[ghorrocks]

There is an FAQ on accuracy: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

In this case I doubt you will find the assumption of steady state appropriate. Highly buoyant flows like this are often transient. This is discussed in the FAQ.

[CFDST]

Thank you for the reply.

I set the inlet with massflow, the outlet and an opening after . So in my case I see that I have to put some Openings and this is the truth.
Like the attached picture 1 from the CFX solver modeling guide they said it is most robust to put Mass Flow inlet and Static pressure on the outlet. But there is one sentence I cannot understand very well, because my real garage will be with 4 Inlet Ventilators, 4 Outlet ventilators and 2 openings and the said:

''With more than two inflows, the other openings should be of the boundary condition type Opening. This is because the flow a these other boundaries could be in general be in or out, and the direction will be a part of the solution''

1.So judjing by this I have to put 4 Inlet- Mass Flows and 6 Openings or I'm wrong and What has to be my boundary conditions in this case.

2.Second Question:In picture 2 and Picture 4 about the openings: What means this Opening Pres. And Dirn and Why the values are often 0 or 1 [Pa] in most of the examples I have made ?

3.Third Question: If I use the most robust scheme and set 4 Inlet-Mass Flows with mass flow= 1.5 [kg/s] and 4 Outlets and choose the option with Static pressure for the outlets-and the company, that is making the ventilators says that for 1.7 [kg/s] the ventilators gives 150 [Pa] Static pressure(Relative Pressure) I have to :
Add this value 150 [Pa] for the outlet static pressure or it is too big and I'm wrong? Picture 3
Thank you in advance.

[ghorrocks]

The most important thing is to define boundary conditions which match the situation you are trying to simulate. I see from your first post you have some inlets and outlets - but what defines the flow in them? If they have fans then what is the operating point? Or a fan curve? And what is the condition on the other side of the fan as a reference?

For the outlets - what is downstream of them? What flow condition does that impose?

These are the questions you need to answer to correctly set your boundary conditions.

[CFDST]

Thank you Mr.Ghorrocks and Mr. A_Prakash for the help my work is almost done I think and I have few details to make and run the big simulation. I really appreciate your help without it, I won't be able to do that. As I make a progress with my simulation and at the begining I was not thinking to add a sprinklers into the simulation but now I have time till my defense of the project and I want to add some sprinkler system into the domain. I have searched through the Internet for some topics connected with sprinklers in CFX but nothing specific. Tommorow I wil try to set a simulation with one sprinkler but I don't know how to begin. The first thing that come in my mind is to set the volume as a mixture with water and air, but that will confuse my simulation till now, so my question is do you know How I can simulate the sprinkler system? any suggestions or sources that I can read from?

Thank you.

[ghorrocks]

It depends on what you want to model the sprinklers for.

If you simply want their cooling effect then put a heat sink where they act. Simple (but very approximate).

If you want to see where the sprinkler water goes and how it affects the flow field you can use either a lagrangian or Eularian model with water droplets.

The most complex and most complete way of modelling them is with water droplets, but including the heat sinking effect of the water. This will be quite complex as the droplets will evaporate as they cool so coupling this into the simulation will be tricky. But if you want the complete model then this is what you want - I just hope you have plenty of time to develop it and validate it.

[CFDST]

Originally Posted by ghorrocks

It depends on what you want to model the sprinklers for.

If you simply want their cooling effect then put a heat sink where they act. Simple (but very approximate).

If you want to see where the sprinkler water goes and how it affects the flow field you can use either a lagrangian or Eularian model with water droplets.

The most complex and most complete way of modelling them is with water droplets, but including the heat sinking effect of the water. This will be quite complex as the droplets will evaporate as they cool so coupling this into the simulation will be tricky. But if you want the complete model then this is what you want - I just hope you have plenty of time to develop it and validate it.

Thank you for the reply. I will try to implement the Spray Dryer tutorial model into my simulation. From a surface I will try to add water droplets with a set velocity and Temperature and see if this will works. The problem that I think I will have as you said is with coupling the evaparation and cooling effect from the droplets to the fire. And also as some water falls on a fire, the evaparation of it produces steam. I will try to solve this if it is possible. I have almost 4 months till the end of my project.

[CFDST]

Hello again to all CFD users,

I have validate my fire and smoke scenario and now I have continued with the sprinkler modeling. I try to implement the spray modeling tutorial into my fire scenario. I have imported the CCL( evaporating _drops) into my case, after that I have followed the instructions into the tutorial, but when I run the solver it returns with a code 1.

My geometry is a square cube with sizes 12x5x3, one jet fan, one Inlet fan, one Outlet fan( with pressure 0 Pa), a fire domain cube with sizes 2x2x2.3 and a sprikler above the fire. I have changed the expert parameter pt zone specific tracks = f.

My inlet for the water is the sprinkler like in the tutorial. I run a steady state analysis with 100 iterations(autotimescale) and after that a transient analysis with 300 timesteps each 1[s]. When I run the solver It starts to iterate but after 10 iterations it stops and return with code 1 and says:

| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| The particle number fractions have to add up to a total of one wi- |
| th a tolerance of 1%. The sum of the user specified values exceed- |
| s this threshold. |
|

How can I fix this problem? Thank you in advance.

[A_Prakash]

I believe the message is self-explanatory. Somewhere, you have given a wrong input and therefore, you are exceeding the sum total value of 1. Sorry, I can't give u real pointers because I have no experience with this.

Quick question: What do you mean by 'validate the fire scenario'. Did you do some kind of actual test? I am very interested in the validation part for this CFX fire model.

[CFDST]

Originally Posted by A_Prakash

I believe the message is self-explanatory. Somewhere, you have given a wrong input and therefore, you are exceeding the sum total value of 1. Sorry, I can't give u real pointers because I have no experience with this.

Quick question: What do you mean by 'validate the fire scenario'. Did you do some kind of actual test? I am very interested in the validation part for this CFX fire model.

Hello A_Prakash,

Thank you for the reply.
By validating I mean that I have made a big model and run it on a server for 300 s. I investigate the temperatures of the fire, adjust them for my needs,adjust the jet fan massflow and the smoke quantity was modeled. Everything was enough good for my understanding( this is the first time I'm using CFX, so I am completely new). But the problem is that the geometry is very complex and the server is not that powerfull and the whole process of running was about 6 days. I need to run 800 s simulation and I am looking for a stronger server. The validation is nothing special, I haven't made a real test, I'm waiting for a posibility, but now the things are stucked, so I will see.

During this period of waiting I'm trying to implement the sprinklers model into my model, but it is not that easy.

[CFDST]

Hello all Cfd users,

I have give up with implementing the sprinkler model because I'm running out of time before defending my project. I have made a simulation of my garage for 300 [s] and after seeing the results I made some changes of my model: I repaired the jet fans and insert two cylinders one in another, I reduce my supply fans and exhaust fans and finally I thought everything was ready and I will run my 1200 [s] simulation and there was a big surprise two errors. I don't know what to do with them, because I made the same steps as what I have done for my previous model- the mesh, the split volumes in Gambit, the expressions in CFX, but I got this errors :

ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Floating point exception: Overflow |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine FPX: C_FPX_HANDLERv






and also two NOTICES:

----+
| ****** Notice ****** |
| The Wall Heat Transfer Coefficient written to the results file for |
| Fluid 1 |
| is based on the turbulent wall function coefficient. It is |
| consistent with the Wall Heat Flux, the wall temperature, and the |
| Wall Adjacent Temperature (near-wall temperature). If you would |
| like it to be based on a user-specified bulk temperature instead, |
| please set the expert parameter "tbulk for htc = <value>".

| Notice: The maximum Mach number is 7.975E+00






I have read the FAQ about what to do with this errors:

Тhe model blocked at the beging of the steady state

The mesh is the same quality as the previous, even a bit more precise.

I don't know where is the problem, the mesh quality or the spliting volumes in Gambit, the CEL expressions?


I have worked 4 months for this simulation and I have 2 weeks to finish it and defend my project at the University, but this error surprise me badly. Please help and thank you in advance.

Attached are some pictures:

The Model with the cylinder and cube jet fan is the previous model, that runs correctly

The Model with the two cylinder jet fan is my current model.

[ghorrocks]

I cannot count the number of times people have started by modelling the most complex model they can imagine and got nowhere and then had no results to show for all the work. Surely a better approach is to start with a simple, single phase model and get that working; then add the complexity one piece at a time. In my experience 90% of the time this approach shows that the simple models tell you all you need to know and the complex model is unnecessary anyway. Anyway, enough of my soapbox.

The overflow error is an FAQ: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

In fact the Mach number error is a another symptom of the same problem - your model is numerically unstable.

Don't worry about the htc warning. It is just saying the reference value for the heat transfer coefficients is not what you might expect. This is a post processing issue, not a solver issue.

I would start with a simple model you should be able to get results from easily. That means remove the fans. Then at least you have a result! Then put the fans back in and we will try to get them working. Then add the complexity one bit at a time.

If you want to look at the fans a bit closer please post an image showing how you have modelled the fan geometry.

[A_Prakash]

Hello Angelov,

The Mach number error is the obvious pointer I think. Pressure level seems to be messed up in your problem.

Looking at first two pics:
Pic 1: You have three inlets and three openings. Jet fans are circular... I guess this is your latest model? Combination of inlet and opening is not a good idea [btw, are you using static Pr = 0 or Opening pr = 0 at the opening?].
Pic 2: You have three inlets, 3 outlets and two openings (You previous model, as per your pic caption) This BC setup is good: You have 3 fixed inlets and 3 fixed outlets...so, any flow imbalance between inlet and outlet can be accommodated through openings (i.e flow can come in or go out from ambient surroundings if you have used Opening Press. = 0).
Do you agree?

Here is a possible solution: If you know the amount of massFlow at inlet and outlet (based on actual fan duty), then use that value. If you don't, then do a 10 Air change per hour calculation, find the flow rate and use it [as per BS 9999:2008 for fire ventilation in car parks/basements].
Point is: Constrain the problem in a proper way...rather than vaguely have inlet and opening... and let the software figure out what to do at the opening.

[CFDST]

Originally Posted by ghorrocks

I cannot count the number of times people have started by modelling the most complex model they can imagine and got nowhere and then had no results to show for all the work. Surely a better approach is to start with a simple, single phase model and get that working; then add the complexity one piece at a time. In my experience 90% of the time this approach shows that the simple models tell you all you need to know and the complex model is unnecessary anyway. Anyway, enough of my soapbox.

The overflow error is an FAQ: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

In fact the Mach number error is a another symptom of the same problem - your model is numerically unstable.

Don't worry about the htc warning. It is just saying the reference value for the heat transfer coefficients is not what you might expect. This is a post processing issue, not a solver issue.

I would start with a simple model you should be able to get results from easily. That means remove the fans. Then at least you have a result! Then put the fans back in and we will try to get them working. Then add the complexity one bit at a time.

If you want to look at the fans a bit closer please post an image showing how you have modelled the fan geometry.

Thank you for the answers both of you.Really appreciate.

I have modeled the fans in this steps( in Gambit):

1.First modeling the garage by sketching the base and then sweep the edges.

2. Then creating the faces for the inlet and outlet fans

3. Then building two cylinders one in another for the jet fans

4.Then spliting the main volume with the face inlet and outlets

5.Then the jet fan splitting:
- 5.1.First the outside cylinder with the inside cylinder (command: split volume option: bidirectional connected)(Picture Jet-Split 1 and Picture Jet-Split 2)
5.2. Then the main volume with the two splitted cylinders.(command: split volume option: bidirectional connected).( Picture Jet-Split 3 and Picture Jet-Split 4)

6. Then spliting the main volume with the fire volume

7. Then deleting the splited two cylinder volume and I left only the inside cylinder to add momentum source to it, so there appear a gap between the main volume and the inside cylinder( but the previous simulation was with the same split and it runned without error)

8.Finally meshing the outlet and inlet faces with Tgrid 0.1
Meshing the main volume and the jet fans with Tgrid 0.2

For the CFX model:

I export the CCL file from my previous simulation and import it into my new CFX simulation onto the new geometry. I try to make my last model: With 3 massflow Inlets 1 kg/s; 3 Outlets ( Massflow 1.2 kg/s) and two opening( opp. and dirn pressure 0 [Pa]) and AGAIN the same ERROR about the mach number and the overflow.

I try the both schemes:

Inlets- Mass flow BC [kg/s]
Outlet- Mass flow BC [kg/s]
Openings- Opper and Dirn pressure 0 [Pa]

Second scheme:

Inlets- Mass flow BC
Outlet- Average static pressure - (-500) [Pa]
Openings - Opper and Dirn pressure 0 [Pa]

For the jet fans 6 with momentum source = 20 kg/m2s2

1 jet fan = momentum source - 20 kg/s2m2, due to the direction of the flow.

The relevance pressure is 1 atm.

But there were the same errors. I don't know where is the problem, may be the import CEL expressions file, the mesh of the volumes, or because I set a simulation of 1200[s] and my computer can not cope with it due to low ram memory or may be a mistake.

Attached are the pictures and the output file from the steady state simulation. Thank you a lot

[CFDST]

Originally Posted by A_Prakash

Hello Angelov,

The Mach number error is the obvious pointer I think. Pressure level seems to be messed up in your problem.

Looking at first two pics:
Pic 1: You have three inlets and three openings. Jet fans are circular... I guess this is your latest model? Combination of inlet and opening is not a good idea [btw, are you using static Pr = 0 or Opening pr = 0 at the opening?].
Pic 2: You have three inlets, 3 outlets and two openings (You previous model, as per your pic caption) This BC setup is good: You have 3 fixed inlets and 3 fixed outlets...so, any flow imbalance between inlet and outlet can be accommodated through openings (i.e flow can come in or go out from ambient surroundings if you have used Opening Press. = 0).
Do you agree?

Here is a possible solution: If you know the amount of massFlow at inlet and outlet (based on actual fan duty), then use that value. If you don't, then do a 10 Air change per hour calculation, find the flow rate and use it [as per BS 9999:2008 for fire ventilation in car parks/basements].
Point is: Constrain the problem in a proper way...rather than vaguely have inlet and opening... and let the software figure out what to do at the opening.

Thank you for the answer.
1. The opening is with Opening and Dirn pressure 0 [Pa]

2.Yes I agree, my previous model was like this but I don't know where is the mistake. Everything is the same with the setting conditions.

I have attached the output files and my current model.

My previous output file: transient
http://www.2shared.com/file/G0gUbnMp...-Transien.html

[ghorrocks]

But there were the same errors.

That is because you have not paid attention to my previous post. Remove the fans and just do a simple run with your inlets and outlets. Make sure this runs properly. And if it does run then at least you have a simulation completed which is more than you have at the moment.

At the moment you do not know whether your problem is in your general model or specific to the jets.

And I have already explained what the linear solver and Mach number error is due to - your simulation is numerically unstable and it is diverging. You need to increase the numerical stability.

A further thought - if you are getting Mach number errors then this simulation is using a compressible gas. Why are you using a compressible gas? Most HVAC models are done using an incompressible gas with a thermal model.

[CFDST]

Originally Posted by ghorrocks

That is because you have not paid attention to my previous post. Remove the fans and just do a simple run with your inlets and outlets. Make sure this runs properly. And if it does run then at least you have a simulation completed which is more than you have at the moment.

At the moment you do not know whether your problem is in your general model or specific to the jets.

And I have already explained what the linear solver and Mach number error is due to - your simulation is numerically unstable and it is diverging. You need to increase the numerical stability.

A further thought - if you are getting Mach number errors then this simulation is using a compressible gas. Why are you using a compressible gas? Most HVAC models are done using an incompressible gas with a thermal model.

Thank you for the reply.

I have remove the jet fans from the simulation and only run the 3 Inlet fans, 3 Outlet fans, 2 Openings and the Fire subdomain. Everything was perfect the simulation runs and the model was stable, the residiuals goes well. So the problem is in the fans.

First I want to ask about the compressible gas:

1. I have written somewhere, that when the density in the model is changing significantly,due to the fire, that I'm simulating, I have to set Air Ideal Gas with a Total Energy( Heat transfer Option). Which option is better for my model?: Air at 25 with Thermal Energy model
or Air Ideal Gas with Total Energy model


Second about the geometry:

I have made the Geometry in Gambit and spliting the volumes of the jet fans there, so in my previous geometry they( jet fans) were modeled by a cube and a cylinder and in my new model they are two cylinders, so I think the problem is that- the two cylinders.I don't like the meshing system in Gambit I tried to import my model in Ansys DM to mesh it. There were three scenarios:

First: I import my Gambit model(with the cylinders), I have splitted the volumes into Gambit and after that I transfered(the mesh file) it into Ansys DM - There were 9 Parts, so I made a Boolean operation to conect them(picture 1) and after that when I set the domain in CFX it gave me 9 fluid regions and 9 assemblies(picture 2), so after I run the simulation it gave an error 9 isolated fluid regions.

Second: I have splited the volumes in Gambit directly import the dbs file from Gambit to DM(picture 3) and After that the program creates on its own interfaces between the jet fans cylinders( the outside and the inside cylinder)(picture 4). After running the simulation it says that the gap between the two cylinders were very small and it returns with an error.

Third: I have removed the outside cylinder, after that splited into gambit the main volume and the jet fans. After that transfered into DM- mesh it. After that I transfer the mesh into CFX and again 9 volumes 9 assemblies(picture 6)- I made an interface between the jet fan outside and the another side that appears from the assembly(picture 7). I run the simulation but again an error.





Mr.A_Prakash said in some of the previous posts, that I can made the geometry in Autocad by polylines, but after that when I transfer it into DM for meshing and cleaning what is the procedure, the jets should be frozen bodies, everything has to be in one part the jet fans, the main volume, how is the procedure with the interfaces beetween the jet fans and the main volume, this part is missing for me. If it is possible to explain it: A scenario- jet fan, main volume what is the connection between the to run properly ???

Thank you in advance

[CFDST]

The picture 6 and 7

[ghorrocks]

I have remove the jet fans from the simulation

Good. Now we have a good starting point.

Which option is better for my model?

The thermal model will be more stable so I would start with that. But a fire will result in temperature differences big enough that a compressible model may well be required. But do that once the thermal model is working - small steps.

The fans you are modelling are very small compared to your model. So do you need to model them at all? Why not model the fans as source points - then you completely avoid the geometry/meshing problem but still get the flow moving with source points.

[CFDST]

Originally Posted by ghorrocks

Good. Now we have a good starting point.



The thermal model will be more stable so I would start with that. But a fire will result in temperature differences big enough that a compressible model may well be required. But do that once the thermal model is working - small steps.

The fans you are modelling are very small compared to your model. So do you need to model them at all? Why not model the fans as source points - then you completely avoid the geometry/meshing problem but still get the flow moving with source points.

Thank you for the reply. I haven't used source points and I have written about them into the CFX pre user guide and the modeling guide. I don't know how to transfer my data for the jet fan to be suitable for the source point:

My jet fan is modeled as a Subdomain with a momentum source/porous loss option and the general momentum source 90[kg/m2s2] selon to the direction of the flow(picture 1)

And in the source point option: Which option I have to choose to transfer my 90 [kg/m2s2] to source point:

If Continuity there is one time the mass flow and another time the velocity,there is a temperature(it depends from the volume temp) and also I want to preserve the smoke to run through the jet fans, one time to be sucked from the domain and to go through the fan and then blowing into the domain. How this should be made with the source point?( picture 2 and 3).

Or may be I have to use the other options:
Turbulence Kinetic energy or frequency



Thank you in advance.

[ghorrocks]

Actually, on second thoughts you cannot do momentum sources with source points. Looks like only mass and energy sources an that means you are creating or destroying mass or energy. My understanding is you just want a momentum source, so then you have to use the subdomain approach you previously were using - sorry about that, my bad.

Have you had a look at the solid/fluid simulation in the CFX tutorials? Have a look at how they have meshed it.