Blade Modeling Application Part 2: Workflow from an Adjustable Blade Generation to Simulation

Blade Modeling Application Part 2: Workflow from an Adjustable Blade Generation to Simulation So, the second part of this workflow starts with bringing in the new DesignModeler and uploading the CAD that we generated. Let's name this as... similarly, DesignModeler geometry.

Let's load the NDF file that we have already saved in the previous animation video. It was named as TestTour, remember? So, immediately the flow path and the corresponding blades are already written.

If you remember, we set the number of blades as 3, and that's why we have 3, but we have always an option of changing the number of blades, etc. So, let's continue with the further settings.

So, when we click the main blade 1, we are given different plots on the far right side, and that's for sure we actually have the blade profile with a certain number of points, and we can change; we can move these number of points; we can drag and drop, which means we can modify the blade shape immediately from this plot.

But before doing anything, let's save the project. It's one of the good housekeeping habits. So, let's review the section here on the lower left. And let me actually bring that up a bit so we can see better here.

Now, as I mentioned, the flow path and the number of the blades are put here, and now we have an option of changing the hub and the shroud blend. Remember, in the original design, we had a flat with some radius on the hub region. So, let's make that happen here.

So, on the Hub Blend, the blend option will be with, let's assume, constant radius. And now, when you select that, there are a few options that are given to us. And we can change the ball radius, angle, etc.

If you don't know what this is going to do, you can leave it as it is and perform it and see what happens. So, let's do that. See if I don't make any change, it already put the flat, but this is, I think, quite unrealistic. Anyhow, we can definitely make a modification.

But again, before playing with the numbers, let's confirm the units. We initiated with the original model with inches; that's why we have to change this to inches again. And let's make this or test it with text definition if you can, or other languages, and forward it automatically.

On the shroud side, depending on the design, we have an option of creating a clearance or keeping as it is, if that's a shroud or impeller. Let's explore the impeller with a clearance between the tip of the blade and the shroud, of course.

To add the shroud tip clearance, we're going to have to go to the main blade and open the main blade clearance and rotation options. Now, we have different options here, of course, it can be no, it can be a layer, or it can be a gap.

Now, we're going to have a gap, and we can specify different levels of gap depending on, of course, the design we have on the leading edge to the trailing edge, so we have options of having two different settings here.

Let's make a 0.05 gap on here, and then maybe a tighter gap towards the end of it. Again, it's totally up to us how to make this, and let's see if these numbers are going to work. And even though it's not that visible, but now we have actually a varying tip clearance, which is already set.

So, let's explore how to make other modifications. We started with the three blades, right? Now, let's try to change it and see how fast we can make that happen. So, instead of three, I wanted to have four blades. And let's generate it, and we have our four blades in front of us.

It's exactly the same blade replicated.

And on this side, as I mentioned before, this is the blade profile, and what we can do, these are the points that describe this profile, and we can add points, we can remove points, depending on how we would like, and for that, right-click and insert point, and I'm going to, for example, put one point here, and I'm going to insert another point here.

Let's assume I want to define this region better. And as you see, I didn't put it exactly on the profile, that's why this profile doesn't look as smooth as it was. So, what I can do is actually I can drag and drop, as you see, it's actually fairly easy.

I can make modifications, I can move the point from here to there, too, and make modifications on the blade profile. And once I do that, it's going to be reflected on the blade shape. Let's explore some change on the blade shape. As I'm trying to do it here, it's...

yeah, I think this is a better smooth profile, and let's generate it. And it's generated, so it's that easy to perform blade modification. So, let's assume we are happy with this design, and we want to move on to the further stages, which is going to be meshing, as well as the model settings.

And for that purpose, we will go to the Workbench phase and then add those components. So, let's bring the Workbench file here. Remember, this was our original geometry, where we generated the blade profile, and this is where we read it in.

Let's get the TurboGrid and attach it to this geometry and open it. So, the TurboGrid brings the single passage of the blade, so that we can play with it, since it's symmetric for all of the others. This is the corresponding portion of the single passage.

All these Turbo Machinery settings are already predefined. We have the hub surface, we have the shroud, and we have the inlet region defined, we have the outlet region defined, because ultimately we will need those in the further stages.

So, the mesh is not generated yet, it's just red in there, and probably it's visible here. What we're going to do is we're going to update the mesh here. So, the mesh is generated, and we can understand that with this green checkmark. Let's see the TurboGrid file.

And as you see here, from this plane between the hub and shroud, and this is actually a pretty nice structured mesh with some prism layers attached, we can definitely play with the features of this, and you have already noticed, we have a mesh error, which demonstrates an orthogonality problem here.

So, playing with the mesh features, such as reducing the factor base, in this case, for example, that gets rid of some of the errors that you can have. So, now we have a good mesh with no errors, and we can make it coarser or finer, playing with the method and the scale factor, etc.

So, let's say we want to make a finer mesh. I want to change the file size factor from 1 to 1. 5. And let's see how much of an impact that has on the mesh. As you see, it's actually pretty fine. When I zoom in, we have good numbers of prism layers. Let's zoom in here.

In a very nice manner, actually, put around the blades. So, for this demonstration purpose, I will get to the coarser one and continue with that. So, let's bring the CFX into the Workbench project and connect to the TurboGrid. Let's double-click that.

So, to continue with the turbo settings, we will enable the turbo mode here, and we are asked what type of machine; let's keep it as a pump.

Coordinate frame is put rotational axis is Z direction in this case, and now we have the rotating component, which is going to be named as R1, and what kind of fluid we're going to use; we can use air, water, or totally custom. Let's continue with one of the selections.

Reference pressure, we're not going to be interested in the heat transfer, turbulence; let's keep it a shear stress transport model. And in Net and Outlet templates, we can choose one of the most relevant ones for our application.

I will go with the mass flow inlet and pressure outlet, and I will put the mass flow rate, let's say 0.1 kilograms per second, and offload static pressure is let's assume it's as is.

So, it automatically recognizes the interfaces and the boundaries, and with that, our turbo model is available with the corresponding inlet and outlet sections created, and with the proper settings. There is one thing that the user should pay attention to.

Now, we are considering only, in this case, we have 4 blades, and a quarter of the model. So, if you want to specify the flow rate, you have to pay attention to that.

And I will apply this mass flow rate to all of the sectors if it is considered as 360. And that's pretty much it in terms of the settings. So, let's create an expression for the pressure generation that we will monitor.

So, over here, I want to create a new expression, head, and I will type it as mass flow average absolute of pressure. If you're not aware of what to do here, in terms of, for example, the location, let's take a look at the locations.

We have R1 outlet minus, let's copy this, paste, it's going to be R1 inlet, and the software will return Pascal to us, and if you would like to make a modification on the unit, we could do it over here, or we could still keep it as Pascal, however we like. Yes, there is no error with that.

And let's create a monitor point with that. Thank you for watching. It's going to be an expression, and it's going to be head. Okay, all right, oh okay, that was a mistake. It's good that it's recognized already as a mistake, so I made a typing error here. It's not flow, it's flow. Beautiful.

Okay, now it's recognized. So, the error should remove itself. And with that, I guess we are pretty much done with the settings.

What we can do, of course, in terms of the solver control, we can change the number of iterations, and time scale factor, depending on how we would like to do, and the residual target, etc. But for this purpose, let's keep all those settings as is.

And as you see, the setup is already done here, and we're going to continue with the solution. So, I had some basic settings of double precision, and also the parallel processing. Let's initiate the simulation.

Simulation started, and our monitor point, which is the pressure head generated, is shown here. It's pretty stable. So, let's assume we have a stabilized solution, and we would like to perform post-processing. So, the solution is about to be completed, and I will turn the results on.

Let's bring the results here. You always have an option of bringing a new results tab here, attached to the solution.

Sometimes you may choose to do that, and if you want to perform detailed post-processing, and you don't want to overwhelm everything in one module, so you can actually separate the things, and it would perhaps be easier to even open that post-processing session at that manner.

So, you're always free to add a new post-processing tool, such as this. Anyways, let's go back to the initial results session we had. So, we loaded this, and we can create some post-processing images and contours.

We can create contours with R1 blade and all the mains, and create the blade with the pressure, or we can include hub 2. We can also go to the Turbo tab to perform Turbo machinery-related post-processing. And let me initialize with all the components.

So, I have a 3D view, blade-to-blade view, from a 50% span, as you see, 0.5 indicates a 50% span. And when I change it, I'm going to go to 25% span, which is 0.25, which means closer to the hub, apparently 75, or higher than 50, is actually a cross-sectional location closer to the shroud.

We can create contours, vectors, and similarly, we can take a look at the meridional image on here, as you see, colored with the pressure. So, these are very helpful tools, and we can also add a graphical instance, for example, of R1 of four copies, as we're going to have four blades.

So, it means this is actually an unfolded version of this 360 view from the middle section of the circular cut region throughout the domain.

So, this concludes the series that we covered, generating the geometry, starting from an already available design, and creating a single blade region, and performing design modifications slightly. Thank you for watching. Please contact us at https://ozeninc.com/contact for more information.