aqwa教程 (11)

WS5.1-1 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Introduction to ANSYS AQWA Customer Training Material Workshop 5.1 Load Mapping Workshop 5.1 – Load Mapping WS5.1-2 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training MaterialWorked Example • We are going to create a simple box shaped model to demonstrate the load mapping process • The structural model will include some simple stiffeners to show how to handle internal elements • The Steps of the exercise include: – Create Structural Geometry – Create Structural Model and Information – Create Hydrodynamic Geometry – Create Hydrodynamic Model and Information – Include the Hydrodynamic loading to Structural model (load mapping) – Investigate the final results Workshop 5.1 – Load Mapping WS5.1-3 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training MaterialStep 1: Create the Structural Geometry • Open Workbench • Create a Geometry instance and open DM for editing Workshop 5.1 – Load Mapping WS5.1-4 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural geometry • Create Hull – Select length units as meters – Create box primitive – Set details of box – Generate Workshop 5.1 – Load Mapping WS5.1-5 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural geometry • Create a thin surface – Set Selection Type to Bodies Only – Graphically select box for Geometry – Set thickness to 0m (acts as shell rather than solid) – Generate Workshop 5.1 – Load Mapping WS5.1-6 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural geometry • Create Stiffener – We are going to generate a series of simple plate stiffeners – First generate a new horizontal plane Workshop 5.1 – Load Mapping WS5.1-7 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural geometry • Create stiffener – Use the new plane to slice the model – First Freeze the model to allow the slice – Slice all bodies using the plane created in the last step Workshop 5.1 – Load Mapping WS5.1-8 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural geometry • Create stiffener – Create a second box that will be used to remove the interior of the plate to generate the desired stiffener. Note that we Add Frozen so that it does not combine with the stiffener. Workshop 5.1 – Load Mapping WS5.1-9 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural geometry • Create stiffener – Create the plate surface for the stiffener using the edges generated with the Slice command – Edges are selected using the Workshop 5.1 – Load Mapping WS5.1-10 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural geometry • Create stiffener – Remove interior of plate to create desired stiffener • Use a Boolean operation (Subtract) • Target body is the plate generated in last step – To select the plate use the layer selection image to step through the surfaces • Tool body is the second box Workshop 5.1 – Load Mapping WS5.1-11 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural geometry • Generate copies of stiffener – Use Pattern to create 5 copies of stiffener • Linear pattern type with 5m offset • Geometry is the stiffener created in the last step • Use the face normal of the stiffener surface to define direction. You will need to click on Selection Filter: Model Faces to be able to select the stiffener plate. • Note the use of the red and black arrows to define actual direction. Workshop 5.1 – Load Mapping WS5.1-12 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural geometry • Resulting stiffener definition Workshop 5.1 – Load Mapping WS5.1-13 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural geometry • Complete stiffener connection – Stiffeners are not automatically connected to hull – Use Joint command to make connections – Select all surface bodies as Target Bodies. Can use Box Select mode to simplify selection. Workshop 5.1 – Load Mapping WS5.1-14 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural geometry • Create a single part – Model currently has 8 bodies and 8 parts – To improve meshing create a single part – Rename the new Part to Vessel, and name the stiffener and hull bodies appropriately. – l Workshop 5.1 – Load Mapping WS5.1-15 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural geometry • Geometry for structure is now complete • Exit DesignModeler • Now we need to create a structural meshed model for use in the load mapping stage Workshop 5.1 – Load Mapping WS5.1-16 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training MaterialStep 2: Create Structural Model and Information • Add Static Structural System to project, linking geometry to that created in DesignModeler. • Double click on Model cell. Workshop 5.1 – Load Mapping WS5.1-17 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural Model and Information • Define plate thickness – DesignModeler set plate thickness to 0.0 • Results in Geometry as ? • Set thickness for hull bodies to 32mm • Set thickness for stiffener plate to 50mm Workshop 5.1 – Load Mapping WS5.1-18 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural Model and Information • Mesh – Use default meshing for this model Workshop 5.1 – Load Mapping WS5.1-19 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural Model and Information • Define wetted surface – Load transfer requires definition of wetted (external) surfaces – Use dummy pressure case to define required geometry. This should be a small value since it will be included in the solution. Note that if static hydrostatic loading is required then choose Hydrostatic Pressure and provide real data – Select surfaces manually, or use named selections Workshop 5.1 – Load Mapping WS5.1-20 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural Model and Information • Add Point Masses – Masses represent ballast & storage – Associate mass with hull surface adjacent to position – First mass is at 5,5,-32.5 – Mass value of 1000 tonnes Workshop 5.1 – Load Mapping WS5.1-21 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural Model and Information • Add Point Masses – Add two more additional masses • 1000 tonnes at 5,5,-27.5 • 1000 tonnes at 5,5,-22.5 – Associate these masses to appropriate hull surfaces Workshop 5.1 – Load Mapping WS5.1-22 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural Model and Information • Ensure weak springs are enabled – ANSYS Mechanical defaults to Program Controlled for including weak springs to remove rigid body motions Workshop 5.1 – Load Mapping WS5.1-23 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural Model and Information • Solve – The subsequent hydrodynamic model requires an accurate definition of the mass inertia information for the model. – In the absence of better data this can be extracted from the structural model – In order to obtain this a Solve must be instigated. – Can ignore any warnings and errors related to solution since results from this analysis are not used, we are only interested in the mass information Workshop 5.1 – Load Mapping WS5.1-24 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Structural Model and Information • Mass Extraction – The hydrodynamic model requires an accurate definition of the mass inertia information for the model. – In the absence of better data this can be extracted from the structural model • Select Solution Information and review Worksheet for the mass data Workshop 5.1 – Load Mapping WS5.1-25 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training MaterialStep 3: Create Hydrodynamic Geometry • Structural definition model load mapping is now complete • Exit ANSYS Mechanical • Now we need to create a hydrodynamic model for use in the load mapping stage Workshop 5.1 – Load Mapping WS5.1-26 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Hydrodynamic Geometry • Duplicate structural geometry created earlier. Rename system as Hydrodynamic Geometry and double click in the geometry cell of the new system Workshop 5.1 – Load Mapping WS5.1-27 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Hydrodynamic Geometry • The hydrodynamic geometry is much simpler, it is just the hull • Suppress items in the tree that were used for the stiffener generation Workshop 5.1 – Load Mapping WS5.1-28 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Hydrodynamic Geometry • Modify Geometry – AQWA requires model that is meshed up to water line • Slice the model horizontally • Use XYPlane as the Base Plane (global Z is 0 for this) – AQWA also requires one part for each vessel • Form new part and name as Hull – Close DesignModeler Workshop 5.1 – Load Mapping WS5.1-29 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training MaterialStep 4: Create Hydrodynamic Model and Information • Add a Hydrodynamic Diffraction to the Hydrodynamic Geometry • Double click on Model Workshop 5.1 – Load Mapping WS5.1-30 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Hydrodynamic Model and Information • Add Point Mass – Add a point mass and manually define the mass and inertia values obtained from structural model – Ensure position of point mass is correctly defined (also obtained from structural model) Workshop 5.1 – Load Mapping WS5.1-31 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Hydrodynamic Model and Information • Generate Mesh – In general the load mapping process requires a more refined hydrodynamic mesh than normally required for motions analysis – For this exercise, to reduce run time use maximum element size of 2.5m (and defeaturing tolerance of 1m) Workshop 5.1 – Load Mapping WS5.1-32 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Hydrodynamic Model and Information • Adjust the General Settings for Hydrodynamic Analysis – To reduce run time for the exercise set the number of intermediate frequency values to 8 Workshop 5.1 – Load Mapping WS5.1-33 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Hydrodynamic Model and Information • Check Hydrostatics – Insert Hydrostatic Result to Solution – Solve Hydrostatics to check that we have a valid model Workshop 5.1 – Load Mapping WS5.1-34 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Hydrodynamic Model and Information • Check Hydrostatics – When solution has completed select Hydrostatic Report and review results Workshop 5.1 – Load Mapping WS5.1-35 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Create Hydrodynamic Model and Information • Solve – Select Solve and review pressures using Pressures and Motions results object Workshop 5.1 – Load Mapping WS5.1-36 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training MaterialStep 5: Load Mapping • Hydrodynamic model for AQWA WAVE is now complete • Exit AQWAWB • Now we need to update the structural model to include loading from the hydrodynamic model • Re-open the Static Structural system Workshop 5.1 – Load Mapping WS5.1-37 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Include the Hydrodynamic loading to Structural model • We are going to map four wave cases. In Analysis Settings set the number of steps to 4 • We are going to use command snippets to transfer loads from the AQWA hydrodynamic database – Insert Commands in the object tree of Static Structural – RMB the Commands (APDL) object and select Import... – Click Yes to question about continuing with replacing existing text – Browse to existing file DiffractionSetup.txt Workshop 5.1 – Load Mapping WS5.1-38 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Include the Hydrodynamic loading to Structural model • Provide global data for the diffraction wave load setup – Requires water density and gravitational constant – These are provided as ARG1 and ARG2 respectively in the details panel. – Note that the data must be provided in units consistent with the current selected units. – Set the file directory as highlighted to your current working directory, ending in “_files\dp0\AQW\AQW\AQ \Analysis\Analysis” Workshop 5.1 – Load Mapping WS5.1-39 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Include the Hydrodynamic loading to Structural model • Rename command object in outline tree to DiffractionSetup • Ensure that Step Selection Mode in details panel is set to First (only applied at the first load step) Workshop 5.1 – Load Mapping WS5.1-40 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Include the Hydrodynamic loading to Structural model • Include a second command object. This time import the DiffractionWave.txt – This command snippet requires four arguments • ARG1 is wave direction, in degrees • ARG2 is wave height • ARG3 is wave period in seconds • ARG4 is phase position of the wave in degrees – Apply appropriate data as shown. Assign this information to Step Number 1 (you will need to change the Step Selection Mode to By Number). – Rename the command object to DiffractionWave 1 Workshop 5.1 – Load Mapping WS5.1-41 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training Material...Include the Hydrodynamic loading to Structural model • Repeat the previous steps for the remaining three wave cases – RMB on existing DiffractionWave command object and select Duplicate – Apply appropriate data as below. – If required rename the command object to DiffractionWave 2/3/4 as necessary • The four cases correspond to 0 and 90 degree phase angles for two wave periods of 7.25 seconds and 4.55 seconds. All are for the zero degree wave direction. Workshop 5.1 – Load Mapping WS5.1-42 ANSYS, Inc. Proprietary © 2012 ANSYS, Inc. All rights reserved. Release 14.0 January 2012 Customer Training MaterialStep 7: Investigate the final results • Solve and review results – Add an Equivalent Stress results object to the Solution branch and Evaluate All Results