[ghorrocks]

The length scale of the filter is going to be much smaller than the length scale of the main flow. This means the Reynolds number in the filter is going to be much smaller than the main flow. So if the Reynolds number is low enough that the main flow is laminar then the filter is also going to be laminar.

[lgtmelo]

Originally Posted by ghorrocks

The length scale of the filter is going to be much smaller than the length scale of the main flow. This means the Reynolds number in the filter is going to be much smaller than the main flow. So if the Reynolds number is low enough that the main flow is laminar then the filter is also going to be laminar.

thanks for the prompt response.

can you please explain why the velocity behaves as below then, as it seems turbulent to me. is there the possibility that the infill makes it turbulent because of the high surface area?

[ghorrocks]

Make sure you know the definition of turbulence - you cannot tell turbulence from velocity vectors, and a common misunderstanding for people who do not know fluid mechanics is that recirculations are turbulence (this is not correct). So go to a good fluid mechanics textbook and make sure you know what turbulence really is.

[lgtmelo]

Originally Posted by ghorrocks

The length scale of the filter is going to be much smaller than the length scale of the main flow. This means the Reynolds number in the filter is going to be much smaller than the main flow. So if the Reynolds number is low enough that the main flow is laminar then the filter is also going to be laminar.

Dear Glenn, just a thought that occurred to me: the length scale is much smaller indeed. but velocity increases due to it. I assume not as much as to be more significative then the length scale reduction?

[ghorrocks]

Let's make some educated guesses: If the pore area of the filter is 50%, then the average velocity of the fluid in the filter is 2x the incoming duct. And if the pore size is 1% of the incoming duct then we can estimate the change in Reynolds number to be 2*0.01 = 0.02. So the Reynolds number inside the filter is 1/50 that of the incoming duct.

So the Reynolds number is much lower in the filter than the incoming duct, and therefore more likely to be laminar flow.

[lgtmelo]

Originally Posted by ghorrocks

Let's make some educated guesses: If the pore area of the filter is 50%, then the average velocity of the fluid in the filter is 2x the incoming duct. And if the pore size is 1% of the incoming duct then we can estimate the change in Reynolds number to be 2*0.01 = 0.02. So the Reynolds number inside the filter is 1/50 that of the incoming duct.

So the Reynolds number is much lower in the filter than the incoming duct, and therefore more likely to be laminar flow.

thank you

[Jiricbeng]

Hi there,

I would like to add a question to this otherwise great thread.

- I am trying to simulate the particles with air ideal gas flowing in a duct
- steady state simulation
- I am using the transport solid model
- I applied the restitution coefficients 0 on a wall

What is the most appropriate variable to tell me, how many particle adhered to that wall? What is the best practice to find out the rate/portion of particles that are collected on a wall?

Thanks a lot.

[Gert-Jan]

a) Look in the output file. There in the bottom an overview is given of amount of particle mass that is collected on each wall with R=0, outlet and inlet (in case of back flow).

b) In Post, 1)visualize the particles by selecting the particle object, 2)set filter on the wall of interest with R=0, 3)set the number of particles to visualise equal to what was entered on the inlet of your simulation, 4)Tick the Info-tab that gives you the number of particles in your view.

c) In the Output Control section of Pre, you can generate exports for particles when they exit via a wall or outlet. These exports can contain any variable. This allows for detailed analysis in e.g. MSExcel.

Make sure all your particles end somewhere. If a lot of particles are still floating around or end with an error, then your numbers will not be in balance. Information on the faith of the particles is also given in the output file (=source of a lot of vital information)

[Jiricbeng]

Thank you much for your reply, but I do not see the possibility b)

b) In Post, 1)visualize the particles by selecting the particle object, 2)set filter on the wall of interest with R=0

In filter, there is only filtration according to the diameter... see the attachment.

One more thank!

[lgtmelo]

Originally Posted by Jiricbeng

Thank you much for your reply, but I do not see the possibility b)


In filter, there is only filtration according to the diameter... see the attachment.

One more thank!

you can enable end region and make it into your desired "wall". this way, it will only show/count the particles that ended there.

it is important to note that this excludes particles whose fates are still undefined, i.e. those in between the beginning and the end.

[Jiricbeng]

Thank you guys. Displaying the adhered particles seems to be not perfect. When plotting the particle tracks ending on the wall with rest. coeff. =0, I can see just the entanglement of the "streamlines" (particle track). Colouring the "streamlines" acc. to some criteria is not illustrative either as I would like to see only the adhered positions of the particles. Knowing the particle numbers collected on the wall is helpful, that is good, but I would preferably like to get the contours of spatial distribution of the collected particles on the wall.. Do you please have any tips/tricks for this? Or is it unfeasible?

[Gert-Jan]

- You can plot the particle fraction as a variable on the wall.
- As stated in my previous post, define a csv-export-file (See Output Control in CFX-Pre) of particles ending on a wall. If you only save the coordinates, you can import this file as Point Cloud to display the particles in Post (Insert>Location>Point Cloud).

[Jiricbeng]

Good, I get it. If you look at the comparison of volume averaged fraction of particles on the walls of interest, you can see a good correlation with the point cloud (created in Pre, thanks a lot!). However, the cloud points should be the "correct" positions, whereas the volume avg fraction can take into account even the particles that are just close to the wall but did not adhere to the wall, I guess.

[Gert-Jan]

I expect the volume fraction is the ratio of the number of partcles (in volume and residence time) that flows through and element, and the element volume itself.
Since the volume is just above the wall, then even particles that do not hit the wall are included. This is highly mesh dependent.
I would look in the help for the correct definition.

[Jiricbeng]

I have encountered hiccup:
The exported points (from Pre output control) on the wall with restitution coefficient = 1 are presented. That means, these points are not those which are collected on this wall. I would expect the csv file for point monitor on a wall with rest. coeff = 1 should be empty but it is full of points.
It leads me to the thinking that the only reliable way to observe the collected particles on a wall is via the Paticle track and the filtration.

Moreover, according to the definition of rest. coefficient, if this coefficient is non-zero, that is, higher than zero, no particle can be collected on such wall as there always will be some velocity component of the reflection. This implies me another idea: modelling the adherence of the particles on a wall by setting rest. coeff. is absolutely limited to setting it as zero. But that means an immediate collection of a particle that accidentally hits the wall, without any possibility....

[Gert-Jan]

It all depens on why you do the modelling (why do you do CFD?) and the physics you require for this. Do you need one- or two-way coupling? Is it transient? Do you know the restitution coefficient from experiments? Do you need to know the impact on the blade of the end location on the outlet?

A additional hint is to define two types of particles, one that adheres and one that doesn't. If you do two-waycoupling, than using 2 fractions might influence the results. Then create one for the main stream using R=1 (99.9% of the mass) and one for a small stream using R=0 (0.1% of the mass). That gives you more flexibility just for postprocessing.

[Jiricbeng]

Thanks for giving me the clues. I really appreciate that.
Briefly: The aim is to model collecting the soot particles on a wall of a radial compressor.

This is a new topic and my assumption was:
- One way coupling as particles do not affect the flow. They affect the flow only after they adhere to the walls due to geometry changes of the wall itself. But for the first approach I would neglect this. First I want to see where they collect.
- Stationary flow. But steady state is obviously limited to modelling by restitution coefficients.

It seems that rest. coeff. cannot be used for modelling this issue, that is for prediction of adhering a particle due to some conditions such as low relative velocity or temperature... Probably, I will have to go to transient to be allowed to use wall film modelling... or is there another way (in steady state)?

[ghorrocks]

CFX has only very simple models for particles impacting surfaces. The wall film model is intended for fuel droplets and how they behave on walls. I do not think that will be very useful for your soot particles.

If you want complex wall interaction like you have described (adhesion at low velocity or temperature) then your options are, from what I can see:
* User fortran - I think you can determine particle fates with user fortran. Not certain, but I think you can (I have not done it).
* Fluent - Has more detailed particle models than CFX and the user routines allow a lot of control as well
* DEM - If you link CFX to a DEM like rocky or EDEM then you will get lots of control over what the particle do.

A further comment - particles like soot are likely to have additional physics coming into play very close to the wall (electrostatics, Van Der Wall forces, surface chemistry effects like surfactants or surface energy; squeeze film etc) so the detail of whether the particle deflects or sticks probably has some influence by these more complex effects.

[Jiricbeng]

Glenn,

thanks for the info. To be more accurate, the soot particles might be accompanied by little oil, which, as results, leads to "sintering" the soot particles. So, it seems the main factor is a combination of low velocity and high temperature (I wrote this clumsily in a previous post).

Nonetheless, when reading manual, it seems the oil film modelling could be a way to include the wall temperature effect to model the droplet adhering. But it is interesting the CFX makes it possible to run the "Wall film" option even with soot (Particle transport solid)..

As it is goes in engineering world, one wants to deal with a problem no one knows anything :-).