Riflex modeling from scratch Goal: Analyse a system with a flexible riser hanging from a semi-submersible vessel. Description of final system: A riser is positioned from the sea bottom to a riser base on a semi-submersible vessel. The riser base is connected to the ship 60 m downstream of the riser bottom connection and 10 m above sea level. The water depth is 100 m. The vessel motions are described in the file rao.inp. The ship position is 82.321 m downstream from the riser bottom connection and 1.34 m left. The riser has a mass of 100 kg/m and a diameter of 250 mm and thickness 75 mm. The riser has a quadratic drag of 100 Ns2/m3 and added mass of 50 kg, in normal direction to the riser. The riser has buoyancy elements connected to the pipe between 10 and 60 m from the bottom connection. The buoyancy elements can be modeled as a pipe with an effective external area of 0.3 m2, added mass of 200 kg in both transvers and longitudinal direction and quadratic drag of 250 Ns2/m3 in tangential direction and 200 Ns2/m3 in normal direction to the pipe. The other parameters are the same as for the riser. The fluid in the riser has a density of 1000 kg/m3. The following environment should be used: waves defined by a numerical spectrum, where the spectral value is 3.259e+04 m2s/rad between the rotational frequency of 0.522 and 0.524 and zero otherwise. A current which is 1 m/s at sea level, 0.9 m/s 10 m above sea bottom and 0 at sea bottom should also be used. Some tips: If you get confused with the window layout it is always possible to choose Window > Reset window layout If you make an error, type Ctrl+z to undo. Prerequisites: Be in an open workspace 1. Create a new RIFLEX task Right click in the browser, select New> RIFLEX Task Name the task Flex in the wizard Right click the Flex task and choose Open 3D View to open the graphics view: Zoom in on the the sea surface by clicking in the 3D-view and then using the scroll wheel of the mouse, or (when the mouse cursor is over the 3D graphics) by pressing and holding both the left and right buttons on the mouse and move it away from you. Pan the camera by pressing and holding the left mouse button and (while it is pressed) move it up/down/sideways. Expand in the folder system browser to the right to see the different parts of the model Under model folder, and location folder, double click on Flat bottom: Set position > z to –100 m to create a 100 m water depth. Double click directly on the location folder: Set Water Depth to 100 m. This sets the hydrodynamic water depth used to calculate the hydrodynamic forces. Right click on the model folder and choose New > Support Vessel: Set name to VESSEL Include RAO file, rao.inp (Get the file from the SIMA-INSTALLATION-FOLDER\resources\riflex folder) Double click on VESSEL to open editor window: Set initial position to: X Y Z Rz 82.321 1.34 0 30 Choose Geometry type Geometry file, and select file vessel.hsf (Get the file from the SIMA-INSTALLATION-FOLDER\resources\riflex folder) Let all translation/rotation be 0 and scaling in all directions 1 The SIMA workspace should now look like this: 2. Create cross sections Right click on folder Slender system and create New > Axisymmetric cross section: Axisymmetric cross section is a description of the cross section defined by outer and inner area of the pipe Name it RiserCRS Set the properties of the RiserCRS: The temperature is set to default. We want this to be 20 degrees. Right click on the default value and chose Set to editable. Set the value to 20 Chose default stress calculation, and set the needed values, calculated from the description: Mass coeff Ext Area Int Area Gyration radius 100 4.909e-2 7.854e-3 0 Set cross section type to Beam and choose No hysteresis Set stiffness types to Constant and set: Axial stiffness Bending stiffness Shear stiffness Torsion stiffness 1e9 1e4 0 1e5 Set Hydrodynamic force coefficients, Input code to Dimensional coefficients. Set: Qy My 100 50 The rest of the coefficients are zero Set capacity parameters: Tension capacity Max curvature 1e9 0.4 Copy Riser CRS by right click on it an chose copy (or press ctr+c) then right click and chose paste (or press ctr+v) Rename the new crs elemnent by clicking F2, and enter name BuoyancyCRS Change the following variables of the BuoyancyCRS Set Ext. Area to 0.3 Qx Qy Mx My 250 200 200 200 3. Create supernodes Right click on folder Slender system and create New > Supernode Set name BottomConnection Set supernode BottomConnection properties Constraint: Fixed or prescribed Initial Positions. The initial position always has to be set such that a line is unstretched. One only has to set either global or local position, the other will be calculated: Xg Yg Zg 0 0 –50 Static global position: Xg Yg Zg 0 0 –100 Rotation = –90 Choose boundary connection: Fix all Right click on folder Supernodes and create New > Supernode Set name RiserBase Set supernode RiserBase properties: Constraint: Fixed or prescribed Initial Positions. The initial position has to be set such that a line is unstretched: Xg Yg Zg 160 0 –50 Fixed or Prescribed Configuration: Chose Support Vessel: VESSEL Static global position: Xg Yg Zg 60 0 10 Rotation = –90 Choose boundary connection: Fix all 4. Create internal fluid Right click on folder Slender system and create New > Internal Fluid Type: Set name fluid_40 Set: Density Flow Inlet 1000 End 1 5. Create a line type and a line Right click on folder Slender system and create New > Line Type: Use default name lineType Set Line Type Properties Create new segment by clicking the green plus under the segment line. Do this 3 times to create 3 segments Set the lengths: The Stressfree length should be the same as the length of the segment. segment 1 segment 2 segment 3 10 50 100 Set the number of elements: segment 1 segment 2 segment 3 5 20 40 Set the first and last segments Cross section to RiserCRS. The middle segment has cross section: BuoyancyCRS Set Internal fluid to fluid_40 Right click on folder Slender system and create New > Line: Set name: Riser Set properties: Line Type End 1 End 2 LineType BottomConnection RiserBase 6. Create an environment Right click on model and create New > Environment Set Wave to Numerical Wave: Press on the upper green plus to add a direction. Set the direction to 0. Press on the lower green plus to add 4 frequencies. Set the frequencies to: 1 2 3 4 frequencies 0.5219 0.522 0.524 0.5241 Add the following spectral values to the last table. This can also be done by copying this table, right click where you want them and chose Import > From clipboard 0 3.259e+04 3.259e+04 0 Set Current to Current From the table below copy the white part to the clipboard. In the current editor, press the arrow beside the green plus, and chose Create from clipboard. The table is then imported. No Level Direction Velocity 1 0 0 1 2 –90 0 0.9 3 –100 0 0 7. Set static calculation properties Set properties of Static Calculation under Calculation Parameters: Click on the green plus to add Current forces Set N Step for the Specified Displacements to 200, Set max iterations to 20 for volume forces, specified displacements and current forces 8. Set dynamic calculation properties Set properties of Dynamic Calculation: Under Irreg. analysis set time series length to 4096. This combined with the numerical wave settings, leads to a wave with a waveheight of 12.012 m and period of 10 s. Set simulation length to 72 s with a time step of 3.125e-02 s Set Node step = 1 Under storage choose Displacement, Force responce, curvature responce and visualization responce. Set storage step = 8, and file format = Binary. This leads to file output every 0.25 s. Do this for both Displacement responce storage, force responce storage and curvature responce storage. Set nodes where you are interested in the results e.g, if you are interested in the buoyancy part: Line Line Type Segment Element Number All Elements Riser LineType 2 1 yes 9. Run the simulation Run the simulation Either double clicking the Initial condition Initial (under the Conditions folder) and click the Run Dynamic button in the editor,or by right clicking Inital (under the Conditions folder) and choose Run dynamic analysis If you have not opened the graphics view then open it by right clicking RotatingBodies and choose Open 3D View : In the graphics view there are two drop down menus. The first drop down contains the conditions in the task and will now only show Initial. The second shows the Modeled state, the Static and the Dynamic results. Choose the Dynamic simulation (select Dynamic in the second drop down) and click on the play button (the black arrow adjacent to the drop down menus). You can speed up the simulation result (the animation in the 3D view) by opening the view menu (the small white arrow in the top right corner) and choose Scale playback speed and set it to 10.