CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM

Forces in interFoam laminar simulation (based on DTCHull tutorial)

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 26, 2020, 04:52
Post 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: 3
sharath.murthy is on a distinguished road
Hello Foamers
Thought is it better to start a new thread for the question.


Target of the CFD simulation - Evaluation of multi-hull 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 post-processing 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
sharath.murthy is offline   Reply With Quote

Old   November 26, 2020, 19:15
Default
  #2
Member
 
Claudio Boezio
Join Date: May 2020
Location: Europe
Posts: 59
Rep Power: 3
Ship Designer is on a distinguished road
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.
Ship Designer is offline   Reply With Quote

Old   November 27, 2020, 03:33
Default
  #3
New Member
 
Sharath Srinivasamurthy
Join Date: Aug 2019
Location: Osaka, Japan
Posts: 4
Rep Power: 3
sharath.murthy is on a distinguished road
Hello Claudio

Thank you very much for your response and suggestion. I verified the results of DTCHull tutorial and it indeed outputs the half-hull 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 half-hull and full-hull 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
sharath.murthy is offline   Reply With Quote

Old   November 30, 2020, 09:14
Default
  #4
Member
 
Claudio Boezio
Join Date: May 2020
Location: Europe
Posts: 59
Rep Power: 3
Ship Designer is on a distinguished road
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
Ship Designer is offline   Reply With Quote

Old   December 11, 2020, 03:11
Default
  #5
New Member
 
Sharath Srinivasamurthy
Join Date: Aug 2019
Location: Osaka, Japan
Posts: 4
Rep Power: 3
sharath.murthy is on a distinguished road
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 multi-hull vessel (Length of the single hull is about 1.2 meters). Further, we conducted 1/3 scale model experiment for the multi-hull 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 re-created 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
sharath.murthy is offline   Reply With Quote

Reply

Tags
dtchull tutorial, resistance estimation, wetted surface area

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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 Pre-Processing 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


All times are GMT -4. The time now is 18:39.