with the other src/trg selection conditions. Would you happen to know why this pipe seems unmeshable with normal sweep conditions assigned? If I can correctly assign normal sweep conditions then I bet I can inflate the pipe with no issues and get 2+ elements across the thickness.

Also, I created a recent post where I tried this same geometry but instead of using solid elements for the pipe I used shell elements (in order to avoid needing 2+ elements in the thickness direction). The problem with this set up was that I couldn't get a conformal mesh between the pipe and the inside body, and by the responses I got in that post it seemed to me that it wasn't possible to match nodes between shell and solid elements due to their nature. But according to your discussion with Emad64, conformal mesh between solid bodies and midsurfaces is still recommended and not an issue for Ansys. Can you confirm this statement? Why couldn't I get a conformal mesh between them in that scenario?

Regards,

Richard   

[MehdiPishbin]

Hi Peter, everyone

Hope you're doing well,

I'm working on a project, analyzing fluid passing among two disks which one is fixed and one is rotating. The clearance between disk is very small (about 8 microns). The profile between two disks is shown in below and the problem is how can I mesh this very thin profile as for instance 10 elements across the wall thickness of thin part. I tried your tip and this is not working. Give me some tips.

Thanks

Mehdi

" alt="">

[peteroznewman]

Mehdi,

You are going to have to split the body to get more control of the meshing than is possible with a global setting described in this discussion. I suggest you open a New Discussion.

Peter