[ghorrocks]

The concept is simple (I should write a FAQ on this):

* Make the mesh significantly finer. Halving the element edge length is what you should aim for. This will make your mesh something like 8 times more nodes.
* Run the simulation to full convergence.
* Compare the results of interest to you to the initial mesh.
* If the results are equivalent to within a tolerance you are happy with then you have shown mesh independance and you can proceed.
* If the results are not equivalent to within a tolerance you are happy with then go to step 1 and halve the edge length again, and repeat the whole process.

Obviously this usually leads to very large meshes - but that is what CFD needs for accuracy.

Also note this method is pretty crude, can be fooled and is not very efficient. A much better method of showing mesh sourced errors is using grid convergence indexes and techniques like Richardson extrapolation - but these techniques are too complex to explain in a forum post. There are some links to these more advanced techniques in this FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

[A_Prakash]

Originally Posted by CFDST

A lot thanks.

Always happy to help and at the same time learn something new in the process.

Originally Posted by CFDST

My profile of the jet fan is getting better but still, I'm not satisfied at all.

I think because I'm used to Gambit and my geometry is made in there, and the mesh also. The flow in the jet fan doesn't look very good. In the Inside of the jetfans it is clear and looks good but after that when it enters the domain it is awfull in my opinion.The mesh is TGrid for the Entire Volume and the Fire subdomain, and Hex/Wedge for the Jet Fan There are pictures attached down.

What do you think:

1.Is it possible to make the simulation with a geometry from Gambit and run it into CFX to get good and real results ? because when I made the geometry on the top of my Gambit window there is sign: [ GAMBIT Solver:Fluent 5/6 ID: Name of the project ]. I have heard the difference between the CFX and Fluent solver- about the nodes ( CFX) and the cells(Fluent). Or may be I have to make it into Ansys Design Modeler or another program. I have the geometry also made into Autocad too- but I dont know to make it by surfaces or to be union solid and then the extraction and cleaning?

Thank you in advance.

1. You can use Gambit, no doubt. In Gambit set your solver to Fluent 5/6 (as you already have). Export the mesh in .msh format. Go to CFX-Pre and use File>Import>Mesh>(select Fluent *cas *msh in drop-down menu). One recommendation: If you are taking your mesh to CFX, do not create any "Interior" BC in Gambit - it will screw up the naming in CFX. Just assign a BC type to your faces and hit export. Don't waste time in selecting the perimeter/outer walls of your garage... Hit export...Gambit will give you a message after the export that a default 'wall' bc was created for for such and such faces. After importing in CFX you will see a faces under 'wall'.
1.b I did some work of geometry extraction from AutoCAD. It is simple: 1) Create a new layer in AutoCAD 2) Use polyline or line tool to draw the geometry in the new layer of step.1 (which would basically be: walls of ur garage, vents, columns and jet fans). Export as IGS from AutoCAD and import in Gambit.
1.c Once you import in Gambit, make ur volumes and usual stuff of cleaning. Once u get to meshing stage: Mesh jet fan and Fire Subdomain by hex/or pave first and try this option for rest of the big volume : use Hexcore (native). See pic. Also, It is absolutely possible to do this geo with all-hex or hex/prism.
1.d Another option you can try in the existing model u have is to use Tgrid throughout (jet fan and remaining volumes) with constant size.
By constant I mean, don't grow the mesh. See pic. It will lead to too high number of elements, that's the disadvantage.

[CFDST]

Originally Posted by ghorrocks

The concept is simple (I should write a FAQ on this):

* Make the mesh significantly finer. Halving the element edge length is what you should aim for. This will make your mesh something like 8 times more nodes.

Thank you for the reply. The element edge size means the interval size in Gambit,when meshing the faces and volume for example or the nodes for the edge meshing?


Thank you.

[CFDST]

Originally Posted by A_Prakash

Once u get to meshing stage: Mesh jet fan and Fire Subdomain by hex/or pave first and try this option for rest of the big volume : use Hexcore (native). See pic. Also, It is absolutely possible to do this geo with all-hex or hex/prism.
1.d Another option you can try in the existing model u have is to use Tgrid throughout (jet fan and remaining volumes) with constant size.
By constant I mean, don't grow the mesh. See pic. It will lead to too high number of elements, that's the disadvantage.

Thank you for the reply. It is a pleasure to help for me also, but I'm new to those things and do not have a serious amount of experience to do that.

1.I understand what you are talking about it 1.d to make the mesh with one interval size throughout the whole geometry, but I don't know may be my Gambit is different version I don't have this option about the grow rate and max size or I cannot find it.

2. About the Modeling the model by Hex or pave first the jet fan and fire volume and then Tgrid with Hex Core (Native) for the Entire Volume again I don't have them too again in my Gambit.

2.1) My problems are with the Gambit version or?
2.2) If the problem is not with the version to go first with the jet fan and fire subdomain, but when I choose Hex then _>>>>> which one to choose Map,SubMap,TetPrimitive,Cooper or Stair Step.
2.3) If I choose Hex/Wedge there is only one option - Cooper for the jet fan and fire subdomain.

Attatched are pictures.

3.The Hex/Pave mesh is better mesh than the Tgrid or?

Thank you in advance.

[A_Prakash]

Hmm...
'one single interval size' is different from 'growing' the mesh. In Gambit you choose an element size to tetra mesh and u get additional option to grow (u have to specify what Gambit calls 'growthrate' 1.1 or 1.5 or ...) the elements upto a certain factor (called "Max. size""). You can read documentation on this.
So:
1. In your screenshot no.4, what do you have when u select Tgrid? Post ur screenshot
2. In your screenshot no.4, what do you have when u select Hex core? Post ur screenshot

Hex/pave is definitely better. You get a neat distribution of elements and u end up generating a lot less net total number of elements compared to tetra.

[CFDST]

Originally Posted by A_Prakash

Hmm...
'one single interval size' is different from 'growing' the mesh. In Gambit you choose an element size to tetra mesh and u get additional option to grow (u have to specify what Gambit calls 'growthrate' 1.1 or 1.5 or ...) the elements upto a certain factor (called "Max. size""). You can read documentation on this.
So:
1. In your screenshot no.4, what do you have when u select Tgrid? Post ur screenshot
2. In your screenshot no.4, what do you have when u select Hex core? Post ur screenshot

Hex/pave is definitely better. You get a neat distribution of elements and u end up generating a lot less net total number of elements compared to tetra.

Hello, thank you. I have made the Pictures.
1.Tgrid 2. HexCore selected

[A_Prakash]

Well, I am not sure why you don't have additional options. But, nevertheless it look like you are already using uniform tetra mesh without growth factor, which is what I suggested earlier. Try Hex core option too. You can then take slice at various sections and see how Hex core does the job.

[ghorrocks]

I will leave the discussion on how you mesh in Gambit to others, but the end effect is that for the mesh refinement if you had a 1m cube meshed with 10x10x10 elements you would have 0.1m edge lengths. If you halve the edge length you would have 20x20x20 elements with 0.05m edge lengths, and your mesh size has gone from 1000 to 8000.

[CFDST]

Originally Posted by A_Prakash

Well, I am not sure why you don't have additional options. But, nevertheless it look like you are already using uniform tetra mesh without growth factor, which is what I suggested earlier. Try Hex core option too. You can then take slice at various sections and see how Hex core does the job.

Ok thank you. I have made 3 steps of meshing:

1.First to mesh a face of the jet fan with Ouad/Pave
2.Then to mesh the Jet Volume and Fire Volume with Hex/Wedge Cooper
3.Then to mesh the big Volume with Tgrid with HexCore

1.)Do you think works or it is wrong procedure? Because it gave me 11 highly skewed elements.The skewed are a big problem for the simulation or not??

2.) I have another question about the procedure, because when I was learning fluent at the university. The told us first to mesh the faces- Inlets, Outlets, walls and after that the Volumes. In my case a have a lot of volumes for my real geometry- all the jet fans are volumes, the fire volume and the entire garage volume. My faces for Inlets and Outlets(picture 4) are only the big garage ventilators in case of fire, and the will be only faces of which I will set Boundary conditions of Velocity intlets and Outlets. So because I want to try the mesh method that you recommend me Tgrid with one step all the volumes and If I first mesh the faces Inlets and Outlets(as they told me at the University) and after that the Volumes, this will lead to a grow rate of the mesh at some places. So my question is
2.) If I select all the volumes and make them Volume mesh with Tgrid(one step) this will mesh the faces too or not?

Thank you.

[CFDST]

Originally Posted by ghorrocks

I will leave the discussion on how you mesh in Gambit to others, but the end effect is that for the mesh refinement if you had a 1m cube meshed with 10x10x10 elements you would have 0.1m edge lengths. If you halve the edge length you would have 20x20x20 elements with 0.05m edge lengths, and your mesh size has gone from 1000 to 8000.

Thank you. I understand the edge length now.

[A_Prakash]

Originally Posted by CFDST

1.First to mesh a face of the jet fan with Ouad/Pave
2.Then to mesh the Jet Volume and Fire Volume with Hex/Wedge Cooper
3.Then to mesh the big Volume with Tgrid with HexCore

1.)Do you think works or it is wrong procedure? Because it gave me 11 highly skewed elements.The skewed are a big problem for the simulation or not??

No. The procedure is fine. You may need to vary the mesh sizes a little bit. It is trial and error. Generally though, 11 skew elements would not matter much if your net no. of elements is say 1 million. Of course, you need to be sure where your skews are located, that will determine how critical they are. skew elements right next to inlet BC face for example would not be acceptable. I have done simulation with few skews of .98 in about 5 million. The skew elements were in a deadzone behind an obstacle. Solution converged. Results were fine too.

Originally Posted by CFDST

2.) I have another question about the procedure, because when I was learning fluent at the university. The told us first to mesh the faces- Inlets, Outlets, walls and after that the Volumes. In my case a have a lot of volumes for my real geometry- all the jet fans are volumes, the fire volume and the entire garage volume. My faces for Inlets and Outlets(picture 4) are only the big garage ventilators in case of fire, and the will be only faces of which I will set Boundary conditions of Velocity intlets and Outlets. So because I want to try the mesh method that you recommend me Tgrid with one step all the volumes and If I first mesh the faces Inlets and Outlets(as they told me at the University) and after that the Volumes, this will lead to a grow rate of the mesh at some places. So my question is
2.) If I select all the volumes and make them Volume mesh with Tgrid(one step) this will mesh the faces too or not?

That kind of growth is expected. And, it wouldn't be a big deal. The growth rate I had spoken to you about is something different. See picture. It is from Sedan Geometry mesh tutorial. Back to your question: yes, u can mesh your inlet and outlet faces and then use Tgrid mesh, that's fine.

Meanwhile, I have attached another pic for you to give u an idea of how u can use Hex/Pave Cooper for your garage volume. Do the volume splits as indicated. Then do ur jet fan volume mesh, Volume X & volume Y mesh, fire subdomain volume mesh, inlet & outlet face and then do your garage mesh by Cooper scheme. It should work fine.

-------------------------------
Going off-track a little bit to CFX model: Do you think velocity inlet and velocity outlet BCs are good idea?
Are these directly connected to inlet and exhaust fans via duct?

[CFDST]

Thank you for the replies a lot.

First I have made the volume splits and try to made the Volume mesh as follows:
1.Hex/Wedge-Cooper scheme for the fire volume, jet fan,Volume X and Volume Y.
2.Then Tgrid with Hex Core it works, but the inside mesh is cooper and the mesh next to the walls is Tgrid.I'm not interested in the conditions near the walls, so Is this a problem? Because in a lot of tutorials I have seen that they put infaltions next to the walls and there the mesh is cooper and inside the domain it becomes Tgrid or Pave - Picture 1 and Picture 2.
So my question is:

1.Is this a problem, the Tgrid mesh next to walls and cooper scheme inside?

[Quote]Meanwhile, I have attached another pic for you to give u an idea of how u can use Hex/Pave Cooper for your garage volume. Do the volume splits as indicated. Then do ur jet fan volume mesh, Volume X & volume Y mesh, fire subdomain volume mesh, inlet & outlet face and then do your garage mesh by Cooper scheme. It should work fine.[Quote]

I have tried to make the things that you said as follows:

1.Mesh faces of Inlets and Outlets with Quad/Tri-Pave
2.Mesh the Fire Volume,Jet Fan,Volume X and Y wit Hex/Wedge-Cooper
3.Then the big Volume with Hex Wedge Cooper and there is a source face which stops the whole operation.It gives me an error:Source facing do not allow Cooper meshing for Volume 1(the big Volume) Picture 3(with initial meshing of the round faces with Quad/Pave), Picture 4(without initial meshing of the round faces) the same error. I think the problem is with the round faces of the jet fan and big(round intlets and outlets)or because there is a gap inside the jet fan between the cylinder and the cube for the protection of the jet fan(picture 5).

So what do you think?
2.Where is the problem with the cooper meshing, the gap, the mesh of the round facese of the inlets and outlets or smth else?

Thank you

[CFDST]

-------------------------------
[Quote]Going off-track a little bit to CFX model: Do you think velocity inlet and velocity outlet BCs are good idea?
Are these directly connected to inlet and exhaust fans via duct?[Quote]

The Inlets and Outlets at the walls are the big fans for supply and exhaust air in case of fire, if you are talking about them. They are big ventilators like picture 6 and picture 7, that are connected with a big shaft that goes outside. Do you find a problem modeling the like this BC- Inlets and Outlets???

[ghorrocks]

The CFX documentation has important comments on boundary condition selection. If you select velocity inlet and outlet then the pressure level is not set and the simulation is badly posed. You need to set the pressure somewhere.

[CFDST]

Originally Posted by ghorrocks

The CFX documentation has important comments on boundary condition selection. If you select velocity inlet and outlet then the pressure level is not set and the simulation is badly posed. You need to set the pressure somewhere.

I set the refference pressure into the domain options to 1 atm? So is this correct?

[ghorrocks]

The reference pressure does not set the pressure level in the simulation domain as there is still the unknown pressure offset from the reference pressure. Reference pressure is used to reduce numerical round-off errors. You need to set the pressure level somewhere, somehow.

[A_Prakash]

Originally Posted by CFDST

First I have made the volume splits and try to made the Volume mesh as follows:
1.Hex/Wedge-Cooper scheme for the fire volume, jet fan,Volume X and Volume Y.
2.Then Tgrid with Hex Core it works, but the inside mesh is cooper and the mesh next to the walls is Tgrid.I'm not interested in the conditions near the walls, so Is this a problem? Because in a lot of tutorials I have seen that they put inflations next to the walls and there the mesh is cooper and inside the domain it becomes Tgrid or Pave - Picture 1 and Picture 2.
So my question is:

1.Is this a problem, the Tgrid mesh next to walls and cooper scheme inside?

No, it is absolutely not a problem. There is no need to discriminate between Tgrid and Hex mesh. Both serve as a means to mesh depending on the complexity of geometry (and the particular region of interest. You are right about inflation- for example, you need this approach for more precise wind tunnel simulation). Of course, do not forget that you would get stupid results with both meshes if one's model is not set up with good engineering judgement. Hence, to answer your question: Tgrid mesh next to walls and cooper scheme inside is fine... and it is still better than full-Tgrid mesh. Why? One reason being that Hex core will give you less number of elements compared to full-Tgrid mesh for same geometry. This is good news because your solution time is directly related to number of elements.

Originally Posted by CFDST

I have tried to make the things that you said as follows:

1.Mesh faces of Inlets and Outlets with Quad/Tri-Pave
2.Mesh the Fire Volume,Jet Fan,Volume X and Y wit Hex/Wedge-Cooper
3.Then the big Volume with Hex Wedge Cooper and there is a source face which stops the whole operation.It gives me an error:Source facing do not allow Cooper meshing for Volume 1(the big Volume) Picture 3(with initial meshing of the round faces with Quad/Pave), Picture 4(without initial meshing of the round faces) the same error. I think the problem is with the round faces of the jet fan and big(round intlets and outlets)or because there is a gap inside the jet fan between the cylinder and the cube for the protection of the jet fan(picture 5).

So what do you think?
2.Where is the problem with the cooper meshing, the gap, the mesh of the round facese of the inlets and outlets or smth else?

Probably it could be the round faces of jet fan. Moreover, the 'gap' you mention, is actually an ENCASING volume. It is a good thing you put it around the jet fan. I suggest, make it slightly oversize-1.2xJF diamter for end faces, length=jet fan length. See pic. And then split this volume with jet fan volume and garage volume. Now mesh this volume with Hex/wedge Cooper. However, I am thinking that if you make it oversize as I just suggested..it may not mesh by Cooper by default. I am not sure... you may need to try it. If that happens, then pre-mesh just one of those oversize faces with pave and try cooper volume mesh again.

The idea behind this ENCASING volume is to make make it easier for Cooper algorithm to find end caps- i.e source and projection faces-for volume mesh. (However, It looks like you have actually subtracted this volume from the domain- and that's why u call it 'gap'. Is that correct? ) Once you have done all this; proceed to creating Volume X and Volume Y, and then splitting them with garage volume... and then the steps as before:
1.Mesh faces of Inlets and Outlets with Quad/Tri-Pave.
2.Mesh the Fire Volume,Jet Fan,Volume X and Y wit Hex/Wedge-Cooper [ADD: mesh of ENCASING volume]
3.Then the big Volume with Hex Wedge Cooper
I hope above steps work out for you. If not, then we need to troubleshoot more. In any case, you still have a Tgrid-HEx mesh, which is good enough progress!

----------------------------

Originally Posted by ghorrocks

The CFX documentation has important comments on boundary condition selection. If you select velocity inlet and outlet then the pressure level is not set and the simulation is badly posed. You need to set the pressure somewhere.

That is right. Velocity is a derived quantity. It is not a good constraint especially now in this case where you have temperature and density variation. Further, if you go to Calculators>Function Calculator in CFD-Post and check the massflow at your inlet face, is it similar to ur fan capacity?
So, instead of velocity, how about setting a mass flow boundary condition?

[CFDST]

Originally Posted by A_Prakash

That is right. Velocity is a derived quantity. It is not a good constraint especially now in this case where you have temperature and density variation. Further, if you go to Calculators>Function Calculator in CFD-Post and check the massflow at your inlet face, is it similar to ur fan capacity?
So, instead of velocity, how about setting a mass flow boundary condition?

Ok thank you about all the replies. You are really great.Really appreciate.

You were absolutely right about the inlets and outlets with velocity, I was really surprised what I have seen. Total disaster,nothing with reality.
I have set BC with Mass flow and now works better, but I have few questions.I have the mass flow of the fans in m3/h from the company that is selling them, but in CFX i have to set the mass flow in kg/s and due to the fact that I have I lot of variations in the density:

1.For example I have One Inlet Ventilator(with Inlet CFX BC) with mass flow 5300 m3/h that blows air with temperature 20 C in case of fire , and one outlet ventilator(with Outlet CFX BC) that sucks air with flow 6000 m3/h in case of fire. So the air density is app. 1.2 kg/m3 for the inlet with air at 20 [C],so my mass flow in kg/s = 5300*1.2/3600=1.766 [kg/s]. But about the Outlet, what is density????? Because it is changing throw all the simulation, because I suck hot gases and there density varies,but I need to set an mass flow in the begining of the simulation???? When I run the simulation there is a problem with the density of the Inlet Air,till the 80 [s] everything is fine, but after that the density of the air that comes from the inlet starts to rise till value of 3.40 [kg/m3], so there is a mistake and I dont know Where? Attached are picture with the variations of density and the CFX input.
My reference pressure is set to 1 atm, buoyancy effect included with z=-g, Total energy heat transfer model, Turbulence=Shear Stress Method, Fluid Material-Air Ideal Gas. The Fire grows quadratic from 0 to 80 [s],the from 80[s] to 160[s] maxPower and there from 160[s] to 200[s] extinction. Timesteps are 200*1[s]
So My questions are:

1.Why is this problem with the inlet density, because of the static temperature, I has to enter Total temperature or smth else???
2.How I can set the Outlet to be consistent with the density variations and also with the my initial value for the massflow rate 6000 m3/h?

Thank you.

[CFDST]

CFX setup:

http://www.2shared.com/photo/ipkWn0N...Mass_Flow.html
http://www.2shared.com/photo/QGtiI69...Mass_Flow.html
http://www.2shared.com/photo/aDznbiV...id_Models.html
http://www.2shared.com/photo/fXgowx_...e_Profile.html
http://www.2shared.com/photo/ypqYTzO..._Settings.html

[A_Prakash]

Your assessment of inlet side density to compute massflow is logical. However, it is strange as to why you see such high density. Even Air at -25C has Rho of 1.42 kg/m^3 (Source: Wikipedia). But seeing the pics u have attached, should we jump to conclusions? You have attached just one slice plane of contour. Do not forget that CFD calculation is about average values, nothing is entirely absolute. A better thing to do, I suggest, is to take areAve of Density at your inlet face at various timesteps, I am sure it would not be as high as 3.4 kg/m^3.
Other things to ask yourself: [I am sure Mr. Glenn and other experience users can add more insight on this...]
1. What about your convergence criteria? 1e-4, or less tight?
2. Is your specified flowrate (1.766 kg/s) being maintained? Check it through Function Calculator. Is it different from 1.766 kg/s? If yes, then how much? Is that 'how much' significant or 'ignorable'. If a solution is converged, then almost invariably your flowrate would be 1.766 +/- 0.001.
[All that has been mentioned above in pt. 2 is based on my little experience so far. Experienced users may have a more refined explanation. I hope Mr. Glenn or other users add their opinions too].
3. Try using physical time steps instead of Autotimescale. They make that clear in the CCL sheet you have posted in the beginning of this thread. It says:
"Buoyant flows can be difficult for the steady state solver to converge. It is often beneficial to use the transient solver even for a steady state solution. Time steps of around 1s may be possible for an inert fire model. The steady state solver can be run initially with auto time stepping. The time steps reported by the auto time stepping can by used as a guide for setting a transient time step."

Originally Posted by CFDST

1.Why is this problem with the inlet density, because of the static temperature, I has to enter Total temperature or smth else???

Total temperature would be used when u have viscous heating.. and it is more relevant for high-speed flows. There is already a lot on this in the forum.

Originally Posted by CFDST

2.How I can set the Outlet to be consistent with the density variations and also with the my initial value for the massflow rate 6000 m3/h?

Theoretically *you would estimate average density at outlet and use it for massflow*. However, ur problem does not have any opening BC. If, let's say, u set inlet mass flow is 1.2 kg/s (mIN) and outlet is 4 kg/s (mOUT)... that's not possible. Solver will struggle to make mass balance. mOUT much higher than mIN.
Back to ur specific case: Your exhaust fan must have the same or similar extraction capacity as inlet fan? Is that right? If yes, just set your Outlet flowrate to be same as inlet flowrate.
However, I am curious as to why your model garage does not have any atmospheric opening. Usually for ventilation purposes, mechanical supply is 80% (even upto 90% sometimes) of mechanical exhaust, rest 20% is sucked in through atmospheric openings.