Mesh gradiency problem

  • 40 Views
  • Last Post 14 September 2018
  • Topic Is Solved
ahmadzaki posted this 13 September 2018

Hello,

I've been having some problems with forming a structured mesh around a building; the domain is inside and outside the building. The geometry was sliced using the building faces, then meshed with Ansys Mesher. The mesh specifications  were as follows:

Global Mesh: Adaptive, 200mm element size

Local Mesh:

Multizone, Hexa. program controlled.

Body sizing: sphere of influence, 10 mm

The Problem:

As shown in fig.1, the mesh was gradient from the center to the outer domain faces except for the backward region.

fig.1

So I sliced the backward region so the backward region is at the same distance as the front surface from the centre (fig.2, 3). The mesh behind the center (building) was refined, yet the rest of the domain was still uniform.

fig.2

fig.3

 

I will be gratefull for your support. Thank you.

 

 

Order By: Standard | Newest | Votes
rwoolhou posted this 13 September 2018

I think it's a function of the order of meshing and sizing. Changing what order you mesh in may help, but it's also worth looking at the overall set up. Edge sizing with clustering might help, but may cause other problems. 

Look at the edge sizing on the top plane: you have a small size set near the building, and let it grow away from the building. This works well in the building volume, but gives stretched cells further away in the volumes in the x & y directions (assuming z is up). With a mapped mesh, you're going to finish up with stretched cells or a big jump in cell size in the adjacent volumes (as you're seeing in the grey & it's mirror volumes). 

 

Whenever I've looked at buildings I've not worried about a structured mesh as I want to cluster cells around the building & wake region (and nearer the ground) but want a coarse mesh in the far field. 

What you haven't said is what you need from the model: this is important as it guides how we mesh the model, and what settings we need in the solver (which may further define how we build the mesh). 

  • Liked by
  • ahmadzaki
ahmadzaki posted this 13 September 2018

Thank you for your response.

I think that what I needed is what you mentioned, which is finer mesh around and inside the building and near the ground. I tried edge sizing (red line) on the top plane with the same biased manner as shown below. However, I get this message every time I try.

I also tried changing the order, for example, I started with body sizing instead of multizone. Unless you suggest specific mesh types in a particular order?! Shall I stop using body sizing and start manually edge size each component so that all edges are biased towards the building and ground?

I've been stuck in this for almost three weeks now (I've tried a lot of different things).

Thank you for your support.

rwoolhou posted this 14 September 2018

Setting just that edge won't help as the mesh may skew depending on the order you mesh in: you may need to set all the sizes.  The warning just means you're not recording the mesh process so can't re-run it: look for selective meshing in Help. 

In the interests of getting some results I'd suggest inflation on the building & ground and tet the volume. Maybe put a volume around the building & it's wake to retain a finer mesh.  Then talk to your supervisor and see he they can talk to support or send you on training: as ANSYS staff I'm very limited in how much help I can give on a public forum. 

  • Liked by
  • ahmadzaki
ahmadzaki posted this 14 September 2018

Thank you for your kind support and concern. I've been trying and I used edge sizing on the bottom edges (same as building height). Then I used body sizing for the whole domain. Its like what you said "Changing what order you mesh in may help".

The mesh problem was solved and the gradience became symmetrical.

 

Thank you

Ahmad

Close