Recommendation regarding pipe flow / pressure drop

[ramrecon]

Hi all, thank you for this forum I am an avid surfer on here 🙂

I would like to ask for recommendation regarding internal turbulent pipe flow, what sort of turbulence model would be acceptable to determine the pressure drop? The fluid I am working with is steam, I specified it as a custom material within CFD (properties evaluated at 99% steam quality at 10 bara), I am not doing any heat transfer, just determining the pressure drop. Since my geometry is fairly complicated I am having a hard time determining the "truth" or the acceptable truth with the literature.

1. I am curious about the Intelligent Wall Function (IWF) when you specify wall roughness in the material options for the pipe itself, when using k-omega SST it is mentioned in the help that you need to disable the IWF if you specify a wall roughness, does that apply as well for the k-epsilon ?

2. The meshing, how would you go about the enhancement layers for the internal flow, for k-epsilon with IWF 5 layers, 0,45 layer factor and Auto graduation is acceptable? For the k-omega SST I am using 12 layers 0,6 layer factor and 1,30 graduation. The pressure drop varies signifigantly about 1-2kPa when comparing those two. I am doing 2x adaptive meshing runs with my inital meshing size as auto meshing with volume adjustment of 0,5 for the entire model, this applied for both turbulence models k-epsilon and k-omega SST. ADV5 is used for both turbulence models.

For the overall pressure drop I am getting lower values for the k-epsilon then the k-omega SST but which one should I put my trust in, my pressure drop goes from 6kPa to about 9kPa. 

Any recommendation on this would be greatly appreciated and if there is anything I can provide you with you with to make things clearer I will do my best to supply, I am currently running the model as we speak so I might not be able to upload the share file just now.

Kind regards. 

[Jon.Wilde]

Hi,

You should be able to upload a CFZ fine, as soon as you started running the model, CFD would have produced a _support.cfz in the folder. Please could you share this with us?

Thanks,

Jon

[ramrecon]

Hi,

Oh sorry for that, I have the file it is attached 🙂

Regards,

[Jon.Wilde · Accepted solution]

Thanks for sharing, here are some pointers before we get into the actual results:

1. You need longer outlets. I would use at least 10x diameter in length. Right now you results will be highly unpredictable as you are going to see recirculation over the boundary conditions - this must always be avoided
2. Suppress all solid parts from the mesh, they are not needed -  you can set the wall roughness to the steam to have the same effect 😉
3. Keep an eye on your flow velocities incase this is compressible. A custom steam material so you can use a fixed density and incompressible flow is great but you may not be capturing the full physics
4. I would have thought you could get great results on your first run with this, given enough mesh

I am not sure what turbulece model is best to capture wall roughness as I rarely use it - about to ping a colleague to ask for a little assistance.

Kind regards,

Jon

[Jon.Wilde]

Either turbulence model can work, although ke has no wall function anyway. With SST, you will need to turn of IWF.

[srhusain]

I might mention that in V2015, the k-e model does have IWF, aka "Scalable Wall Function" capability, which is recommended for pipe flow analysis.

Hope this helps.

[Jon.Wilde]

You only need to disable IWF for the SST model. With the ke model you can use IWF and wall roughness together.

[ramrecon]

Thank you for your quick responses, I will extended my outlets, get rid of the solid parts (which is great!), I also assume the flow to be incompressable.

Then I will run both models SST (no IWF) and ke with both, for comparison sake.

One last thing, how would the process of evaluating saturated fluid such as saturated steam go about, that is the workflow. Do you solve the flow first then the heat transfer or do you do both at the same time and do you require any additional meshing since the fluid is saturated for the solution to converge?

Thank you in advanced for the help 🙂

[Jon.Wilde]

If you are to consider heat transfer (possible phase change?) you will need to mesh the external solid again.

You would need to use a steam model and run flow and heat transfer together, as they would then be related.

[ramrecon]

Ok, again thank you for your help and quick responses.

Think I will will manage from here on and maybe get some good numbers from my model 🙂

Regards,