Community
CFD Forum
Welcome to Autodesk’s CFD Forums. Share your knowledge, ask questions, and explore popular CFD topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Tunnel Jet fans

29 REPLIES 29
SOLVED
Reply
Message 1 of 30
Berkan_vent
2106 Views, 29 Replies

Tunnel Jet fans

Hi everyone,

 

i want to ask a question about my model that related about tunnel ventilation system.

 

As you know tunnel needs ventilation. For this reason i want to use jet fans for my model. In material tab, i see internal fan/pump. Can i use it for my model? or do i need to use different thing?

 

if i use internal fan how should i describe boundary conditions?

 

Thank you so much.

29 REPLIES 29
Message 21 of 30
Jon.Wilde
in reply to: sahar.rubin

Hi Sahur,

 

I'm getting there, don't worry 🙂

 

Looking at the mesh diagnostics, there are some really thin surfaces. I tried to show how to access this and the location of this small surfaces (there are more than one, all the same) in the attached image. You need to remove these in CAD, they are likely caused by small gaps.

 

Kind regards,

Jon

 

Small Surfaces.png

Message 22 of 30
Berkan_vent
in reply to: Jon.Wilde

Hi Jon,

 

You are a very great Autodesk Supporter. Thank you so much for your precious support. We do good models because of you. By the way Sahur you did great job 🙂 

 

I read your writings and in light of this i finalized my model. As you know i asked you about cylindirical  jet fan model not like Sahur's fans.

 

I created cylindirical shroud around the cylindirical jet fan model. And i suppressed all solid parts as well solid shrouds around jet fans.

 

I assigned internal fan/pump material for my jet fan model, and also assigned constant flow rate (20 m3/s) because i haven't got any data for fan curve. What is difference between constant flow are and fan curve datas?

 

 

*For jet fans, do i have to assign RPM? 

 

*I assigned slip factor 0,3 but you did 0,7 for Sahur's fans. So what should i assigned slip factor value for jet fans?

 

*Do i have to assign boundary conditions to jet fan inlet and outlet side?

 

* I want to add fire for my model so how should i define fire?*

 

 

I added my model so Could you check my model please? 🙂

 

 

Thank you so much,

 

Berkan

 

 

Message 23 of 30
Jon.Wilde
in reply to: Berkan_vent

Hi Berkan,

 

Thank you for the compliment, it is good to know I am making a difference.

To answer your questions:

 

I assigned internal fan/pump material for my jet fan model, and also assigned constant flow rate (20 m3/s) because i haven't got any data for fan curve. What is difference between constant flow are and fan curve datas?

That is fine, the fan will pump the 20 m3/s. If you assign a curve, the pump will produce the flow rate based on the dP across it - here is it mainly open so it will be close to the maximum anyway.

 

*For jet fans, do i have to assign RPM? 

You do not have to. Try it with and without. One will swirl, one will not. To match reality it might be better to assign an rpm. We typically do use an rpm unless the fan is represented with a cuboid, then it does not work so well - try it and you will see how it tries to rotate the cuboid...

 

 

*I assigned slip factor 0,3 but you did 0,7 for Sahur's fans. So what should i assigned slip factor value for jet fans?

What made you pick 0.3? I do typically use 0.7 but if you have data to suggest otherwise that is fine.

 

*Do i have to assign boundary conditions to jet fan inlet and outlet side?

No, we never should assign internal surface boundary conditions. (I am about to contradict myself as there is one exception)

 

* I want to add fire for my model so how should i define fire?*

This is usually done with a resistance called 'fire' inside a hollow vertical tube (which can be suppressed). It will have a volumetric heat load applied to it (to represent the fire) and a scalar = 1 (100% smoke) applied to the top surface.

You will then need to set a Scalar = 0 to the model inlets (this represents clean air). Any air that passes through the fire will become scalar 1, which in this case will be 100% smoke. We need to set a diffusion coeff (0.12 cm/s) and turn scalars on.

You will also likely want to run with air-variable and gravity also, so that natural convection is considered.

 

Check out these links:

Scalar Mixing

Smoke Analysis

 

It might be worth you checking out the Wiki and the help in future as many of the answers you seek should be there 🙂

 

Regarding your model.

I would run with a P=0 on all inlets.

Is there a reason for the temp on the celing? This will be 100% fixed is that correct? Perhaps a film coeff might be better, something like 5W/m2/K at the ambient temp, to allow heat to escape but still maintaining the reference ambient temp?

The inlets also need a temperature, or CFD will not know what temps are where.

I would extend all inlets and outlets a little, so the celing BC is not touching the inlet/outlet ones.

Be sure to give those fans a good uniform mesh, like in the guide I posted.

 

Kind regards,

Jon

Message 24 of 30
sahar.rubin
in reply to: Jon.Wilde

Agree with everything Berkan said, you're an AMAZING supporter!!

 

Now for my simulation:
I changed the jet fans because the volume somehow made problems so I just put them as cubes with the fan material and face it in the parking lot, 
I've made 200 iterations solver and the results are attached.

Now I want to make smoke and fire in the parking lot and see the temperature and pressure throughout the model, but, the guidelines are really difficult to understand and I never really know if what I do is correct, do you have a tutorial for smoke/fire in a closed space with ventilation ? Or any tips on how to do it?

BTW, for the parking lot walls, don't I need to do slip/symmetry?
And, why doesn't the software recognize the ducts as ducts? The material is air as shown at the tutorial, but the inlet/outlet seems from the hole in the ceiling rather than from the edge of the duct, I bet it's something to do with the air in the main void (all the inside of the parking lot)


thanks again!!
You're the best 🙂

Message 25 of 30
Berkan_vent
in reply to: Jon.Wilde

Hi Jon,

 

Thank you so much for the support 🙂

 

For my old model, I just wanted to assign initial condition to tunnel air temperature. So it is not for the ceiling.  

 

For my new model i want to assign stack effect to the inlets as you know stack effect causes pressure drop. According to my pressure calculation, stack effect causes 8.37 Pa. (Between enter and exit portals). Can i assign this value? if i am wrong please correct me.

 

And also i have a plane problem,  my tunnel model has slope ( 2 degrees) and it is about 1800 metres. Im just trying to obtain good plane ( Z or X axis). But tunnel model has slope so i couldnt. I try to rotate plane but i couldnt again. How can i obtain proper plane? I attached my model so you can understand me clearly.

 

Thank you so much.

Message 26 of 30
Jon.Wilde
in reply to: Berkan_vent

Hi Berkan,

 

You can use the curved arrows on the cut-plane to rotate it.

Better to left click on the plane, click on the top right icon (align to surface) and select the underside of the tunnel and the plane will snap to it.

 

Kind regards,

Jon

Message 27 of 30
sahar.rubin
in reply to: Jon.Wilde

hi! 
i have a question about smoke ventilation, in the attached file, you can see a parking lot with 4 outlets (each 10000 cfm), 1 inlet (free air inlet) and 4 jetfans for air circulation and movement,

my question is why can't all the air be changed?

i calculated the outlets by 6 air changes (sum of 40000 cfm) = means that in 10 minutes all the smoke (scalar 0) needs to be ventilated!

 

some numbers:  

area = 1985 m^2

height = 3.2 m

 

Thanks!

Message 28 of 30
Jon.Wilde
in reply to: Jon.Wilde

Hi Sahur,

 

What results are you seeing presently? Is it possible that you have some dead zones that are seeing less flow and so the air is not fully cleared?

Message 29 of 30
sahar.rubin
in reply to: Jon.Wilde

Hi!

 

i got funny result to my simulation.. 

after 600 seconds the suddenly a rise in pressure and velociity.. why does it happen??

i attached the support file.. 

 

tnx

Message 30 of 30
Jon.Wilde
in reply to: sahar.rubin

I suggest this is down to mesh. This is only one element through the fiire thickness, should be 4-5 at least. The same for the gap beneath it.

It might also be the timestep sizing, 1s with 1 inner iteration is quite fast, perhaps 3 inner iterations might help?

 

Kind regards,

Jon

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report