# how to quantify numerical dissipation

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

 November 3, 2005, 09:30 how to quantify numerical dissipation #1 MÃ¡rcio Ricardo Guest   Posts: n/a Hi, is there a general way to quantify numerical dissipation regardless of the spatial discretization scheme, if you're not using upwind? I'm working with FEM (2D incompressible, fractional step), and I'm getting a laminar pattern for a Re = 500 around a cylinder with about 10000 points in the mesh. Also, when running cavity flows, I can't get the top left vortex that appears after Re = 2500. For this Reynolds I'm using 165 X 165 points, but I've tried with 215x215 and the result was the same. TIA Márcio Ricardo

 November 3, 2005, 10:44 Re: how to quantify numerical dissipation #2 diaw Guest   Posts: n/a Marcio, Check your scaling method - if you use one. In other words, if you draw in millimetres. I scale firstly on residence time through the model & then on Reynold's number. The first scaling - if not performed will result in the same Re, but will not give the correct time-relationship. Try it & see if it changes your result. diaw...

 November 3, 2005, 13:29 Re: how to quantify numerical dissipation #3 MÃ¡rcio Ricardo Guest   Posts: n/a Thanks, diaw. I'll try it. I'm running on a scale 1:10 ( my characteristic length is 10 times lower than the physical length: for a given Reynolds I use a velocity profile u = 1.0 and a length = 0.1, and then the viscosity is 10 times lower too, with a unity-density). -Márcio Ricardo

 November 3, 2005, 16:18 Re: how to quantify numerical dissipation #4 Mani Guest   Posts: n/a Good question. There is certainly some information about numerical dissipation buried in your discrete equations, but to analyze them including all aspects of the method can be quite difficult. Of course, the obvious (and useless) answer to your question is this: If you know the exact solution, compare it with your numerical solution, and you can extract the numerical dissipation. Well, one thing you can do is increase the grid and time resolution (significantly... at least by a factor of 2). This will effectively reduce any numerical dissipation. If that doesn't solve your problem, I would tend to think that there is something else, aside from numerical dissipation, affecting your results. About the cylinder, what do you mean by "laminar pattern"? On the wall, in the wake....? The wake (starting with the separated shear layer) should become turbulent first, before the boundary layer transition, as you increase Re above 180. One thing you should be aware of, though: 2D flow at Re=500 doesn't exist in reality. At that Reynolds number the wake is three-dimensional. That may or may not be linked to turbulence... And also: 10000 points seems quite low for this kind of flow. Are you using high-order discretization?

 November 3, 2005, 17:15 Re: how to quantify numerical dissipation #5 MÃ¡rcio Ricardo Guest   Posts: n/a >>laminar pattern: The flow past the cylinder looks like at Re=30, 40. There is only a static bubble downstream, which is less than 1D long. At Re = 500, even knowing that the flow is three-dimensional, I expected some kind of vortex shedding. >>number of points and order of discretization: The exact number of points I'm using is 16142, shared by 3978 quadrilateral elements. I'm using 2nd order lagrange elements for the velocity (9 nodes per element) and 1st order elements (4 nodes per element) for the pressure. I'm using constant weight functions (CVFEM), and the formulation is based on weighted residuals, not variational formulation. If the problem is not numerical dissipation, could this be some kind of error in the spatial discretization of the advective term? Thanks in advance Márcio Ricardo

 November 3, 2005, 18:16 Re: how to quantify numerical dissipation #7 Mani Guest   Posts: n/a .... and some more questions: What initial conditions do you use for the unsteady flow computation, what time-step did you choose, and how many time-steps did you run?

 November 4, 2005, 06:47 Re: how to quantify numerical dissipation #8 MÃ¡rcio Ricardo Guest   Posts: n/a The domain dimensions were: a rectangle with L=5, H=2.5, a circular cylinder with D=0.1 located at x=1.65 from the west boundary at y=1.25. The time step was dt=0.0003 and I've run 162000 time iterations. I always use density = 1.0 and set the Reynolds number only by varying the viscosity. The initial conditions were u, v, p = 0 in the whole domain. As boundary conditions, a unity velocity profile on the west face, and on the south, east and north faces I used homogeneous neumann bcs for vel, with p=0 on them. Of course, u = v = 0. on the wall, dp/dn = 0 on it too. Also, in my fractional step scheme I did not include the pressure in the intermediate velocity equation. This leads to a 1st order scheme for pressure, but the velocity is still 2nd order in time, isn't it? I'm using explicit time advance with Adams-Bashforth for convective terms, with a lumped mass formulation for the transient term (diag(Mij) = sum_j(Mi), off_diag_i = 0); Thanks a lot. I'll check the paper right now. Márcio Ricardo

 November 4, 2005, 07:26 Re: how to quantify numerical dissipation #9 Renato Guest   Posts: n/a Have you got a convergent solution, for Re 500, starting up your problem from a stationary velocity field withou any kind of Reynolds ramping strategy? " ...By the formulation you are working (CVFEM) I guess you are from UFSC in Brazil, am I right? ... " Renato.

 November 4, 2005, 07:50 Re: how to quantify numerical dissipation #10 MÃ¡rcio Ricardo Guest   Posts: n/a Yes, I've got a convegent solution, but not a satisfactory result, as I've posted. I'm brazilian, too, from Federal University of Uberlândia - MG(UFU). Actually, I'm with 2 advisors, one from here and the other from UNESP at Ilha Solteira. We look at CVFEM just like any other finite element method, by calculating the element matrices, assembling them on a global matrix and so on. I'm not sure, but I think in UFSC they use the method as an unstructured finite volume method, the shape functions and derivatives being used just to calculate variable and flux values at the control volumes faces, but no element matrices are assembled. Indeed, professor Maliska call their method "Element-based Finite Volume Method".(Anyone from UFSC please correct me if I'm mistaken). You work with FEM too, don't you? -Márcio

 November 4, 2005, 08:09 Re: how to quantify numerical dissipation #11 Renato Guest   Posts: n/a Yes, I'm from COPPE/UFRJ and I've been working with edge-based stabilized finite element formulation (SUPG/PSPG to be more specific) with linear tetrahedral elements. I've just finished to implement the parallel transient part of my code and ran this problem for Reynolds 100 to validate my implementation. The result seems to be fine up to now and I haven't ran this problem with Re 500 because I intend to implement some kind of LES-based turbulence before (maybe a standard Smagorinky model before something more sophisticated). It's good to find another Brazilian here... We could keep in contact (rnelias@gmail.com) Regards Renato.

 November 4, 2005, 08:43 Re: how to quantify numerical dissipation #12 MÃ¡rcio Ricardo Guest   Posts: n/a I'm thinking about using SUPG too, but in a CVFEM fashion. I've seen it in the paper "A flow-condition-based interpolation finite element procedure for incompressible fluid flows" [ Bathe and Zhang, Computers and Structures 80 (2002) 1267â€"1277] They use SUPG for the advective term only, but their formulation is based on a discontinuous finite element method, which I'm not familiar with. For a 9 noded quad element, they take patches of 4 noded sub element and use linear shape functions in it. The weight functions are unity-constant too, and split each patch in four sub-control volumes. Do you know this method? Regards Márcio My email: pivello@gmail.com

 November 9, 2005, 10:38 Re: how to quantify numerical dissipation #14 diaw Guest   Posts: n/a Mani wrote: As a rule of thumb, keep your free-stream boundary about 30-50 diameters (or chord lengths) away from the object (cylinder, airfoil...). --------- Excellent point. Can I ask how you specify the 'free stream boundary' - assuming you are refering to the top & bottom lateral boundaries? Do you set a velocity & pressure condition - or 'do nothing'? I would heartily agree to set any lateral boundary imposition as far away as possible, in order to minimise its interference. --------- Mani wrote: Depending on your time stepping scheme (let's say second-order), you will need in the order of 50-100 time steps per oscillation period. The period is given by T=1/f,... ---------- Very good advice. What is the '50-100 time steps per oscillation' based on? I guess experience? Thanks for that shared wisdom, Mani... diaw...

 November 9, 2005, 14:25 Re: how to quantify numerical dissipation #15 Mani Guest   Posts: n/a >Can I ask how you specify the 'free stream boundary' Diaw, I suppose it depends on the equations you are solving. With a compressible code I am typically using a quasi-1D Riemann approach as a non-reflecting farfield boundary condition.There must have been early studies on the distance requirements, depending on the BC, but don't ask me about references. These rules of thumb are passed down from researcher to researcher to become common knowledge. In case of the cylinder I actually did check on convergence as the distance to the boundary is increased. It's not a clear-cut case, because the wake is never going to be "undisturbed farfield", even far downstream. The question there is: How far downstream does the wake still induce an influence on the cylinder? And: How far downstream do you actually get an accurate solution near the wake, considering the numerical diffusion of the wake? >What is the '50-100 time steps per oscillation' based on? I guess experience? Yes, others' experience as well as my own, specifically for the laminar cylinder. You need a certain temporal resolution to minimize numerical dissipation, which would alter the vortex-shedding frequency or even suppress shedding altogether (damping effect of numerical "viscosity"). In that sense, Marcio's initial question on numerical dissipation really hits a nerve, but a solution to this problem is relatively straight-forward: increase both spatial and temporal resolution.

 November 9, 2005, 21:15 Re: how to quantify numerical dissipation #16 diaw Guest   Posts: n/a Mani, Thanks so much for the excellent comments. I have noticed that the proximity of boundaries, coupled with their influence on the 'wave nature' of the flow field certainly has a very significant effect on 'stiffening' the equivalent bulk modulus of the system. I call this 'container effect'. This effect thus alters the 'second viscosity' of the fluid 'system'. The temporal & spatial discretization requirements again seem to correspond to those required to resolve a very low-speed event in a 'wave field'. I term this the 'viscous shock, or bump'. I have seen effects in 1D at speeds as low as 0.5 mm/s. This phenomenon is the thing we have been smudging out with upwinding & convection-stabilisation. In corresponds to the 'onset of unstable flow', but really only becomes dominant when large-enough to overcome the viscous damping of the fluid & system. diaw...

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Flo Main CFD Forum 6 January 25, 2008 13:35 zwdi FLUENT 2 June 3, 2004 21:09 QU KUN Main CFD Forum 2 February 23, 2004 04:46 Praveen Main CFD Forum 0 September 6, 2002 07:09 sam Main CFD Forum 0 June 22, 2002 19:14

All times are GMT -4. The time now is 19:09.