Ansys Fluent

And we’re going to use under the component systems again the Fluent With Fluent Meshing block. Previously to this update that we’ll talk about, we would have had to first open up nTop SpaceClaim, pull in the MSH files still with their named selections associated with them, save it as a SC Docker SpaceClaim document, and then pull those into the Fluent Mesher.

So with this update, we’ve eliminated this step. We’ll launch Fluent with Meshing, with the Fluent Mesher open. We’ll under workflow select the fault tolerant machine under Import CAD And Part Management, we’ll navigate to the MSH files. With the MSH files, we’ll control-select all three. So they’re called fluid hot fluid and solid core. Select “Okay.” Units we exported in meters and we’ll select “Create Meshing Objects” at the bottom.

Before we continue on with the rest of the fault tolerant workflow, we’ll come under the outline view tab, open up Geometry Objects, and here we’ll see a list of all the MSH objects we imported. This step is pretty crucial. We need to control-select each of the bodies that belong together and essentially merge them together. So we right-click, “Merge Objects,” and we’ll just call this XX core. I’ll go ahead and do the same thing for the two fluid domains.

With those complete, there’s one more step. We’ll expand each of these. We’ll come under the face zone labels, right-click, select to create labels, select all, and we’ll create a label for each face zone. So we’re basically just stitching together the name selections and then extracting them as labels.

With that complete, we’ll come back to the workflow tab and continue down the fault tolerance tree. Internal flow through an object. We don’t need to create large caps or identified regions or closed leakages. So we’ll describe geometry and flow. This point, we only have three regions. That’s what we want to see, both fluids and the core itself. So we’ll define the cold fluid as a fluid. It’s going to be wrapped. We’re also going to wrap the hexa-core and define the hot fluid as a fluid polyhedra elements for all three. Update regions, and we’ll go and select “Choose Options for Meshing.”

Now, the default curvature and proximity are applied to all three domains. So I generally, especially if I’m doing conjugate heat transfer analysis, come into revert and edit, and I’ll remove the hex core. We’ll call this one fluid curvature, and I usually decrease these a bit. Under local sizing, we’ll select the hex core. We’ll call this core curvature. It’s significantly thinner, so we’ll reduce it to maybe 45 and maximum size. We’ll set to three. Add local sizing, and we’ll do the same thing for proximity. So we’ll call this core proximity. Go with the same values of 0.45, 3. I’m only going to do two cells per gap, so we should see when the mesh is graded only two polyhedral elements hex core. Add local sizing, select “Yes,” apply all four of those.

Now, as you get comfortable with working in Fluent and these steps, generally what I’ll do is rather than going to surface mesh, waiting, and coming and defining everything else, we can ahead of time prep the volume measure. So under cold inlet, we’ll select Mass Flow Inlet. We’ll go ahead and define the outlet and inlet for the other two as well. Now you’ll notice I didn’t define interface regions for the contacts. The reason being is when we get to the boundary layer stage, I find it easiest to have the boundary layers grow on only walls and then within Fluent itself, I’ll set up the actual interfaces. So I’ll click “Add Boundary Layers” here. I’ll select “No” that way it doesn’t start running the surface mesh. And with both the updated boundaries and boundary layer selected, I can come to “Generate Volume Mesh” here at the bottom. I’ll select “Generate the Volume Mesh.” And in this case, it would in sequence go through each of the steps.

Now just so we can see how long the surface mesh takes and the elements that created, we’ll just generate the surface mesh as its own right now. So I’ll pause the video and restart it when the mesh finishes. Okay, the surface mesh is finished. Go ahead and render it on the flu. See what that looks like. At the same time, we can see that we have about 4.7 million elements and it took about 63 minutes, so just over an hour to mesh all three bodies. So not too bad. See how the resolution looks for first pass. Not too bad. I might actually decrease it for future iterations, but overall and let’s look at a cross-section. Overall, not too bad. And we can do the same thing for the solid. And with the color coding, we can still see that we’ve preserved our name selections.

So with that, we’ll just select on “Generate Volume Mesh” here at the bottom. It’s going to move through the update boundary condition, add boundary layers, and start the volume mesh. So we’ll check back in when that finishes up here shortly. The volume mesh is finished. Just over 8 million elements. We can see the distribution between the three. Overall quality, pretty good. Took about an hour and 30 minutes to complete. Pretty dense, but for a first pass, not too bad. See what the solid looks like. Looks good. We have two or so elements in that thickness. We’ll switch to solution mode at the top left. Going and start to set up the model. Keep most of the values at default. I will change a handful of them. Turn the energy equation on. Going to change the turbulence model, K Epsilon. I’ll leave the both fluid domains as air and the solid as aluminum. But to change those, you would come under create and edit and you can navigate the fluent and other databases.

Set mass flow to 0.45, 300. Fine. Apply hot inlet 0.3. We’ll bump this up to 375. Come to the walls. And a good best practice, at least initially, is to right-click and display each of our interfaces just to make sure that we are capturing the intended interface. So that first one didn’t look good actually. But here on the left, you can there’s a handful of solid to colds. We can display this and see that we just have a random few elements that were separated from this overall body. So we’ll make this one an interface. We look at the solid to hot. Looks good. And then let’s also look at the hot to solid. Also looks good. So we’ll control select these and cold to solid. Fortunately, I captured all of this. I’m not entirely sure why that happened, but we at least don’t have the inlet and outlet sections. That’s okay. We should be able to proceed with this.

So we’ll right-click, “Label Interface,” come under “Miss Interfaces,” gold to solid, solid to cold. Select “Create.” Do the same thing for the hot. Click “Close.” Defaults of those should be all right. We’ll go ahead and start to set up the method. Start off with a handful of iterations and then see if the results look like and add some more. Just quickly view a couple results and finish off the iterations. With that start to wrap up this tutorial. Pretty uniform distribution temperature distribution across the heat exchanger as you’re moving in the primary direction of flow. Soon to come will be the integration with Star CCM. We’ll start with single fluid domains. Branch out from there.