A Workflow for Reducing the Time Needed to Share Topology in Large CFD Models
Hello everyone, this is Mohsen Seraj from Ozen Engineering. Today, I want to introduce a workflow for sharing topology in Ansys Discovery efficiently.
Introduction
In large CFD models, sharing topology can be time-consuming due to the numerous faces and edges involved. This is especially true when dealing with both solid and fluid zones. I will demonstrate a method to accelerate this process by using a smaller model as an example.
Initial Workflow
Let's consider a model with a pipe containing multiple solid bodies. Typically, you would:
- Go to the Prepare tab and extract the volume to define the fluid zone.
- Cap the two ends and choose the interface to extract the volume.
- Hide the solid part and tube to view the volume domain.
This approach works well for models with a small number of bodies, faces, and stages. However, for larger models, a different workflow is more efficient.
Alternative Workflow
Instead of sharing topology for the entire model, follow these steps:
- Share topology only between solids, without including the fluid volume domain.
- Define the two ends as named selections: Cap End 1 and Cap End 2.
- Save the file in PMDB format and send it to Ansys Fluent Meshing.
Ansys Fluent Meshing
In Ansys Fluent Meshing, perform the following:
- Read the PMDB file to import the geometry.
- Generate the surface mesh and accept the default sizes.
- Cap the ends and extract the fluid region.
- Create the volume mesh and generate the polyhedral mesh for the fluid domain.
This process creates shared topology between the fluid and solid zones efficiently.
Application to Large Models
For very large models with thousands of edges and faces:
- Remove the volume domain before sharing topology.
- Perform shared topology only between solids, reducing the time significantly.
- Use the PMDB file format for meshing and achieve conformal mesh at the interfaces.
Conclusion
This new workflow reduces the time required for sharing topology in large models. Instead of handling everything in Ansys SpaceClaim, you can:
- Create shared topology between solids in Ansys Discovery or SpaceClaim.
- Use Ansys Fluent Meshing to create the volume and fluid zones, and generate the conformal mesh.
This method is particularly beneficial for models with hundreds of thousands of stages and faces, reducing the process from days to hours.
For more information, please contact us at Ozen Engineering.
A Workflow for Reducing the Time Needed to Share Topology in Large CFD Models Hello everyone, this is Mohsen Seraj from Ozen Engineering. Today, I want to show you another workflow for sharing topology in Ansys Discovery.
If you look at this model, for example, as you can see, we have a pipe that we have many bodies, solid bodies inside that. And then for sharing topology, we have maybe thousands of faces and edges to be shared. If it is a CFD problem, then we need to also build the volume here.
Besides the sharing faces and edges and the interfaces between solid and solid, also we need to share the topology between fluid zones and also the solid zones. So, this may take a very long time when we have many numerous phases and stages.
So, I'm going to show you how to accelerate this procedure, and besides, instead of sharing topology for everything here, we can have another workflow that I'm going to talk about in this video. So, instead of working on this very large model, I just cut it into a smaller model.
As you can see, we have a pipe that we have solid bodies inside that. One way is that I go to the Prepare tab and extract the volume for defining the fluid zone. So, just work on the two ends to cap it, and then for interface, choose this one and extract the volume.
So, if I hide the solid part and the tube, you can see that this is the volume that I have, for example, if I have a section of that, you can see that here I have the solid bars in the middle along the axis and around it, this is the volume domain that we have.
So, in this kind of problem, it is easy to work with when we have a small number of bodies and faces and stages to be shared. If you want to share, it is easy to go and just do everything for the shared topology here. So, let's do it.
Okay, you can see that everything is shared here because it is a small number of bodies and a small number of faces and stages compared to this one that we have thousands of stages and faces to be shared. So, let's do it in another way.
In this small step, the next step is to just send it to Ansys Fluent Meshing. But let's skip and remove the volume part and just share the topology here. Share the topology here only between solids, as you can see. Only between solids, we don't have a fluid volume domain.
And let's define the two ends named selection as Cap End 2 and this end Cap End 1. And so, we did the shared topology so far only for the solids. If you can review that, and we don't have the fluid volume domain here.
Now, for sending that, instead of going directly to watertight geometry, we can go for another one that we call PMDB. We save this file with this format. Okay, just give it a name, Share Topology.
Save it, and now we go to Ansys Fluent Meshing with this file and see that how we can perform another workflow that I told you. This is the PMDB file format that I sent to Ansys Fluent Meshing. Read it. This is the file that we have, the geometry, as you can see, on the solid parts.
No need for local sizing for this video. Let's generate the surface mesh and accept the minimum and maximum sizes for the surface meshing. This is the surface meshing as you can see.
For the described geometry, we say that we have only solid regions, say yes to capping, and extract the fluid region, and no to the rest for the shared topology, multi-zone, whatever. Described geometry, now we need to enclose the two ends. Then we need to do this to extract the volume domain.
These two. These are the faces that I already defined in Ansys Discovery for capping. So, let's do capping. So, you can see that now the cap surface is generated. This one. Now it understands that it needs one fluid region. Say yes. Now, creating the region, the fluid region.
So, you can see that these are the solid parts. This is the fluid region. Now we have it. Add bonded layer, let's leave it for now, go to generate the volume mesh, accept the default values for this case, and say generate.
Now, if you look at the model and meshing, you see that this mesh is a polyhedral mesh that I created. This is exactly the fluid domain that we have. Okay, you can see that everywhere I have the volume fluid zone. So, it created, which is good.
So, basically, I created shared topology between the fluid and the solid in a new workflow. The new workflow is like this: I share the topology between solid bodies in Ansys Discovery or SpaceClaim, and send out the file with this format for Ansys Fluent Meshing.
As you can see, there is no volume fluid here, there is no fluid domain here, then back to Ansys Fluent Meshing, I create the volume mesh, the fluid zone, and conformity for the meshing happens here, the interfaces between the solid and the fluid.
Okay, so I hope that this workflow can help you to make it much faster when you are dealing with a very large model that has thousands of stages and faces to be shared. Let's check this method for a very long model that we have.
You can see that we have hundreds of solid bodies, with each one also having many other solids. Here in this model, we have thousands of edges and faces to be shared among the solids and also here I created the volume by extracting the volume here, so I created the fluid domain here.
So, we have a tube, as you can see, this is the tube that I have, this is the fluid, and these are the solids that we have. So, as you can see here, if we go to the tube and make it transparent, so you can see that.
So, if you want to do the shared topology here between everything, between solids and between the fluid domain, it will take a long, long time. So, I stop the video here, and after finishing the shared topology, I will be back to you. Okay, it took 5 to 10 minutes to share the topology.
As you can see, about 2,000 faces, 30,000 edges. So, if you want to do everything together here, it will take about 5 or 10 minutes. And then, after that, you need to send it out for meshing.
But now, what we are doing here is that if I choose to get rid of the volume domain, this is the I will remove the volume domain that I have. So, I remove it from the body from the modeling that here I have. And then I will do again the shared topology.
It took about a couple of minutes, which is much less than when we have the fluid zone and the solid zone together, and then we can send it with a PMDB file format for meshing and finish the sharing topology and having the conformal mesh at the interface between fluid zone and solid zones in Ansys Fluent Meshing.
Okay, back to the small model. Okay, I just added a boundary layer here. So, you can see we have inflation layers there. Besides the conformality, it is like we are performing the sharing topology as before, but with this new workflow that you are seeing.
Okay, you can see this boundary layer is also created here, and also for the other side. So, let's send out this, first save it, save the mesh, and send out this to Ansys Fluent. We want to verify the splitting of the walls between the fluid and solid, and the interface between them.
For conjugated heat transfer, we need the wall and shadow walls. This is the model. Now, let's look at the boundary conditions for the walls. See here, you can see that we have wall and shadow walls.
That formation of this, in this way, we can verify that the walls also split at the two sides for the fluid and for the solid parts, and the interface between these two zones. So, it is also ready for conjugated transfer if we need to do this.
So, hopefully, in this way, I could, with this new workflow, you can decrease the time for sharing topology, and instead of doing a sharing topology between every part of your model, solid parts, and fluid domain inside Ansys SpaceClaim or Ansys Discovery, you can just create a shared topology between solids in Ansys Discovery or Ansys SpaceClaim, and then use Ansys Fluent Meshing to create the volume zone, the fluid zone, and then you can create the conformal mesh.
Please be sure that even here in Ansys Fluent, you can see the splitting of the walls at the interfaces between solid and fluids. And in this way, you can reduce a lot of the time. We have some applications that we have very large models with hundreds of thousands of stages and faces to be shared.
If we wanted to do this everything in a structured topology only in Ansys SpaceClaim took days. But we verified this workflow that we can do the shared topology, and creating conformal mesh, and the meshing volume, meshing everything together, it is just a matter of hours.
So, hopefully, you enjoyed watching this video. Please contact us at https://ozeninc.com/contact for more information.
