[ghorrocks]

Thermal conductivity is a field variable so it can handle variable property materials. That is why what you have done does not work.

Set a variable called "thermal conductivity" to the value for thermal conductivity you want to use. Then set your material to have that variable as thermal conductivity.

You can also get this directly by using some sort location function (probe, areaAve, volumeAve) of the thermal conductivity variable.

[Shomaz ul Haq]

Great you're back Glenn I have made an expression for effective thermal conductivity (keff) using a correlation and made that the thermal conductivity of a duplicate of water I name "Nanofluid". I am using that in place of water in domain "Hot water" whereas domain "Cold water" remains the same using just water. I wanted to ask would using an enhanced thermal conductivity increase the temperatures along the length of the pipe or heat transfer? Would be grateful. Thanks.

[ghorrocks]

The effect of the increased thermal conductivity will depend on the configuration. But really you should be telling us what the effect should be - it is your topic after all, and you need to be able to work out basic issues like this yourself.

[Shomaz ul Haq]

Thanks. You are right. As you know I am using two fluids hot water in inner tube and cold water in annulus. I made a new material as a copy of water named "Nanofluid" and changed Basic Settings Option: to Pure Substance with the same Material Group: Water, Constant Property Liquids and introduced thermal conductivity as CEL expression "keff" with rest of the properties unchanged. I wanted the cold water domain to have the same material as before water but when I changed the Fluid and Particle Definition Fluid 1 Material to Nanofluid it changes that to Nanofluid in all domains. In short I want the material Nanofluid to be used in inner pipe (Hot Water) domain and plain water to be used in annulus domain (Cold Water). Please help me regarding this. Would be grateful. Thanks.

[ghorrocks]

CFX insists that the same fluid be used in all domains, even if they are not connected. If you want to use different fluids in different domains you should use a multiphase model and use the volume fraction of the fluids to determine which fluid is where.

CFX has a expert parameter to remove the checking of constant domain physics. If you activate this expert parameter it will allow you to put different fluids in different domains without the need for a multiphase model. But it is an expert parameter for a reason - this option can have unexpected consequences (greatly increasing numerical roundoff error being a key one) so if you use this option you need to know what you are doing.

[Shomaz ul Haq]

Thanks Glenn. I was expecting that answer. You confirmed my suspicions. So this expert parameter you are talking about, can I use it?

[ghorrocks]

Yes, of course - but be careful, and keep an eye out for unexpected problems. Especially roundoff errors.

[Shomaz ul Haq]

Thanks a lot Glenn. Before I do that I did calculations for counter flow double pepe heat exchanger without nanofluid. On paper (theoretically) calculated the outlet temperatures of both inner pipe and annulus for hot water and cold water using properties of water at average of inlet temperatures of inner pipe (60) and annulus (20C) which is 40C. The flow is turbulent according to Re on paper and also on CFD. On CFD I did that in CFD Post using a line in center of inner of inner pipe along the axis for hot water and a line parallel to the axis along the annulus. I then used these in chart and got temperature variation along pipe length (z). When I compared paper results with CFD there was a difference of about 7.26C at inner pipe outlet for hot water and 2.3C at annulus outlet for cold water. I checked my speeds for both inner pipe and annulus inlets which is 5 m/s. Why is there a difference when everything else is the same. I am using k and e model to account for turbulence and high Re number with k=.01 m^2 s^-2 and e=.1 m^2 s^-3. Would be grateful.

[ghorrocks]

FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

First you need to ensure your CFD model is accurate, see the FAQ for some tips here. Then you need to consider how accurate the result is you are comparing to is. It appears you are comparing to hand calculations which probably use lots of empirical models - you cannot expect exact answers from these type of models.

[Shomaz ul Haq]

You are absolutely right Glenn. I corrected it some some extent using those FAQs. Thanks a lot. Also I wanted to ask is there any way I can plot outlet temperature variation with inlet speed along z axis (Velocity w) using chart. Can't figure that out. I know how to get mean of temperature at outlet using a plane and average function in an expression and using a variable but I don't get it how to do it without using a line as a line along the outlet plane and even at a point would give me something else and not what I want. In other words can I use a pre defined variable like Velocity w but give it a range over which to check outlet temperatures even though the variable has been given a constant value in inlet boundary condition in CFX-Pre. Would be grateful. Thanks

[ghorrocks]

I do not understand what you are trying to plot. Please post an image of what you are trying to do.

[Shomaz ul Haq]

Hi Glenn. I want to plot a chart of outlet temperature versus inlet speed. How can I do that without going through these steps:
1. Going to CFX-Pre changing the boundary condition
2. Running the CFX-Solver,
3. Running CFD-Post, and
4. Then noting the values and shifting them to excel one by one for plotting.

In short how can I do that for mean outlet temperature variation with changing speed directly. Hope you understand it now. Would be grateful for help. Thanks.

[ghorrocks]

You can do this as a parametric model in ANSYS workbench. That allows you to plot values over multiple simulations to get curves like you describe.

[Shomaz ul Haq]

Thanks Glenn. What's a parametric model and how can I use it to make a curve over multiple simulations? Would be grateful.

[ghorrocks]

Search the ANSYS documentation on parametric modelling. Note this is a ANSYS workbench feature, not CFX; so you need to look in the ANSYS workbench documentation. There are some tutorials on it as well I think.

[Shomaz ul Haq]

Thanks Glenn. I have seen the documentation. It is helpful. That expert parameter you told me about to remove checking of constant domain physics, what is its name. Can't seem to find it in ANSYS Documentation-CFX-Modeling Guide-Expert Control Parameters section. Would be grateful. Thanks

[ghorrocks]

The expert parameter is "check isolated regions"

[Shomaz ul Haq]

Thanks Glenn. I checked ANSYS Help 15.0 for parametric modeling tutorials. In ANSYS Workbench Tutorials it says To access tutorials for ANSYS Workbench, go to http://www.ansys.com/tutorials. I need tutorial regarding usage of parametric modeling for making curves over multiple simulations in CFX. In Design Exploration Toolbox in Workbench I dragged the "Parameters Correlation" in Project Schematic. It creates Standalone System but I don't know how to connect/link this to CFX-Post. I tried connecting CFX-Post by dragging it to CFX-Post but it doen's budge. Would be grateful for any source of tutorials or help. Thanks.

[Shomaz ul Haq]

Hey Glenn. I clicked on ""check isolated regions" expert parameter. When I tried to change the material in annulus to water while trying to maintain nanofluid in inner pipe, again the material snapped to only one material. Any idea why isn't it working? I haven't used solid domain for the inner pipe but in the "Domain Interface: Default Fluid Fluid Interface - Additional Interface Models Tab - Mass and Momentum Option" I selected No Slip Wall. I checked "Heat Transfer", in "Heat Tranfer - Option" I selected Conservative Flux, in "Interface Model - Option" I selected "Thin Material", in "Material" I selected Copper, and in "Thickness" I selected .001 [m]. Is that expert parameter not working because I did not use a physical solid domain between the two regions and used instead a thin material. Would be extremely grateful for help. Thanks.

[ghorrocks]

You are probably going to have to set up the multiple fluids yourself through CCL. The CFX-Pre GUI will not support this option as it is an expert parameter.