[Vishnu_bharathi]

Hi,

I am doing transient heat transfer simulation. A simple model with porous region is showed in the attachment. I was trying with the actual high temperature settings and there was convergence and back flow issues. So before proceeding I wanted to observe the simulation under ambient temperature ranges. The fluid is compressible(density dependent only upon temperature). The turbulance model is SST with mesh quality parameters are very good.

I performed few basic simulation runs for the shown model(attachment). 1st try: Reference pressure for fluid and porous domains is 1 atm. Inlet conditions are 0.5 kg/s and Inlet TEMP is 25 deg C. outlet BC set to static pressure with relative pressure being 0 bar. With this setup I received the velocity streamline as indicated in the attachment. All moving to the bottom of outlet surface area. It is understood this is because of the warning message I received during solver run "68% or 55 % or 75% wall is placed at outlet region try changing the outlet to opening" . I already have extended the outlet from my previous runs as far as I can to reduce the % of wall being placed at outlet. But still received the same message even with ambient temperature conditions(temp 25 deg).

I understood that its the pressure Boundary conditions that make the difference. I gradually increase the inlet BC from 0.5 kg/s to 1.0 kg/s to 2.0Kg/s and finally to 5 kg /s(with temperature at inlet being only 25 deg C). I observed the % of area being made wall at outlet reduced for 2.0 kg/s and vanished for 5 kg/s. I checked the pressure drop in case of 5.0 kg/s between Porous inlet and porous outlet. It difference happened to be around 30,000 Pa. with pressure from porous outlet till fluid outlet(actual outlet BC face)being 17 to 20 Pa less than the atmosphere.

So the pressure difference really made the difference with all setup being identical(Temperatures at Inlet being ambient 25 deg only).

Try 2 :With the inlet conditions being constant: 0.5 kg/s and temperature 25 deg, I tried with keeping reference pressure 15,000 Pa above atmosphere for fluid and porous domain and pressure at outlet to 3000 Pa above atmosphere. But this has not improved the % of wall being placed at outlet message even by small amount. I get few "%" like 2%, 3% being made wall during initial iterations but after some time it again goes to the normal 65%, 75% etc.,

Try 3: With the inlet conditions being constant: 0.5 kg/s and temperature 25 deg, I tried with keeping reference pressure 15,000 Pa above atmosphere for fluid and porous domain and pressure at outlet to few pascals below atmosphere(eg 20 Pascals) but the message "% of wall being placed at outlet" does not change anything from Try 2.

How does the pressure at outlet(static relative pressure) and reference pressure works out? When I tried with 0.5 kg/s, 25deg C at Inlet conditions and reference and relative static pressure being 15,000 Pa and 3000 Pa above atmosphere , I expected the message "%" of wall being placed at outlet to be comparatively lesser but it did not.

Could we somehow adapt the pressure conditions with 0.5 kg/s and same Inlet Surface area to achieve the velocity streamline going out through the full surface area of the outlet unlike shown in the attachment?

Could anyone suggest possible pressure combinations(at reference pressure and static outlet pressure) to tryout?

[ghorrocks]

Please attach your CCL and your output file.

[Vishnu_bharathi]

Originally Posted by ghorrocks

Please attach your CCL and your output file.

Hi Ghorrocks, I could not upload the ccl files and .out files here so I have created a link and uploaded files:

https://www.4shared.com/folder/ynCKktkm/ccl_and_.html

If you cannot download the files, please let me know. I should find some other means to send the file

In the attached excel I have included the details of combinations that I tried. Temperature at Inlet is only 25 deg for all cases.

[evcelica]

Looks like you may be including gravity in the simulation and you defined the outlet as constant pressure?
So once you take into account static head, all the flow wants to go out the bottom?
Really the outlet would have a pressure gradient with height.
Turn off gravity and re-run to check if this is the problem.

[ghorrocks]

I don't download foreign links. Please just post it on the forum.

Is gravity actually doing anything in this simulation? Do you have a multiphase or buoyant model present? If not then gravity has no effect and gravity should not be modelled. Then the static head issue mentioned by Erik will be avoided.

[Vishnu_bharathi]

Originally Posted by ghorrocks

I don't download foreign links. Please just post it on the forum.

Is gravity actually doing anything in this simulation? Do you have a multiphase or buoyant model present? If not then gravity has no effect and gravity should not be modelled. Then the static head issue mentioned by Erik will be avoided.

I could not post in the forum as its little over 200KB and also the .ccl format is not supported. Sorry, Is there any simple means to add file in the forum that I am not aware of?

I have the buoyant effect in my simulation. But for this simulation run with Temperature being 25 deg I guess it won't have influence. I will try deactivating it once. Ultimately, for my actual simulation I need to include buoyant model because the temperature is well over 500 degree C and I believe it should and will be present in real case.

I think the files that I am going to attach has more information and you could have a look and suggest . It is the pressure drop between the porous region that makes difference in the flow streamline, I guess.

[ghorrocks]

Attachments: Trim the output file to remove most of the boring convergence steps. Just leave the starting section and the convergence near the end. For the CCL file, feel free to rename it as txt. It should be a small file and easy to attach.

Just because it is hot does not mean buoyancy is important. Buoyancy is driven by temperature differences which cause density differences, and these effects need to be significant relative to convection. So buoyancy is not necessarily important. As you can see, modelling buoyancy makes the modelling more complex so you should only model it if it is significant.

[Vishnu_bharathi]

Originally Posted by evcelica

Looks like you may be including gravity in the simulation and you defined the outlet as constant pressure?
So once you take into account static head, all the flow wants to go out the bottom?
Really the outlet would have a pressure gradient with height.
Turn off gravity and re-run to check if this is the problem.

Hi Evcelica, Thanks for your reply.

Looks like you may be including gravity in the simulation and you defined the outlet as constant pressure?
yes. I included gravity in my simulation. I defined outlet with static pressure. I performed steady state before moving to transient as in the latter there was some convergence issues. At first I wanted to see if it works without any temperature and so I set inlet with 0.5 kg/s and temp. at 25 C. and then with 2.5 kg/s and 4.5 kg/s, where the message "% of outlet being made wall" reduced for 2.5 kg/s comparing with 0.5 kg/s and with 4.5 kg/s it seemed to almost okay with the flow.

So once you take into account static head, all the flow wants to go out the bottom?
In the first case(0.5 kg/s) the streamline was moving downward in the outlet face because more than 60% of outlet was turned into wall and this was not the case with 4.5 kg/s, the fluid goes out through the entire outlet surface. The pressure drop was about 30,000 Pa between Porous inlet and porous outlet and about 8,000 Pa in 2.5 kg/s and about 450 Pa with 0.5 kg/s. All being at Inlet temp 25deg. I can not change the inlet surface area so I was trying to adapt the pressure conditions at outlet and reference pressure(I do not know if its the best approach) to make the fluid flow through out all of outlet surface area. I believe it should be quite simple and I do not know why it is not working even with eliminating the heat parameter.

For 2.5 kg/s the % of outlet being turned wall was about 12% and for 4.5 kg/s it was only 0.3%. For the above three gravity was activated.

Please have a look into the attached excel file in the previous message, I have tried few combinations and provide your feed back. Thanks

[ghorrocks]

If you must run with buoyancy, also make sure you have the buoyancy reference density and location set correctly. If your fluid is constant density then the reference density must be this density. If your fluid is variable density then you need to carefully set the reference density and account for the variable density in the boundary condition.

The reference location should be somewhere in the middle of your domain.

[Vishnu_bharathi]

Originally Posted by ghorrocks

Attachments: Trim the output file to remove most of the boring convergence steps. Just leave the starting section and the convergence near the end. For the CCL file, feel free to rename it as txt. It should be a small file and easy to attach.

Just because it is hot does not mean buoyancy is important. Buoyancy is driven by temperature differences which cause density differences, and these effects need to be significant relative to convection. So buoyancy is not necessarily important. As you can see, modelling buoyancy makes the modelling more complex so you should only model it if it is significant.

Thank you for the quick reply

"Just because it is hot does not mean buoyancy is important. Buoyancy is driven by temperature differences which cause density differences, and these effects need to be significant relative to convection"
I have taken a note of it. As you have mentioned the buoyancy is driven by temperature differences which cause density differences, it is interesting to me. Once I sort this normal simulation without any big temperature I think I need to include this for my model. Eg., my model is 2m * 2m in cross section and the height increases for later simulations. The length is over 6 m. With temperature over 500 C and with above measurements I am now really interested to see the comparision between on and off buoyancy settings. But that comes later.

Attachments:
I have attached an excel having data's for pressure values that I tried out. Please have a look into it and it would be great if you could give feedback. I am trying to see if adapting pressure conditions could make the "% outlet made into wall" message disappear for 0.5 kg /s inlet condition. From my observation I see the pressure settings really makes the difference between 0.5 kg/s and 4.5 kg/s and as I can not change the surface area at Inlet, I am trying with pressure parameters.

I have attached the .out files and ccl files of 0.5 kg/s and 4.5 kg/s. For 2.5 kg /s every thing stays the same expect mass flow condition and "% outlet being made wall" is above 12 %.

[ghorrocks]

I have had a quick look at your CCL.

* You have viscous work turned on. Unless you think this effect is significant then turn it off. All physical models add complexity, so if the physical model is not important then why make things hard for yourself?

* Your fluid is Air at 25C. This is an incompressible fluid model so will have constant density.

* But you are using the Total energy thermal model. Why did you do this? If you are using an incompressible fluid model you should probably be using just the thermal energy model.

* Your buoyancy reference pressure is 1 kg/m^3. Based on the models mentioned previously this means the hydrostatic pressure will be wrong over the outlet and you will have regions of forward flow and regions of backward flow. So this explains the weird flow at the outlet.

* You have also selected Average static pressure for the outlet. You might need to consider whether this is appropriate.

* You also have complex material models in your CEL. I would debug your simulation using simple, constant properties material models and introduce the complexity once the simpler material models are working.

[Vishnu_bharathi]

Originally Posted by ghorrocks

I have had a quick look at your CCL.

* You have viscous work turned on. Unless you think this effect is significant then turn it off. All physical models add complexity, so if the physical model is not important then why make things hard for yourself?

* Your fluid is Air at 25C. This is an incompressible fluid model so will have constant density.

* But you are using the Total energy thermal model. Why did you do this? If you are using an incompressible fluid model you should probably be using just the thermal energy model.

* Your buoyancy reference pressure is 1 kg/m^3. Based on the models mentioned previously this means the hydrostatic pressure will be wrong over the outlet and you will have regions of forward flow and regions of backward flow. So this explains the weird flow at the outlet.

* You have also selected Average static pressure for the outlet. You might need to consider whether this is appropriate.

* You also have complex material models in your CEL. I would debug your simulation using simple, constant properties material models and introduce the complexity once the simpler material models are working.

Hi, Thank you for the suggestion

I removed the viscous term. Changed to thermal energy instead of Total energy(the temperature does not change from 25C). Removed the buoyancy option. The simulation ran for 0.5 kg/s without the message '% wall has been changed to oulet'. very good. The steamlines are perfect!

I removed the viscous term. Used thermal energy option. The Inlet temperature is 650 C, mass flow = 0.5 kg /s and outlet condition is static relative pressure = 0 Pa, reference pressure for domain = 101325Pa, Buoyancy is removed. The simulation is very good so are the streamlines!

I removed the viscous term. Used Total energy option(I used fluid whose density varies with temperature). The Inlet temperature is 650 C, mass flow = 0.5 kg /s and outlet condition is static relative pressure = 0 Pa, reference pressure for domain = 101325Pa, Buoyancy is removed. The simulation is very good and so are the streamlines

But when I activated buoyancy condition with ref. buoyancy density = 0.717 kgm^-3 it creates problem with other conditions being kept the same. I used the same fluid which worked with Total energy option but now with buoyancy activated, receive the message '% wall placed at outlet. With increasing mass flow from 0.5 kg/s to 2,5 kg/s to 4,5 kg/s the '% wall ' message disappears.

Does increasing the mass flow remove the buoyancy model effect? I red in the documentation and see that "Boussinesq Model" is used for constant density fluid case and "Full buoyancy model" for density as a function of pressure or temperature.

I believe my model comes under "Full buoyancy model" as Fluid density vary over temperature and range of operation between 25 C and 650 C. I need to include this effect, I believe.

I have attached images of my density profile and reyNum profile. I did not understand the formula mentioned in CFX documentation to check if buoyancy model has significance in any case. Is this the formula to check the requirement of buoyancy model?

Please could you suggest if Buoyancy should be activated or not? If yes, why it tries to create wall at outlet? Could you suggest any steps?
I used average ref. buoyancy as 0.717 kgm^-3 for my case.

Any suggestions for this?: "Based on the models mentioned previously this means the hydrostatic pressure will be wrong over the outlet and you will have regions of forward flow and regions of backward flow. So this explains the weird flow at the outlet"

Attachment: images showing density variation over temperature and CFX formula.

[Vishnu_bharathi]

Originally Posted by evcelica

Looks like you may be including gravity in the simulation and you defined the outlet as constant pressure?
So once you take into account static head, all the flow wants to go out the bottom?
Really the outlet would have a pressure gradient with height.
Turn off gravity and re-run to check if this is the problem.

Hi Evcelica,

It worked with turning off gravity When I include gravity the solver turns 70% of outlet as wall and so fluid goes to the bottom of outlet. I tried with 'gravity on' for ambient temperature at Inlet(which should not have any effect as density wont change) and with 600C at Inlet. In both the case i receive the message '% outlet turned into wall' . Does the hydrostatic pressure phenomenon a problem in this case, when we introduce ref. buoyancy density?

I tried with buoyancy on with ref. buoyancy density as 0 kgm^-3 and with 0.717 kg m^-3. But something is not right. Any suggestions to try? Since my case has fluid with density dependent on Temperature, I need to include this effect.