
[Sponsors] 
Forces in interFoam laminar simulation (based on DTCHull tutorial) 

LinkBack  Thread Tools  Search this Thread  Display Modes 
June 26, 2020, 04:52 
Forces in interFoam laminar simulation (based on DTCHull tutorial)

#1 
New Member
Sharath Srinivasamurthy
Join Date: Aug 2019
Location: Osaka, Japan
Posts: 4
Rep Power: 7 
Hello Foamers
Thought is it better to start a new thread for the question. Target of the CFD simulation  Evaluation of multihull ship resistance based on DTCHull. Using version 5.x. Using symmetryPlane feature. The simulation type is laminar due to low Reynolds number (model scale simulation to compare with model scale experiment results). turbulenceProperties file is changed accordingly. In postprocessing of forces, pressure and viscous forces are obtained. When obtaining the Cf (coefficient of viscous force) value, wetted surface area of half hull needs to be used (as per my understanding). However, if we use half hull wetted surface area, the viscous coefficient is not correct when compared with Blasius solution. But if we consider the full hull wetted surface area, it matches with the Blasius equation. I am really confused with the reason for it. Therefore, now considering if the modeling of simulation (setup conditions) are correct or not. Please help with some insights especially if you have used DTCHull tutorial. Thanks in advance. Sharath 

November 26, 2020, 19:15 

#2 
Senior Member
Claudio Boezio
Join Date: May 2020
Location: Europe
Posts: 137
Rep Power: 7 
Hello Sharath,
Does this happen if you let the function objects calculate the Coefficients of Resistance? I calculate the coefficients manually after the simulation and never used the function objects for that. I would need to try that out. I recommend using the wetted surface area of the entire hull (not just half), and double the forces for calculating the Coefficients of Resistance. After all, the quantity of interest are the resistance forces for the both sides of the hull, not just half. You can also use the forces of just one half and then half the wetted surface area to calculate the coefficients, the result is the same. 

November 27, 2020, 03:33 

#3 
New Member
Sharath Srinivasamurthy
Join Date: Aug 2019
Location: Osaka, Japan
Posts: 4
Rep Power: 7 
Hello Claudio
Thank you very much for your response and suggestion. I verified the results of DTCHull tutorial and it indeed outputs the halfhull resistance forces. So, double the forces for calculating the coefficients of resistance is correct, while using wetted surface area of entire hull. Sorry for the confusion about halfhull and fullhull wetted surface area previously. It is resolved now. Further, I have now continued the laminar simulations. My target is to obtain coefficients manually from the resistance forces and compare the viscous coefficient with Blasius solution (like comparing the viscous coefficient with ITTC line in case of turbulence simulation). However, until now, they do not compare well and I suspect it is mainly due to my grid resolution (meshing). Error in prediction is about 40% which is quite high (between Blasius solution and viscous coefficient of laminar simulation). Would be grateful if I can get some pointers/suggestions on laminar simulation of hull resistance using OpenFOAM. Is there any specific setup conditions? Thank you. Sharath 

November 30, 2020, 09:14 

#4 
Senior Member
Claudio Boezio
Join Date: May 2020
Location: Europe
Posts: 137
Rep Power: 7 
Hello Sharath,
Have you tried calculating let's say the DTC Hull Tutorial with simulationType laminar? So far I have been focusing on meshing and getting the wave resistance as close as possible to published model test results. I've noticed though, that viscous resistance strays a lot, depending on whether turbulence is on or off and the mesh has a few layers of boundary cells at the hull wall or not. What I've also noticed, is that often when I stop the simulation (by letting it reach endTime) and restart it again from there, the viscous resistance makes a jump, not sure why but this seems odd to me. There might be something wrong. I'm not sure whether the mesh resolution has the same effect on the accuracy of the viscous resistance as it has for pressure resistance. May I ask why you are interested in calculating the viscous resistance in the laminar regime? The Reynolds number for the model (approx 6 m length on waterline) is in the millions, thus well in the turbulent regime. I'm calculating the DTC Hull right now, but with a custom made mesh that has no boundary layers yet. While turbulence is on and I use the nutkWallFunction instead of the tutorial's nutkRoughWallFunction, the viscous resistance is way too high, in excess of over 50%. As soon as I manage to get snappyHexMesh or cfMesh to reliably add boundary layers with the thickness I want, I'll see how the viscous resistance compares with the published model test results. However, the published viscous resistance of model tests is oftentimes calculated with the ITTC 57 correlation line anyway. So even if you manage to get turbulence to work properly, that's what you are likely to compare against. If you're just interested in estimating the hull resistance, you could always use OpenFOAM to calculate the pressure resistance and add the viscous resistance by using the ITTC 57 correlation line. That should be reasonably accurate. Viscous effects have an influance on the wave pattern, but I think the difference to be small. Please keep me posted on your progress if you like, I would like to hear how it goes for you. Cheers, Claudio 

December 11, 2020, 03:11 

#5 
New Member
Sharath Srinivasamurthy
Join Date: Aug 2019
Location: Osaka, Japan
Posts: 4
Rep Power: 7 
Hello Claudio
First of all, please accept my apologies for the late response. Thank you for your reply. I tried simulationType laminar inside turbulenceProperties file for the DTC Hull tutorial. Unfortunately, it does not work. I would like to explain the research topic for clear explanation. I want to determine the hull resistance of a small multihull vessel (Length of the single hull is about 1.2 meters). Further, we conducted 1/3 scale model experiment for the multihull vessel. Therefore, for validations, length of the single hull in simulation is about 0.4 meters. Reynolds number is around 1.7E05 (laminar regime) for the lowest velocity case. While using forced turbulence simulations, it was found that simulation hull resistance predicted was way different from the experimental value. Therefore, decided to employ laminar regime. DTCHull tutorial is the base tutorial employed with changes to simulationType laminar and I recreated the domain to suit our vessel (single hull for now). I have been trying to add more boundary layers (about 6 layers for now) using snappyHexMeshDict corresponding to thickness assumption of a flat plate (laminar thickness). Though, I have not been able to achieve mesh convergence yet. Now, I'm thinking of (i) increasing boundary layers further, (ii) refine grid further. Thank you for your suggestion regarding the viscous force through correlation line. Since the regime is laminar, I'm using Blasius solution to compare the simulation viscous resistance for now. It is a reasonable solution to calculate pressure resistance from OpenFOAM and assume Blasius solution for viscous resistance. I will update you further if I have much more progress. Thanks for your time and insights. Cheers Sharath 

Tags 
dtchull tutorial, resistance estimation, wetted surface area 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
laminar and turbulent flow simulation in elbow fitting to find K values wtr Re  prashanth1234  FLUENT  4  January 18, 2019 11:06 
Residuals and forces spiraling out of control before failing  edomalley1  OpenFOAM Running, Solving & CFD  3  September 7, 2018 11:42 
Terminate simulation based on probe  Bernhard  OpenFOAM Running, Solving & CFD  18  September 11, 2014 11:54 
Boundary conditions for hassan hemida interFoam tutorial  vishal_s  OpenFOAM PreProcessing  0  August 21, 2013 01:21 
Strange results from interFoam solution converges but sum of all forces not equal to zero  nicasch  OpenFOAM Running, Solving & CFD  0  April 15, 2008 03:01 