September 17, 2020 at 2:10 pmAyomikun1Subscriber
I am trying to evaluate the thermal efficiency of a subsea warming spool at -47.3C submerged in sea water with an ambient temperature of 4C , in a variety of arrangements In 2D in a 50mby 50m domain. Firstly, single straight Pipe, then a 2 Pipe set-up with offset in the X Direction with the distance between the pipes as a factor of the pipe diameter (i.e 2*D, 3*D , 4*D etc), and finally a 2 Pipe set-up with offset in the Y-Direction with the distance between the pipes as a factor of the pipe diameter (i.e 2*D, 3*D , 4*D etc).
Firstly, as I am trying to model to evaluate the Total heat transfer rate and surface heat transfer coefficent through the pipe to the surrounding sea water and the surface heat transfer coefficent. Do I input the properties of the pipe in the reference value section or of seawater in the reference value, boundary conditions and operating conditions section . In addition, for the pressure in the reference value and operating conditions section do I input the hydrostatic pressure at the water depth. If so the bottom of the seafloor is 800m below sea water and the pipe is in the midldle of the domain. Do I use the Hydrostatic pressure at a depth 800m or at 750mSeptember 17, 2020 at 2:14 pmAyomikun1SubscriberPlease Pardon My Spelling mistakesnSeptember 18, 2020 at 12:53 pmRobAnsys EmployeeThe reference pressure is used for pressure coefficient calculations, so doesn't matter here. I'd also suggest checking how each heat transfer coefficient is calculated in Fluent as we have 3-4 of them. My usual approach is to use the heat flux, and area from Fluent and then pick the temperatures that make sense to you as you would in an experiment and use Excel/calculator/piece of paper to find the HTC. nThe only other thing to watch is gravity and operating density to prevent the water moving due to height effects. Look at section 22.214.171.124 and I'd suggest making sure that rho_0 (operating density) is exactly the same as rho_s. nRe the turbulence, RNG ke with buoyancy terms on is recommended if it's turbulent. I'd also extend the profile to be larger than the temperature range you're modelling. nSeptember 23, 2020 at 1:19 pmAyomikun1SubscriberGood Morning. When I do that I do get the currect values for the heat transfer coefficent as my imperically calculated values I don't how ever see the convective effects Illustrated in the models above. I see no convection in the velocity Contour and No fluid Build Up at the Bottom of the pipe. Why does Changing the Way Pressure is modelled have an effect on the expected convective effect and the total heat tranfer rate?nSeptember 23, 2020 at 1:55 pmRobAnsys EmployeeIt's not the pressure, it's the operating density that's being fixed. Check the documentation section I suggested, the flow is a result of rho_s - rho_0 not being zero and you not calculating the exact pressure on each bc. It's not zero it's a function of the height and density difference, so the bottom boundary will have a pressure of a few pascals more than the top, the sides are then a variable value based on position. nSeptember 23, 2020 at 4:59 pmAyomikun1SubscriberAre you then suggesting that the pressure gradient is what is preventing the observed convection wake when i dont model hydrostatic pressure. i have gone through the document and understand what you mean with regards to rho_o , what is confusing me is why changing the hydrostatic pressure affects the presense of a convection wake I have observed in previous simulation. I am aslo no wwondering if I am using the correct inflation layer set up. When i use a total thickness inflation set-up and specify the thickness to 20mm I reach steady state much later in my simulation I also get a much larg much larger range for total heat flux and the wrong final value. Where as when I use a first layer thickness Specification at 5mm for the first layer; I get the correct value for Total heat Transfer rate and reach steady state in the faction of a second. I dont understand why there is such a variation ? nSeptember 25, 2020 at 11:09 amRobAnsys EmployeeThe wake is formed by the buoyant plume (warm, less dense material rises). If you get the pressure bc's wrong (ie don't account for hydrostatic head) such that you get flow induced by the boundaries it can mask or reverse the buoyancy driven flows. nThe near wall mesh will effect the heat transfer from the solid to the surrounding fluid. Given the motion is driven solely by the temperature gradients getting it right is critical. You also need to account for the flow and thermal boundary layer thickness: they can be different. nViewing 6 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.Trending discussions
- Suppress Fluent to open with GUI while performing in journal file
- Heat transfer coefficient
- What are the differences between CFX and Fluent?
- Floating point exception in Fluent
- The solver failed with a non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Getting graph and tabular data from result in workbench mechanical
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
Top Rated Tags
© 2022 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.