Pure Drift of Surface Combatant DTMB 5415 Free to Sink, Roll, and Pitch: Tutorial 1

Transcription

1 Pure Drift of Surface Combatant DTMB 5415 Free to Sink, Roll, and Pitch: Tutorial 1 COMPUTATIONAL NAVAL HYDRODYNAMICS Surface Combatant 5512 at 0, 10, and 20 Degree Static Drift Conditions Gregory Dooley, Adam Austin, Sean Seelau Problem Description In this tutorial, simulations of pure drift of a DTMB 5512 surface combatant will be performed at static drift conditions of 0, 10, and 20 degree angles. The ship will be allowed to pitch, heave, and roll. The simulation will predict forces and moments, sinkage, trim, and roll as a function of Froude number and drift angle. Three Froude numbers will be run for each of the three angles: Fr = 0.138, 0.28, and The DTMB 5512 is a model of a surface combatant ship with a sonar dome on the bow. It has a = 3.048m. The full geometry of the ship will be used, as opposed to prior tutorials where only half the ship was modeled and symmetries were applied. The six degree of freedom solver (6dof) will be used. Table 1: Hull particulars (Bhushan et al. 2015) Simulations will be run on a ship model without the bilge keels. This is done to reduce the complexity of the grid system. Since the motion is not symmetric, the full ship geometry will be needed in the simulations, as shown below in Figure 1. Figure 1: DTMB 5512 Results will be compared to the data in the supplied 'Static Drift' files along with the experimental and CFD results summarized in Bhushan et al. (2015). (Note: In Bhushan et al., the simulation run by ReFRESCO in that document was also run without bilge keels.) Link to download report: Bhushan2015.pdf Simulation Setup For this tutorial, none of the input files need to be created. The grid files, boundary conditions file, Suggar++ input file, and REX name list file are all provided. They differ slightly from the prior tutorials, and those differences are discussed below. Link to download files: DTMB5415_PureDrift.tar.gz Grid Files There are five grids needed for each simulation. There are two grids needed for the ship, one for the background, and two refinement grids. The refinement grid is split into two parts to make all of the grid files approximately the same size. This allows Rex to run efficiently. Table 2 Description of Grid System

2 Block Name Grid Points Hull - port side HullPt.grd 87 x26 x 42 Hull - starboard side HullSt.grd 87 x26 x 42 Refinement - front half Ref1.grd 66 x 85 x 61 Refinement - back half Ref2.grd 66 x 85 x 61 Background Bkg.grd 121 x 66 x 42 Total 1,209,840 points This simulation was run with the water coming in at angles of 0, 10, and 20 from the centerline (x-axis) of the ship. An example of the 20 angle is shown below. Figure 2: Grid system showing flow angle Although the grid files for 0, 10, and 20 are provided, if you wanted to change the angle of the grid system you would need to make some changes in the Gridgen file (.gg). (There is a bug in Gridgen that causes errors if you make the changes using the individual grid files.) 1. Import the Drift0.gg file into Gridgen: Link to file: Drift0.gg MAIN MENU > Input/Output > Gridgen-Import > navigate to and select "Drift0.gg" > Open. 1. Modify the blocks. We will be rotating the 2 refinement grids and the background grids. We want to keep the ship in position along the x- axis: MAIN MENU > Blocks > Modify > select the 2 refinement grids and the background grid > Done > Rotate > Use Z-principal Axis > Enter Rotation Angle > enter number of the degrees, for example, type: Drift Angle (degrees)>done Rotate > Done Replace Blocks > Unlink Block > Done. Using the same coordinate system shown in figure 3 the the angle entered will be negative for the flow hitting the port side of the ship and positive for the flow hitting the starboard side of the ship. This same idea is applied for describing the flow velocity vector and is discussed later in this tutorial.

3 Figure 3: Rotated refinement and background grids It may also be necessary to have the ship in a different position relative to the refinement and background grids. For example, in Figure 3 above, we would want the ship to be a little higher in the picture. The steps to translate the grids is similar to the rotation steps. MAIN MENU > Blocks > Modify > select the 2 refinement grids and the background grid > Done > Translate > Enter Transl. Offset > enter the three x,y, z coordinates for the offset: 0, -0.1, 0 > Done - Translate > Done Replace Blocks > Unlink Block > Done. This will position this ship properly for the simulation, as shown below in Figure 4. The reason for this is to better capture the data coming off the far side of the ship. It should be stated somewhere that flow is coming from port so its clear why the grids need to be shift to capture the flow near the rear starboard side of the ship Figure 4: Rotated and translated grid system Once the grids have been properly positioned and rotated each of the individual grid file need to be exported as well as the full grid system, as done in previous tutorials. The boundary conditions file given for the 20 case can be used for each of the other cases as these conditions will not change case to case. The specifics of the boundary conditions for this setup will be discussed further in the next section. Boundary conditions The main difference in this case for the boundary conditions is that since the whole ship is modeled, rather than just half, you won't have the symmetry conditions for the ship and refinement and background grids. Instead, you will see the 'patched' conditions for the two halves of the ship. See the.bcs file for details. Also, when we did the simulation for this ship in Tutorial 4, we set up waves as the Input type for the Background grid, which was type #17. For this tutorial, we return to the far inlet boundary condition, type #10. Background: >>Inlet boundary condition in, #10

4 Determine flow parameters The first step is to determine the flow parameters. The flow parameters include the Reynolds number, the Froude number, and the velocity in the x and y directions (to account for the angle). The Froude number is reported in the experimental documentation. In this case, we will show the setup for Froude 0.28 at 20º. The Froude number is defined by = U / (g*lref)^0.5 and is used to find the incoming velocity by =Fr*(g*Lref)^0.5. Therefore, the corresponding Reynolds number is given by = (U*Lref) / v. For this setup, ==3.048, =9.807 / 2, and = /. The resulting incoming velocity is =1.531 /. In order to match the experimental setup as closely as possible a Reynolds number of is defined for the Fr = 0.28 cases based on the value found in the report. This value is different than the scaled value because of the water temperature at the time of experimentation, changing the kinematic viscosity of the water. The flow parameters can be calculated for the other cases using the equations and values above. Due to the fact that the flow is coming in at an angle, the velocity needs to be broken into an x and y component. For the x component, ufullspd = 1 * cos 20, and vfullspeed = -1 * sin 20 for the flow hitting the starboard side of the ship and vfullspeed = 1 * sin 20 for the flow hitting the port side of the ship. The same equations are used for the 10 cases. These values along with the Reynolds and Froude numbers are used in the Input.nml file. Input.nml In order for the solution to be solved for in a timely manner the grid system must be split in order to utilize the availability of parallel computing. A file has been included in the tar file in order to see how the grid system has been split for this specific setup. The goal of the grid split is to split each of the grids into blocks of equal size, this will minimize the wait time of processors running solutions for blocks of smaller sizes. The grids have only been split is the x direction in order to avoid any grid splitting at the free surface or at the boundary layer at the ships hull. The grid split implemented in the Input.nml file can be seen below. Figure 5. Grid definition and processer setup found in Input.nml file. From figure 5 it can be seen that two nodes will need to be requested from the HPC setup (8 processors per node). For these cases all of the processors on the first node will be used for the CFD computation and on the second node 6 processors for the CFD computation and 1 processor to run Suggar++. In total 15 processors will be utilized for this simulation but 16 must be requested to run the job if full nodes are used. Also found in figure 5 there are the definitions of the predicted grid motions. Since the ship is free to pitch, roll and heave the grid motions is3_o, is4_o, and is5_o must be defined as non-zero values. For the hull grids the "surge indicators, for pitch roll and heave are set to a value of "1" for predicted motions and for the refinement grids and background grid these same value are set to "2" for predicted motion but the mesh does not move in the these directions. This is done to maintain the original grid setup during simulation. In order to achieve a converged solution the computation was run for iterations at a time step of s* in order to properly resolve all of the ships motions. Once the time step, iterations, and flow conditions have been set the Input.nml should be ready to run. The corresponding namelist file is setup for the case with a drift angle of 20 degrees at a Froude number of Input.xml As with the boundary conditions, the main change to the Input.xml file is losing the symmetry conditions that we had when we were only modeling half the ship. Instead, we have a 'block2block' type which connects the two halves of the ship. Similarly, since the refinement grid was split into the two halves, there will be a 'block2block' connection for those as well. For the cases where the background grid and refinement grids have been shifted (10, 20 ) the grids are no longer defined in the Cartesian coordinates. This issue is resolved by removing the statement cartesian_g rid = "yes", found in the volume grid definitions for both of the refinement grids and the background grid. The new definition can be found in the figure below.

5 Figure 6. New volume grid definition for rotated grid cases Post Processing Calculating Forces and Motions Calculate the forces and motions using the output files from Rex. The forces in the X and Y directions are calculated by using the ctotxs and ctotys values from the.forces1 file. X = 2 * ctotxs * (Lpp/Tm) Y = 2 * ctotys * (Lpp/Tm) For pitch, heave and roll, values from the.output_motions1 file are used. For heave, Heave = xb3lpp For pitch and roll, the values output by Rex are in radians, so the values will need to be converted to degrees. Pitch = xb5 (degrees) Roll = xb4 (degrees) In order to remove some of the "noise" from any oscillation in the solution a moving average should be taken from the 7000 iteration on for all of the solution being analyzed. Overall converged values are then to be plotted against Froude number and drift angle. An example of these plots can be found in the figure below.

6 Figure 7. Potential plot of heaving motion versus Froude number for all of the drift angle cases to be run with provided experimental data included for comparison. Figure is missing These non-dimensionalized values can now be directly compared to the experimental values included in the files given for CFD validation. Free Surface and Flow velocity (Slice) Contour Plots The th iteration output files were used to create a free surface contour plot and the flow velocity slices for comparison to the other CFD computations found in Bushan et al. (2015). The *_10000.p3dpuvwf and *_10000.p3dxyzi output files are to be loaded into Tecplot for these plots. The free surface contour plot can be setup using the same instructions found in Tutorial 3. A contour plot of the flow velocity around the ship's hull is to be created using the "slices" option found in Tecplot. The slice is to be done in the X- plane and for this case we will defined at X = The I-blanking previously defined for the free surface plot should also be followed for this plot. This is done by checking the " Obey source zone blanking" box. This definition can be seen in the figure below. Figure 8. Slice location definition in Tecplot Once the slice is defined the contour to be plotted must be defined. Click on the contour tab in the same slice "Slice Details" window shown in figure 8. The contour type should be set to "Flood" and the flood by definition should be set for "RHO-U". Once this is defined the details of the RHO-U contour need to be defined. The color distribution of the contour should set to " continuous" with a minimum value of 0 and a maximum value of 1 for easy comparison of the plots found in the report. The contour levels must also be set with the same values with a total number of levels set to 6. The full setup can be found in the figures below. Figure 9. Contour Details and contour levels setup.

7 For easy visualization of the flow, the contour was also plotted with vectors. The full and final set up for a slice at X =0.935 for the Fr = 0.28 and a Drift Angle of 20 can be seen in the figure below. Figure 10. Contour plot of flow velocity for Fr = 0.28 and D = 20 at a location of X = References 1. Bhushan, S., Yoon, H.., Stern, F., Guilmineau, E., Visonneau, M., Toxopeus, S., Simonsen, C., Aram, S., S-E Kim, and Grigoropoulos, G., "CFD Validation For Surface Combatant 5415 At Straight-Ahead And 20 Degree Static Drift Conditions," IIHR Technical Report # 493, February 2015.