Fluids

Fluids

Fluent equivalent to “opening” boundary in CFX?

    • simonhackett
      Subscriber
      Hi everyone, new to posting here so apologies for any formatting issues. nI am using a student license of 2020 R1.nI have completed one-way FSI analysis of a sounding rocket fin, and I am now trying to take what I learned from my one-way simulation, which uses Fluid Flow (CFX) and Static Structural analysis systems, to a two-way simulation using Transient Structural and Fluid Flow (Fluent) systems with system coupling. Those three things are all new to me so I expect it to be tricky. nIn my model, there is a boundary which gets counted as an opening, since I have only modeled a block of air around the fin. I'm just wondering which of the boundary options in Fluent are equivalent to that in CFX. nI expect I'll have lots of other questions, but I've been able to follow tutorials I found online up to this point.n
    • DrAmine
      Ansys Employee
      Pressure outlet is equivalent to CFX opening.n
    • simonhackett
      Subscriber
      Thank youn
    • simonhackett
      Subscriber
      HiArray,I understand it's been a while since you responded but I was hoping you might be able to help me here.nAfter doing some work with my two-way FSI simulation, I realized that convergence of the Fluent system was my biggest issue so I have now started to work on that alone.nAfter getting it to solve, I put in a pathline from the inlet and it appears that lots of particles immediately veer off into what should just be a 0 Pa gauge pressure opening, rather than travelling relatively straight through to the outlet. If I start the pathline at the fin wall surface, the same thing happens:the lines immediately shoot towards the nearest opening surface. I plot 400 pathlines, and none of them even come close to going through to the intended outlet. This results in a basically nonexistent pressure profile on my fin geometry.nHere is a screenshot of my pressure-outlet settings:nAnd here is the resulting pathline in Fluent:(the outlet boundary is the surface on the right, and a pressure contour on the fin is included)nVersus what I see in CFX using the opening boundary condition:nHave I just set this up incorrectly with the wrong settings for a properly behaving free stream style opening?n
    • Rob
      Ansys Employee
      Have a look at the flow field and pressure (contours) to see what's going on. If you have one inlet and multiple outlets why would the flow prefer one over the other? n
    • DrAmine
      Ansys Employee
      Plot velocity vectors at mid plane and add more details about all BCs.n
    • simonhackett
      Subscriber
      HiArray, nI'm not sure what you mean by flow field I already show what the particle pathlines look like coming from the inlet, but the pressure contours on the fin are basically nonexistent, especially compared to CFX. It doesn't make sense to me why the flow would favour one outlet over the other. My only guess is that my settings for the free stream outlet are incorrect.nArray, See below for all the boundary condition windows. For more reference, I'm using the pressure-based viscous physics model with default k-epsilon. I don't know what you mean by velocity vectors at mid-plane though. Boundary conditions are inlet, free stream, outlet, fin, and fuselage:nPlease let me know if any of these settings could be what is causing my problems. Once again, I've just tried to recreate the same case as what I have been working with in CFX.n
    • DrAmine
      Ansys Employee
      Model settings CFX vs Fluent ? Compressiblity effects? Convergence in Fluent? n
    • simonhackett
      Subscriber
      I just realized something that could have been causing issues. I did not set a value for number of iterations in the calculation, so it must have only been calculating once. I now set it to 20 and then ran it again at 150, and the results look better but still not great (it could just be that Fluent is more detailed than CFX and these results are more realistic)nnModel settings CFX vs Fluent ? I can paste screenshots of the setup in CFX if that would help. I'll open it up now and try to summarize. Air as ideal gas, continuous fluid, 1 atm reference pressure, non-buoyant. Heat transfer is by total energy, k-epsilon for turbulence. The inlet follows a supersonic flow regime, 0 Pa relative static pressure, 686 m/s, high intensity turbulence, 2.5 degrees C static temperature, outlet is supersonic as well. The walls are no-slip with 3.2 micron roughness, adiabatic heat transfer. That's basically it for CFX. Let me know if I'm missing any details. nCompressiblity effects? I'm not sure where to check this, the tutorials I have been following never mentioned it.nConvergence in Fluent? I don't know how to check convergence in Fluent alone. I used this same setup with system coupling for two-way FSI and Fluent was not converging, so now I am diving deeper into Fluent. Here is a plot of the residuals though: nMaybe I just need to run for more iterations? This just becomes a problem for FSI as my computer can only handle so much. It took nearly an hour and a half to run 200 iterations of the coupled FSI system, and I need to increase that already as I want to get more than just one second of real time simulated. n
    • Rob
      Ansys Employee
      That solution isn't converged, you're looking for flow residuals below 1e-3 and good mass conservation. Some of this is covered in the tutorials. nLooking at the fin, how much does it move? FSI is good where the flow is affected by the moving geometry, it's less necessary where the two are fairly decoupled. Focus on the flow side of the model and work through the tutorials to get a good flow solution. Then apply that to the FSI problem. nGases are assumed to be compressible above about 0.3M This is a rule of thumb so can be bent somewhat, however 686m/s in air would be over Mach 2, so you'll have shockwaves to contend with too. You definitely need to get the CFD model right before trying FSI under those conditions. n
    • DrAmine
      Ansys Employee

      That solution isn't converged, you're looking for flow residuals below 1e-3 and good mass conservation. Some of this is covered in the tutorials. Looking at the fin, how much does it move? FSI is good where the flow is affected by the moving geometry, it's less necessary where the two are fairly decoupled. Focus on the flow side of the model and work through the tutorials to get a good flow solution. Then apply that to the FSI problem. Gases are assumed to be compressible above about 0.3M This is a rule of thumb so can be bent somewhat, however 686m/s in air would be over Mach 2, so you'll have shockwaves to contend with too. You definitely need to get the CFD model right before trying FSI under those conditions.https://forum.ansys.com/discussion/comment/97073#Comment_97073

      I agree with Rob here. Forget about FSI first. As you have supersonic flows. providing a velocity inlet boundary is lazy as stagnation properties are not fixed. Here the recommendation to provide total properties.n
    • simonhackett
      Subscriber
      ,ndo you mean how much the fin moves for the one-way FSI? Maximum displacement is about 0.2 mm at one part of the tip of the fin.nWhich tutorials should I be following to achieve the desired convergence? I have a copy of the Fluent guide now, it?s a bit daunting and I don?t know where is the best starting point. Without first reducing the size of the bounding box, I cannot increase the mesh density much more, I?m very close to the node limit for my academic license. So if I increase the mesh density somewhere, I have to decrease it somewhere else.nIs there anything you?d recommend I can change or look at to deal with the compressibility effects?n,nI agree, I am currently only looking at the Fluent system completely standalone from the mechanical coupling in a new project file. I have only been using FSI results for context.nWhat do you mean by provide total properties?n
    • Rob
      Ansys Employee
      Have a look at the NACA examples in the online help, that'll give you an idea re compressible flow, but you'll also want to review how supersonic flows behave. The bounding box needs to be big enough to not alter the result, but you can coarsen the mesh towards the outer region provided that also doesn't effect the results: not always easy with a limited cell count. nis referring to the pressure and far field boundaries where you define the total pressure & temperature. Although you can add a total pressure to a velocity boundary too. It's to make sure the gas density is correct as otherwise the upstream conditions are not sufficiently defined and the gas density will be wrong. n
    • DrAmine
      Ansys Employee
      If flow is compressible and that is compressible with your large Mach number a velocity BC is lazy. Total pressure, Total Temperature, Direction of Flow, Static Pressure are required at supersonic inlet!n
    • simonhackett
      Subscriber
      Array,nAre you referring to chapter 27 of the Fluent Tutorial Guide (In-Flight Icing Tutorial Using Fluent Icing)? I'm unfamiliar with the Online Help portal, I don't see anything else that mentions a NACA airfoil. nI'm going to need to dig a bit deeper it seems, I'll be back if I run into any other issues but certainly my next goal is to fully define the problem.nArray,nWhen you say total pressure and total temperature, where are these input into fluent? I realized I was simulating without checking the energy box, so now I have defined the temperatures of my boundaries. I'm still not sure where to define the total pressure and static pressure though. The velocity is defined with magnitude normal to boundary so I think that is enough for flow direction. nLike I stated above, I am looking over the guide for icing of the clean NACA0012 airfoil. It won't be exactly the same as my problem definition but it should hopefully be a better starting point.n
    • Rob
      Ansys Employee
      Total pressure etc are set in the Pressure boundary panels and/or far field depending on what you use. nI was referring to the NACA airfoil tutorial, I think there's one in the Help, but it may be in the videos. I'm more familiar with the (paid for) training materials than the free ones as I teach the former. n
    • DrAmine
      Ansys Employee
      So basically you did not account for compressibility of flow. Now enable energy equation and try to use pressure inlet boundary.n
    • simonhackett
      Subscriber
      Array, I think I found the one you mean. There's some helpful stuff in it that should hopefully help me get a bit further with this. Thanks for the advice.nArray, when you say enable energy equation is this checkbox what you mean? nI have that activated and energy equation is selected under solution>controls, but I'm unsure what you mean now by using the pressure inlet boundary? If I change the inlet to a pressure inlet then I cannot define the velocity. Do you mean to calculate the dynamic pressure based on the defined velocity?n
    • DrAmine
      Ansys Employee
      Yes:again compressible flow (ideal gas EOS to get started) requires pressure inlet or far field. You can for sure use velocity boundary but that is again lazy but can work. n
    • simonhackett
      Subscriber
      ,I see. I'll look into that as it's been a while since I've done some fluids calculations. Is it still valid to define 0 gauge pressure and the outlets?n
    • DrAmine
      Ansys Employee
      Yes is valid if the absolute pressure is plausible. (Gauge+operating)n
    • simonhackett
      Subscriber
      thank you. I just want to make sure I'm understanding the documentation for a pressure inlet (compressible, supersonic flow) correctly. This is the equation given for calculating the Gauge Total Pressure:nIn this equation, p_s is the Supersonic/Initial Gauge Pressure? Is p_s intended to be calculated with Bernoulli's equation using the operating pressure as the reference, or am I getting this mixed up?n
    • DrAmine
      Ansys Employee
      No using isentropic relation ( what you shared). Ps being an absolute static pressure. n
    • simonhackett
      Subscriber
      ,sorry I think I might be getting confused. So the Supersonic/Initial Gauge Pressure is also calculated with that isentropic relation?n
    • DrAmine
      Ansys Employee
      No: the relation is to get the link between total and static pressure. You need to know both or you know static and Mach or Total and Mach. That is an input.n
    • simonhackett
      Subscriber
      ,I don't really understand what the Supersonic/Initial Gauge Pressure is calculated based off of then. Really all I know for this are the operating pressure (101325 Pa) and Mach.n
    • DrAmine
      Ansys Employee
      Then you miss an input. n
    • simonhackett
      Subscriber
      ,oh I see. I was under the impression that both fields were required. So then I would input my total pressure, using the isentropic equation, with operating pressure used as reference?n
    • DrAmine
      Ansys Employee
      No you need to know either one of the pressures. Look You do not know rge static pressure at inlet that is something what you actually need to know if you are supersonic. For that reason you need to live with velocity inlet.n
    • simonhackett
      Subscriber
      ,so what you're saying is that because this problem is theoretical and not based on measurements (of either static or total pressure), I can't use the pressure inlet boundary.n
    • Rob
      Ansys Employee
      You can, but you need to know the total pressure. If you look at the NACA airfoil examples (YouTube etc) one of them should run through the calculations. Basically, the data is needed to get the incoming gas density correct. n
Viewing 30 reply threads
  • You must be logged in to reply to this topic.