## Fluids

Topics relate to Fluent, CFX, Turbogrid and more

#### Modeling Small Fluid Domains in CFX

TAGGED:

• vinnakbm
Subscriber

Hello, I'm trying to perform a transient analysis in CFX of a miniature fluid domain which has a rotating spindle (modeled using immersed solid & rigid body solver). Diameter of the cylindrical fluid domain is in the order of 2 to 4 mm and height is 10 mm. I'm interested in the motion of the spindle due to the fluid flow. My simulations are converging without solver errors. However, when I change the mesh size and run the simulations for mesh independence study, I'm seeing that the results are changing a lot. I'm wondering if there is a limit of some sort in Ansys on how small the domain can be? Is my domain too small? Any help is appreciated.

• NickFL
Subscriber

As long as the continuum is maintained (think back to your very first day of fluids class), modeling it with the control volume approach is valid.

What you are comparing when looking looking at the results from two different grids? How are you modeling the immersed solid? If there is not a fitted grid around the body, then the solution quanities are interpolated onto the surface. This could be the cause of deviation.

• Rob
Ansys Employee

There is a limit but you're a ways off it. The value you're looking for is the Knudsen Number.

• vinnakbm
Subscriber

Thank you Rob, I'll look at the documention for Knudsen Number. But are the cappilary effects taken into consideration since the domain is in the range of capillary length of water?

• vinnakbm
Subscriber

Thank you for your response. How are the surface tension effects included in the analysis (dominant at scales lower than the capillary length of ~3mm for water and my domain is in that range). Water is my working fluid and I’m interested in the translation and rotation of the spindle. I did not specifically create the fitted grid around rigid body. Just used the default adaptive mesh with small element size of 0.1mm to start with so that I get approximately 20 elements along the diameter of 2mm. I then refined to 0.075mm and increased to 0.11mm element size. Motion of the spindle is very different in terms of angular velocity magnitude and direction – CW and CCW. I have a monitor set up for the angular velocity and translation and am stopping the analysis when a steady state is reached for these output variables.

• Rob
Ansys Employee

You'll need a fine mesh as you're going to see some interesting free surface shapes. Read up on VOF to see how the solver works.

• vinnakbm
Subscriber

Thank you Rob. My domain is comletely filled with water there is no air in it. I’m a little confused about free surface shapes. Can you please explain?

I wanted to add: there is air as it gets filled up initially. But I’m interested in the spindle movement after the domain is filled. So, I did not model the air in it. The domain is 100% water. So, surface tension does not play a role, maybe?

More details from previous post for reference: I did not specifically create the fitted grid around rigid body. Just used the default adaptive mesh with small element size of 0.1mm to start with so that I get approximately 20 elements along the diameter of 2mm. I then refined to 0.075mm and increased to 0.11mm element size. Motion of the spindle is very different in terms of angular velocity magnitude and direction – CW and CCW. I have a monitor set up for the angular velocity and translation and am stopping the analysis when a steady state is reached for these output variables.

• Rob
Ansys Employee

If it's full of water there is no surface tension effect: that's only a factor at the free surface. So, in your case it's going to be viscosity etc that's effecting everything. If you're refining the mesh, how well resolved is both the gap and surface curvature?

• vinnakbm
Subscriber

Do you mean the gap between spindle and wall that is filled with fluid? I did not do any additional refinement at the wall. I used the same element size for spindle (modeled as immersed solid, using rigid body solution) and fluid domain. I thought that the velocity of fluid is matched with the velocity of the body for the overlapping nodes. I did not change the momentum source scaling factor, using default 10.

• Rob
Ansys Employee

I don't know much about CFX. You do want to resolve the curvature as well as near wall resolution.

• vinnakbm
Subscriber

Thank you Rob. I’ll try improving the near wall resolution. Is there someone I can tag to help with CFX?

• Rob
Ansys Employee

I'll give him a nudge, you can't tag people (yet).

• vinnakbm
Subscriber

Thank you!!

• DrAmine
Ansys Employee

What do you mean with your results are changing a lot? Can you show a plot?

Aslo I recall that partitioning might be critical here. Please check the Ansys CFX Modeling guide as running in parallel might be bit sensitive.

Again assess the convergence of every case before looking into the results.

• vinnakbm
Subscriber

Hello Dr. Amine, The change is in terms of magnitude and direction of spindle rotation. Attached are some plots. I’m not running it in parallel and all the residuals are under the tolerance of e-5 specified. Time step 5e-6 s unless stated. The mesh details and the monitor plot of Angular velocity Vs Accumulated time step are shown below for 3 cases.

• DrAmine
Ansys Employee

Aslo the medium mesh is completely far off and I recommend looking into the setup and the other results too.

What does happen if you keep refining the mesh?

• DrAmine
Ansys Employee

Addtionally please check Near Wall Treatment for Immersed Solids Section. Boundary Layer resolutionis required.

In general Immersed solid approach is applicable when forces on immersed body are  pressure-dominated because the visous effects are generally not well captured.

• DrAmine
Ansys Employee

I sincerly recommend not having the immersed solid at all and using Rigid Body Solver with Mesh Smoothing. There is a tutorial showing how to do that for Buyo.

• vinnakbm
Subscriber

Thank you Dr. Amine. My refined mesh analyses are running. I do not have steady state yet but the patttern for angular velocity is as expected – similar to b (not cyclical about 0). I’ll check the near wall treatment. I did go through the buoy tutorial. But the displacements in that are small. In my case the angular velocity of immersed solid is around 4000 rad/s which is ~39000 rpm. I’ll also be running some scenarios where the the rpm will get higher. Will the buoy approach work? The other question I have is about the Courant #, for high rotations like this is there a target courant # (<1?)?

• DrAmine
Ansys Employee

Time Step Size to be at max 0.01/Angular Velocity.

If you require more flexibility you might have a look into an Ansys Fluent Solution deploying Oversert Mesh.

• vinnakbm
Subscriber

My understanding was that CFX is more suitable for turbomachinery type applications. Since my system has a rotating spindle (at a high rpm), I thought CFX would be a good fit. Is there a specific reason to use overset mesh in fluent instead of immersed solid approach for this case?

• NickFL
Subscriber

CFX and Fluent solve the same equations. CFX has been considered the "Turbo" package because of historical reasons, but Fluent is equally capable at solving turbomachinery.

Why are you attempting to use the spindle as an immersed solid? Is there a reason a body fitted grid approach would not work? Is a full transient necessary? Because at 39k rpm you are going to need a tiny timestep and a lot of computational resources to bring it to a steady state. Could you obtain the results you wanted using a steady state model and one of the rotating interface models?

• Rob
Ansys Employee

To follow on NFLynn's comment, unless the spindle is non-cylindrical the sliding mesh or reference frame models in Fluent are sufficient. CFX will have an equivalent.

• vinnakbm
Subscriber

Thank you for your inputs! I'm using a time step of 2e-6 sec. The spindle has vanes and other features, so it is not a simple cylindrical geometry. Also, I found CFX being used in some of the reference journal articles. So, I modeled in CFX. I picked immrsed solid as I do not have to subtract the spindle from fluid domain like in fluent ( I was not aware of overset mesh at that time). If I do subtract the rotor body, it leaves 0.25mm circumferencial regions around it i.e. the clearance between spindle and wall. I do not have space to define a stationary and rotating domains. I'm using the rigid body solver to get rpm as an output, as I want fluid to move the spindle. In CFX, if I don't use rigid body solver, RPM has to be defined in the set up.

• DrAmine
Ansys Employee

Immersed solid is a nice tool to model that but again the near wall treatement for immersed boundaries is critical. For that reason we recommend to use mesh motion with smoothing on top of the rigid body as it is known to be more accurate, though less flexible compared to Immersed Solid.

How does your mesh actually look alike? Can you please share a couple of screenshots espcially near the Immersed Solid?

• vinnakbm
Subscriber

This is from the fine mesh analysis that is running. The inside body is spindle. Used adaptive unstructured mesh.

• vinnakbm
Subscriber

Inlet region

• Rob
Ansys Employee

Those gaps look big enough to add a sliding interface to me.

• vinnakbm
Subscriber

The gap in this zoomed image is 0.25mm. Is that big enough?

I'm trying to understand if I should abandon CFX altogether and start from scratch in Fluent. If both are solving the same equations, I'm not convinced that Fluent will solve all the issues. I have a some older/reference analyses that are in CFX and am trying to follow a similar approach. Any advice on how I can improve my present CFX analyses so that I do not lose the time and effort already invested is greatly appreciated. thank you!

• NickFL
Subscriber

Yes, 0.25 mm can be divided.

If you are comfortable in CFX there is no reason to switch. The biggest questions are: Is it necessary to do a full transient analysis or can a mixing interface model work? I would abandon the immersed boundary all together if time is critical. It would be interesting to compare both the immersed body approach to a mixing interface approach and identify potential sources of error between the two.

• Rob
Ansys Employee

The size of gap is more dependent on scale than actual dimension. So, a 0.1mm gap in a 10mm domain is probably OK, but in a 100m domain may give you an excessively large mesh.

• vinnakbm
Subscriber

Thank you for the inputs. When you say, if time is critical, does it mean immersed solid is not suitable for transient analyses? I'll look into mixing interface model.

• NickFL
Subscriber

The immersed solid method is valid for transient analysis. The main reason why I would suggest moving to a body fitted grid and using an interface model is because of the rotational speeds at which you are simulating. It was discussed above how we will have to have a fine mesh near the body location to get an accurate representation of the forces on the body. But the down side of this is, with such a quick rotational speed the immersed body with swing through a large number of cells per timestep. This is not really what we want and will cause us to reduce the timestep even further, making our “wall-clock” time even longer.

The approach I suggest solves for the fluid near the rotating body in a rotational frame. This is then patched onto the stationary body using an interface model. This is typically done with rotating machinery problems at least as a first step. I would suggest looking closely at these models in the documentation and here: https://bakker.org/ . If you are trying to see a specific start-up vortex impinge against something in the stationary domain, these mixing interface models will not be appropriate. But even then you could move to a full rotating transient and basically get the same information you would as your immersed boundary model with the advantage that we do not have to consider how the body moves through the grid because the grid is moving with the body.  Even if I went to a full rotating transient model I would first use one of the mixing interface models to get a “steady” solution as an initial condition for the transient simulation.

(ANSYS Employees, I hope it is OK that I linked an outside website. But Andre is a former colleague and all).

• DrAmine
Ansys Employee

The main reason remains for me the way Immersed Solids treats the near wall cells that has an impact on the accurcy of anything related to viscous effects. Besides that NFLynn highlighted the aspects dealing with temporal resolution required. An Interface Model or complete Transient Sliding Mesh (Transient Rotor) are good alternatives. Please have a look into the Ansys CFX Tutorials like Axial Turbine Stage.

• vinnakbm
Subscriber

Thank you very much!! This is very helpful. Appreciate all your inputs. I'll look into those tutorials and documentation.

• Rob
Ansys Employee

@NickFL external links are fine, it's when they're external links to our documentation that we object. Well, we also object to links to gambling sites, banking, real estate (I suspect we won't like virtual estate either) and young ladies of dubious virtue.....  Thanks for posting. I remember Andre from the Fluent days.

• Liam Smith
Subscriber

While there is no hard limit on the size of the domain, certain factors can affect the accuracy and stability of your simulations. Verify that the fluid properties used in your simulations are appropriate for the small-scale domain. If necessary, consider adjusting the properties, such as viscosity, density, or thermal conductivity, to match the actual conditions.

• DrAmine
Ansys Employee

If surface tension effects to be included I would start then recommending to move to Ansys Fluent.

• vinnakbm
Subscriber

Thank you all !!