Beginner questions  modelling lift and drag on a towed body
Hello!
I need to find the lift and drag of a body being towed through water. The body is a fairly stocky torpedo shape with a tail 'ringwingthing' supported on four quadrant fins. I'm using Abaqus CAE 6.12. My basic reason for this post is I have very little idea where to start. I have a multitude of questions, and would really appreciate any tips and pointers on how to begin going about this problem. Would you model this as a 3d solid body, or is it possible to do it with axisymmetric shell elements (even considering that the fin pieces aren't continuously axisymmetric)? I have the body modelled in Solid Edge, and I've been able to import this into CAE using a Step file. I've also got a model of the water  a block with the shape of the towed body removed using a boolean operation. My original thought was to place one inside the other, with a tie representing a rope, which would tell me the forces on it and therefore I could derive the drag. However, this would require a cosimulation and my Abaqus licence doesn't have enough tokens to run one of those. I'm now wondering whether I even need to model the rope, as I think I can get drag as an output variable on the nodes at the fluidsurface interface. This led me to wonder whether I even need to model the body itself? Can I just model the block of water flowing over the shape? The body can be assumed to be rigid.  Any and all suggestions and advice would be appreciated. My background: recently graduated mech engineer, I did one brief module on FEA, which used ANSYS. I've since started work and have spent a couple of weeks doing Abaqus tutorials, only one of which has been CFDbased. While I feel I have a very basic grasp of FEA, I'm still totally at sea (excuse the pun) with CFD, and would greatly appreciate any help. If anyone knows where I could find a few more CFD tutorials for Abaqus I'd be eternally grateful. Thanks, Adam 
Hi Adam,
One aspect that you have not mentioned is whether the "object" is fully immersed or partially immersed (i.e it floats on the surface). From your post, I think that the object is fully immersed. To get to the bulk part, I would model the object as not being deformed by the water pressure acting on it (this assumption depends on the object properties). In a first pass, I would not simulate the rope as I would expect it to be thin compared to the object  but would estimates its effect using a text book expression (I am sure that there is analytical expression for the drag of a cylindrical object in water). 3D model vs axisymmetric: it depends on a number of parameters. Can the geometry be approximated as axisymetric? Does the scenario allows for axisymetry (ie is the object flowing straight on the water or slightly inclined)? What are the benefits vs drawback of an axisymetric simulation compared to a 3D (is it going to be easier to setup, does it integrate well with the software work flow)? I hope this help. Julien 
Hi Julien, thanks for replying.
The object is indeed fully immersed. On having further information I now know the object is not axisymmetrical. I also intend to model the body as rigid and undeformable. The only potentially deformable part of my model was going to be the element representing the tow cable. If I assume the body is undeformable do I even need to have a part instance for the object in the model? Can I just model the flowing water with the shape of the body removed (boolean operation) and have the nodes at the flowsurface interaction locked? Or do I need to fill that space with a rigid body part instance? I'm thinking I would actually be best to start with modelling the flow over something very simple like a perfect sphere, for which I can find exact expressions against which to match my results. I'm still generally unsure how to go about that too, though, so I am still hunting for abaqus tutorials (or particularly processdescriptive tutorials for other packages) that do flow over a rigid body. Kind regards, Adam Quote:

Hi
Hello members!
I would like to introduce myself as CFD engineer and would like to get answers from forum members. Looking forward to your kind support! Regards Michael 
Hi Adam,
I think that you are going in the right direction. I would think that the "boolean operation" is the way to go. It is the usual way for CFD solftware (ie create a computational domain representing the fluid domain only), but it is software dependent. You are proposing to use a simple sphere first (or go through tutorial) and it is the way I would recommend. Start simple and increase complexity after (see http://www.hibouscientificsoftware.c...00%28A%29.pdf). If you can find a case with experimental or theoretical results, I would recommend using it to benchmark your methods. There is a Best Practice Guidelines for CFD in marine application document available on the web (the link is in the document and in the cfdonline links section), which would probably be of interest to you. Julien 
Hi Michael,
Thanks for your post and welcome to the forum. If you want answers/help, best to start a thread and ask questions. Remember that the more information you give, the more likely you will have a pertinent answer. 
Hi Julien,
I’ve managed to get a model of a sphere inside a block but not getting the kind of wake and separation I expected. I THINK it’s because my flow field is too small and the boundary conditions are affecting the flow around the sphere (I put a 1m dia sphere inside a 2x2x4 field – I’ve now increased the field to be 4x4x16 with the sphere placed about 4m from the inlet). The new, larger model is now running. Just for reference I’ve used a noslip condition on the sphere, a dynamic viscosity of 0.1 Pa.s for water and am using a flow of 4.5m/s – do these sound like sensible parameters for getting a good view of the flow around a sphere? As this is my first mostly selfset up model (I’m using a tutorial of a two dimensional problem, flow around a rigid post, as a rough workflow guide), I’m really just looking to get results I can check against an analytical solution. Thanks for the link, I will check that out after lunch. Thanks for your help Julien, I really appreciate it. Kind regards, Adam 
Hi Adam,
I think that you are on the right track. Below is a number of parameters I would be checking the simulation against analytical/experimental solution: 1. Size of the computational domain (the one you are currently doing); 2. Mesh size (including boundary layers); 3. Convergence criteria (just run for another arbitrary 100 iterations and check the difference in drag); 4. Physical and numerical models. A quick note on item (2  Mesh size)  I am assuming that the flow is turbulence and that you are using a turbulence model: if you are using a high reynolds turbulence model, you may get a different answer when you refine the mesh "too much". Highreynolds turbulence models are made for a y+ (some nondimensional parameters at the wall) of between 20 to 100 (approximative numbers). When you refine the mesh at the wall, the y+ will decrease. If it gets below 10, the dynamic of the flow near the wall changes. For more information/details, look at boundary layer and wall functions. Regards, Julien 
Hi Julien,
I’ve finally got a model that gives me results that ‘look’ real (according to a colleague whose life work has been fluid dynamics – he can help with the theoretical side of things, but not the practical since he’s never used a CFD package, he always wrote his own programs). All of my original models returned results that took about 2 seconds (real time) to form a flow pattern and then that never changed – my new model has a wake that varies in length and once settled, shows vortices forming either side in an oscillating fashion, which is what I was expecting. The only problem is to get that difference in results, I had to increase my mesh from about 13k elements to about 90k elements, and the solver now takes all day rather than half an hour. Admittedly my mesh is not very well set up – if I want to increase the density around the sphere, I have to increase the density around much of the rest of it too. Perhaps I should spend an hour putting in a better partition system so that I can get a proper transition from a fine mesh at the sphere up to a coarse mesh in the outer regions. Regarding turbulence, I understand that my model is currently running a turbulent flow. I’m now running a 1.5m/s flow over a 1m diameter sphere, the flow is water so 1000kg/m^3 and 0.1 Pa.s dynamic viscosity. From my calculations that gives me a Re of 1.5E4, which is turbulent. Currently though, there is no turbulence in my model. I know how to add SpalartAllmaras turbulence, with both a turbulent condition at the inlet and a predefined field. However, I have no idea how to select the values for that turbulence model. On the SpalartAllmaras setup page, I can give values for Cb1, Cb2, Cv1, Cv2, Cw1, 2 and 3, Sigma and Kappa – and I have no idea what values I’d want for my model. Similarly, when I give it values for the inlet and predefined field, I can give a value for the kinematic eddy viscosity – again I have no idea what I’d put in here. Could you suggest some sensible values? The SpalartAllmaras setup page has values put in by default, which I assume I can leave as is for a ‘standard’ model. (edit: I've run the model including the default values for SpalartAllmaras turbulence with a kinematic eddy viscosity of 5e6 at input and as a predefined field and the results look the same as for the problem run without them. I've not fully compared them yet (hiccup on the licencing server) but at first glance they seem the same) My final problem now is simply going about validating the results. I’m in the process of looking for either a similarly solved problem or a description of a numerical example that I can use to compare my results, but haven’t found anything yet. I’ve not been looking for long though, but if you know anywhere I’ll definitely find a sphere example please send it my way! Kind regards, Adam 
Hi Adam,
Based on your answer, I understand that you are running a transient model (referring to your comments on vortex shedding and 2s real time). If you are interesting in the time dependent behavior (and can afford the computational resources), this is the right approach. To validate your model google "strouhal number flow around a sphere" (strouhal is a measure of the vortex shedding frequency)  see http://www.chem.mtu.edu/~fmorriso/cm...heres_1990.pdf for example. I am not sure of the framework of your modelling. If you are working for an engineering firm and doing actual design, I think that you may want to revert to a steadystate model. This will save you time and should be sufficient to get the mean drag and lift on the immersed body. You identified that the flow to be model is to be turbulent based on the Reynolds number. It would make sense to activate the turbulence model. The Cb1....Kappa are constants relevant to the turbulence model (the cfdonline wikki section should have comments on them)  I would keep them to the default unless you have lots of time or a paper that tells you that for your specific application you should use a different set (in the later I would compare them). I would set a low value to the kinematic eddy viscosity at the inlet. Again have a look at the cfdonline wikki to check the expression of kinematic eddy viscosity and how to get a value based on velocity, turbulent kinetic energy (as a % of the velocity) and length scale. My personal opinion: the kinetic eddy viscosity will dissipate reasonably quickly and will not affect your results drastically with Spalart Almaras. Difference between simulation with and without turbulence model: there are a great number of things that affect the simulation: grid resolution, time integration, space discretisation and physical model. The first three are numerical items and the last one is physical. Quite a few of them acts in similar fashion: they add dissipation to the solved variable (in other words they smooth gradients and discontinuities). In your case, you may find that the additional dissipation associated with the turbulence model is lower than the dissipation associated with other factors. This is the reason why assessing the impact of the parameters to the solution is important. You already found that increasing teh mesh from 13k to 90k (i.e increasing the mesh resolution) had a dramatic effect on your solution. You may also want to assess the effect of the timestep if you are planning to run transient simulations. Welcome to the maze of CFD. Julien 
Hi Julien,
Thanks for that great response. Right now I’m working on refining my mesh in a sensible manner – my current model was done fairly quickly and as such, increasing the mesh density at the sphere forces the density to increase throughout the whole model. I’ve managed to get it a bit coarser at the outer areas but frankly not enough. I had a think about a better way to mesh it with Abaqus that will give me a high density at the sphere and a suitably low density elsewhere. It’ll take a couple of hours to remesh it I think, but once done it should save me a lot of time overall (the 90k element model takes 8+ hours to get 60s of solved time, while my previous 13k element models took 15min!). With regard to the transient/steady state solver, and amount of time being solved for… This is where my knowledge of the program gets in the way. Unfortunately, I’ve only been able to do two CFD tutorials for Abaqus, and both used similar settings throughout most of the preprocessing. They were both 120 second solutions, and I don’t know how to alter the preprocessor to initiate a steady state solution – if it’s even possible. What I have guessed from my limited experience using the program, is that the CFD solver is much like the Explicit solver, in that stable increments appear based on the smallest element size and … yeah – I think it’s safe to say I don’t know enough about how the CFD solver works to efficiently go about tuning my model outside of what I’ve seen done in tutorials. Thanks for the links, I’ll remesh and see if I can start validating, and I’ll also ask the Dassault Systemes help service for information on running a steady state model instead. Adam P.S. Regarding mesh efficiency, can I model a quartersphere and give it the relevant degrees of symmetry? I know I could do this with FEA but I'm not sure if the same applies with fluids, given the nature of the vortices and their 'oscillatory motion'. 
Hi Adam,
I read through your post. Good luck with it all. In regards to only modelling 1/4 of the sphere: this is not going to be possible if you are running transient and expecting to see flow vortices. The behavior of the vortices is three dimensional and the symetry would not replicate the appropriate behaviour. In steadystate, the 3D nature of the turbulence is accounted for in the turbulence model and only modelling 1/4 is possible  but I would highly recommend benchmarking the 1/4 model to a full 3D model. Julien 
Hi Julien,
Thanks for your responses. I realised as I was setting up the symmetry boundary conditions that I would be putting false constraints on the model that wouldn't be there in the full model. Would I be right in thinking that approach would work for creeping laminar flow? I think the finer details of the model, such as the turbulence model to use, can all be ironed out later. I’ve realised that I have gained enough exposure to CFD that I can move on to modeling my next stage, a SUBOFF unappended body, so that’s my next move. My current crop of questions relate mainly to the usage of ABAQUS itself, so I’ve taken my current line of aid back toward the Dassault Systemes helpdesk, they’re very good. For now I expect I shall go quiet here, until I get to the next stage of my problem where I expect I'll need more general insight to fluid dynamics. :) Thanks again for all your help so far, you’ve been immense. Kind regards, Adam 
Hi everybody,
I'm going to do a degree dissertation on FSI using Abaqus CFD. I'm now considering a simple case, a circular cylinder fully immersed in a fluid domain. In this simple case I consider the cylinder as rigid and fixed. I want to work out the forces on that cylinder. I know that this is possible using Abaqus CFD but I don't know how to do. Maybe it's a really trivial question but I don't know in a practical way how to do it. I have already performed the analysis but I don't know how to extract this result. Thank you a lot Lucia 
Quote:
I actually know exactly how to do this :) Assuming you're working with ABAQUS CAE, you can't get drag data through that interface  the output is supported but it's not listed in CAE's interface. You have to edit the input deck of the model manually. You do this by right click > Edit Keywords on the model name in the list on the left of the screen. This can take a while to open depending on the size and complexity of your model. Once open, scroll down until you find a section about Field and History outputs, it is probably the last thing before the end of the deck. If there's no field/history outputs, go back to CAE and add some, then reopen the keyword editor. Look at the format of how those output requests are included in the editor. Then, use 'add after' to add in a new output request in the History Output section: *Surface Output, surface=<surfacename>, FORCE, To help you see what the format for the surface name should be, when you add your history data make sure it's of a set in the model, and copy the format but for the surface of your cylinder. You have to make a surface which are the faces making up your cylinder in the fluid domain, and the FORCE output on this surface will give you the reaction forces acting on the cylinder  in direction of flow will be drag, others will be lift/lateral force (expect no resultant for cylinder...). I have a tutorial given to me by ABAQUS' tech support which tackles this exact problem, including FSI :) I've attached it. It also includes a python script to input the model they use (since the tutorial doesn't explain how to build it yourself, but you can still open this file and see how they have built it all :)) EDIT: Uh, my attachments failed, since they're too large/wrong file type. If you leave me an email address I will contact you and help you :) Hope this helps. 
Hello Adam,
I'm trying to model flow over an immersed object by developing an FSI simulation in Abaqus. Is it possible you could share with be the tutorial you have? I would greatly appreciate it. Thanks, Jose 
All times are GMT 4. The time now is 08:37. 