Self Intersection Fault

  • 128 Views
  • Last Post 3 weeks ago
  • Topic Is Solved
monicaagabriela6 posted this 16 February 2019

Hello,

I want to perform a CFD simulation on an axial fan. Unfortunately, the mesh failed. I checked the geometry by using the "fault detection in Design Modeler" and I found 2 faults, both of them showing the message "self intersection". However, I don't know how to solve the problem. Can anyone help me with this please? 

Order By: Standard | Newest | Votes
peteroznewman posted this 16 February 2019

Hello monicaagabriela,

Please attach the Workbench Project Archive .wbpz file to your reply so I can take a close look. 

I see there is a small change in the surface where the faults are. I may try to replace the all top faces of the hub with a single face. I expect you don't care about that detail. Right?

I will also open the geometry in SpaceClaim which has repair tools that are easier to use than DesignModeler.

Regards, Peter

monicaagabriela6 posted this 16 February 2019

Hi Peter, 

I have managed to repair the geometry and I have generated the mesh but when I am trying to open the "Setup" for producing the CFD simulation, it shows an error message like the one below, saying that I have exceeded the maximum allowable number of cells. I have also attached my workbench project. Could you please have a look and try to open the Setup in Fluent to see if it works? Thank you so much 

monicaagabriela6 posted this 16 February 2019

I have attached the project file in the comment above. 

peteroznewman posted this 16 February 2019

This site doesn't allow a .wbpj file to be attached because that file on its own is useless. If you use a .zip file, you have to put the _files folder along with the .wbpj file.

ANSYS Workbench provides a File > Archive menu selection that creates a .wbpz file which includes both the .wbpj file and the _files folder combined into a single file.

Please attach a .wbpz file as long as the file size is < 120 MB.  In Meshing, if you Clear Generated Data on the Mesh and save that project and archive it, the file size will be smaller.

peteroznewman posted this 16 February 2019

I have opened your file. I found geometry.stp in the import files folder. I am going to do some more cleanup like removing this small step on the hub.

 

Do you need these buttons kept?

How about removing all these small faces at the root and having a clean hub?

     

With cleaned up geometry, an enclosure about the solid geometry represents the rotating mesh, while a larger enclosure represents the stationary mesh.  The next step would be to add inflation to this mesh. [EDIT: For sliding mesh method, don't want Shared Topology]

  • Liked by
  • monicaagabriela6
monicaagabriela6 posted this 16 February 2019

The buttons are not necessary at all. It would be amazing if a clean hub can be created. Thank you very much! Do you mind if I ask you what kind of mesh size should be ideal for this fan? I am struggling to get a good quality of mesh for the simulation. Also, can you attach the project file here, or using a wetransfer.com link as the one that I have used before? Thank you so much!

peteroznewman posted this 16 February 2019

Is the fan in a duct or is it in open air? What is the tip velocity of the fan? Can you calculate the Reynolds Number for this model?  The Re number is used to decide the height of the first cell above the blade.

I left two planes in SpaceClaim so you can cut the domain into a 1/3 sized pie slice. If you do that and use periodic boundary conditions and do mesh matching, you might be able to cut the model size by a factor of 3 which would allow you to have a finer mesh and stay within the student limit. I'm not sure if you can do that and have a rotating mesh at the same time. The CFD experts can advise you on that.

The clean geometry is attached below with an inflation layer added and contact between the bodies to implement the sliding mesh method. However, you may require a different inlet BC.

Attached Files

monicaagabriela6 posted this 17 February 2019

Hi Peter, 

Thank you so much! That looks fantastic!

The fan is supposed to operate on a fan ring attached by a radiator. The fan ring is supposed to have a diameter of 1250 mm leaving a tip clearance of 5 mm between the fan blade and the fan ring. I want to produce a CFD simulation to compare the results against the experimental data. 

Could you please advise on what type of boundary conditions I should you use for the inlet and outlet? I have watched a couple of youtube tutorials and I know that I have to set it up to "pressure outlet", but what value should I give to the pressure? Would it be the atmospheric pressure?

Once again, thank you so much! Can you also please recommend a book or other youtube tutorials to get a better understanding about the meshing and setup? I have noticed that you've created 1 body sizing and 2 face sizing. Could you please explain to me why is it important to have face sizing as well?

Thank you so much!

 

monicaagabriela6 posted this 17 February 2019

Also, the fan is supposed to be positioned on the opposite direction. The side with the button was supposed to be the one that is attached on the radiator. Do I have to start again in order to do that or is there any quicker way to do that or it doesn't really matter? Should it produce the same amount of air flow? 

peteroznewman posted this 17 February 2019

Hi MonicaGabriela,

What is the length of the fan ring? The fan ring should be in the model. Is the fan ring in a radiator cover that directs the air into the radiator? The cover should be in the model also. If the cover forms a seal between the fan ring and the radiator, then that volume of air is at a higher pressure than the air pressure in the room due to the resistance to flow that the radiator poses to the airflow leaving the fan.  Do you know what that pressure is?

The model should replicate the conditions of the experiment. Please describe the conditions of the experiment. What is being measured in the experiment?

There are many CFD tutorials on this site and on YouTube that you can watch. This site has a list of textbooks.

I can help you with the geometry and some of the meshing. Other members can advise you on CFD model questions you will have. The idea behind meshing is to get good quality elements. The attachment above has elements with excessive skewness.  This can probably be fixed by having smaller elements. The problem you will have is that you are limited to the Student license limit of 512,000 elements. That is where cutting the model into a 1/3 pie slice is a big benefit. I did some reading of the sliding mesh method and it seems like you can do that and have periodic boundary conditions. Since you are just learning Fluent on a Student license, you might want to do this advanced method after you have a full model working.

The best practice for modeling a fan in open air is to have a 5 or more diameters of open air in front of and to the side of the fan, and 10 or more diameters behind the fan where there would be a lot of swirl created.  If you have a duct that the fan is in, that cuts down the size of the air domain to the sides.

 Regards, Peter

  • Liked by
  • monicaagabriela6
peteroznewman posted this 18 February 2019

Hello MonicaGabriela,

Thank you for the detailed description of the environment downstream of the fan. It looks to me like you need to know the airflow characteristics of the radiator in order to get to the point in the system where the measurements are made. You said the airflow is measured 100 mm downstream of the radiator, and I see the pressure gauge is also downstream of the radiator and upstream of the louvre bank. 

For example, if the louvres are adjusted so that the pressure in the box after the radiator is 200 Pa, what is the pressure in the plenum after the fan, before the radiator: is it 300 Pa, 400 Pa, or what?

It would be best to add a pressure gauge in this space and measure it directly. If you build a CFD model of the fan exhausting into a plenum before the radiator, you would assign a Pressure Outlet boundary condition, which means you need to know that value. Do you have a tachometer on the fan?  Another input to the CFD model is the rpm of the fan blades.

When there is a hub with fan blades in a CFD model, a cylinder of air slightly larger than the size of the blades is cut from the larger volume of air that goes out to the walls of the fan ring, at a diameter half way betweeen the tip of the blades and the fan ring. This cylinder and the two flat faces before and after the blades becomes a sliding interface between a mesh that rotates with the blades and a mesh that is stationary. That is what I created in the attachment. It requires specifying the rpm of the blades as an input to the model.  A zero pressure inlet and a positive pressure outlet boundary condition is used at the entrance and exit to the fan ring and the fan ring is a wall boundary condition.

The geometry I constructed is easily edited to make a smaller cylinder around the fan blades and pull the enclosure to match the fan ring diameter. The two ends of the enclosure can be pulled to the correct dimensions of the fan ring, upstream and downstream of the hub. However, the sketch shows a large motor body in the inlet flow path. That body could be modeled in later model to assess the motor body contribution to the flow.

A larger model would have the larger area of the radiator inlet surface. An even larger model could use a porous block to represent the radiator and have louvres on the backside box.

  • Liked by
  • monicaagabriela6
  • Jackely
monicaagabriela6 posted this 18 February 2019

Hello,

The pressure after the fan is not possible to be measured, in the fan plenum, as the air flow is highly swirled. However, the estimative value of the pressure after the fan would around 100,600Pa, considering that the inlet pressure at fan ring is the ambient pressure 100,000Pa.

Nevertheless, in the experiment, the air flow measurements are taken at 100mm distance from the radiator. The pressure after the radiator, where we took the measurements, should be around 100,300Pa. Would this be the suitable pressure outlet value for the boundary conditions?

Also, would it be necessary to create a porous block to represent the radiator since we know the pressure value? Also, the fan should run at 1490rpm.

peteroznewman posted this 18 February 2019

Hello,

I was speaking of Gauge Pressure, so that would be 600 Pa above ambient, after the fan.  I don't think the swirl would affect a pressure measurement too much.

Is the flow measured 100 mm from the radiator on the fan side of the radiator or on the louvre side of the radiator? I assume it is on the louvre side where there would be no swirl. Please confirm.

If you know the pressure in the fan plenum and the outlet area, you can model the flow through the fan without the porous block to model the radiator. But how do you know the pressure in the fan plenum if you don't measure it?  You said you wanted to compare with experimental data and you will only have the flow at one point after the radiator. How do you know the flow is uniform over the whole area of the radiator?

monicaagabriela6 posted this 18 February 2019

The flow is measured 100 mm from the radiator on the louvre side of the radiator. This is a rough estimation of the pressure in the fan plenum.

As it ca be seen in the picture below, a measurement instrument will be placed in different points across the radiator surface to find out the difference in air speed. The final value will be calculated by multiplying the mean velocity by the outlet area. 

Is the outlet area represented by the area of the radiator? If so, the outlet area is 3.43m^2 Please confirm.

Also, the air flow after the radiator is completely uniform, but it is not as swirly as the the one before the radiator because of the radiator fins.

 

Thank you so much!

peteroznewman posted this 18 February 2019

Once you integrate the air velocity at the outlet from the radiator over the entire area, you can calculate a total mass flow as the experimental value you can compare with the total mass flow from a CFD model. Assuming there are no leaks after the fan ring, you could have a small CFD model that begins and ends at the fan ring. The total mass flow out of that fan ring has to be the same. There will be a higher velocity out of the fan ring because the area is smaller than the radiator area.

I still think it would be best to measure the pressure in the fan plenum, before the radiator, rather than assuming it is 600 Pa.  Where did that number come from?  You have to use that number in the CFD as a Pressure Outlet boundary condition. If you don't measure it, I recommend you run a series of CFD solutions to study the effect the Pressure has on the mass flow rate. Once you have a curve of mass flow rate vs pressure, you can just pick the pressure that matches your measured mass flow rate and your model will agree perfectly with your measurement. But if you then measure the pressure and find it isn't the same value you used to get the mass flow rate, then you will have a source of error between a measurement and the model.

This discussion is getting too long for some members to read down to this post so I recommend you close this discussion by marking one of the posts with Is Solution and starting a New Discussion in the Fluid Mechanics section and ask some new questions using the great illustrations above. You can link back to this discussion for reference if you want.

  • Liked by
  • Jackely
monicaagabriela6 posted this 3 weeks ago

Peter, 

I am trying to produce the CFD simulation again by modifying the enclosure. The one that you prepared is cylinder and I want to produce another one which is a box to have the same area of the radiator from the test facility. I am struggling to produce the mesh. I have noticed that last time you produced 1 body sizing and 2 off face sizing. I am trying to create the name selection for the InterfaceEnclosure but I cannot reach the inner faces. Could you please help me out on how to reach the inner faces for that? Also, can I keep the same values that you assigned for the mesh size last time?

peteroznewman posted this 3 weeks ago

Monica,

You can select only the inner faces by changing to Box Select and dragging the box from left to right, enclosing the fan, without enclosing any outer faces.

Yes, keep the same mesh size.

peteroznewman posted this 3 weeks ago

Monica,

These warnings are not a big concern. What is more important is to check the element quality. In Mesh details, in the Quality category, you can set the Element Metric to Skewness, which is the most important metric for CFD.  It give you an overall view, but then you can click the Controls button and zoom in on the "bad" of high skewness.

You can click on any one of those bars and see where the highly skewed elements are located. Then you can try to add mesh controls to improve the skewness. Below are the elements from the tall green bar on the right.

Below is a slice through one of the fan blades. You have inflation, which is good. What you could do is create smaller elements on the leading edge of the blade. You could do that by putting a plane slightly back from the leading edge and slice the faces so you can have a face that gets a mesh control.

monicaagabriela6 posted this 3 weeks ago

Thank you so much! I will try to do that. However, I didn't manage to produce the FaceSizing for the InterfaceEnclosure by selecting the inner faces of the rotating body. Is this going to affect the mesh quality? Thank you so much for your reply! 

peteroznewman posted this 3 weeks ago

Attached is an archive with two new Named Selections, RotatingFaces and StaticFaces.  Each one has 3 faces. You can use these in Face Sizing controls.

Attached Files

monicaagabriela6 posted this 3 weeks ago

Thank you so much! 

Close