Data Loading...
P03_Workshop_01_FENSAP-ICE_GUI Flipbook PDF
P03_Workshop_01_FENSAP-ICE_GUI
771 Views
294 Downloads
FLIP PDF 1.08MB
Welcome and Introduction to FENSAP-ICE GUI
ANSYS, Inc. Southpointe 2600 ANSYS Drive Canonsburg, PA 15317 [email protected] http://www.ansys.com (T) 724-746-3304 (F) 724-514-9494
Release 18.1 April 2017 ANSYS, Inc. and ANSYS Europe, Ltd. are UL registered ISO 9001: 2008 companies.
Welcome and Introduction to FENSAP-ICE GUI
Copyright and Trademark Information © 2017 ANSYS, Inc. Unauthorized use, distribution or duplication is prohibited. ANSYS, ANSYS Workbench, AUTODYN, CFX, FLUENT and any and all ANSYS, Inc. brand, product, service and feature names, logos and slogans are registered trademarks or trademarks of ANSYS, Inc. or its subsidiaries located in the United States or other countries. ICEM CFD is a trademark used by ANSYS, Inc. under license. CFX is a trademark of Sony Corporation in Japan. All other brand, product, service and feature names or trademarks are the property of their respective owners. FLEXlm and FLEXnet are trademarks of Flexera Software LLC.
Disclaimer Notice THIS ANSYS SOFTWARE PRODUCT AND PROGRAM DOCUMENTATION INCLUDE TRADE SECRETS AND ARE CONFIDENTIAL AND PROPRIETARY PRODUCTS OF ANSYS, INC., ITS SUBSIDIARIES, OR LICENSORS. The software products and documentation are furnished by ANSYS, Inc., its subsidiaries, or affiliates under a software license agreement that contains provisions concerning non-disclosure, copying, length and nature of use, compliance with exporting laws, warranties, disclaimers, limitations of liability, and remedies, and other provisions. The software products and documentation may be used, disclosed, transferred, or copied only in accordance with the terms and conditions of that software license agreement. ANSYS, Inc. and ANSYS Europe, Ltd. are UL registered ISO 9001: 2008 companies.
U.S. Government Rights For U.S. Government users, except as specifically granted by the ANSYS, Inc. software license agreement, the use, duplication, or disclosure by the United States Government is subject to restrictions stated in the ANSYS, Inc. software license agreement and FAR 12.212 (for non-DOD licenses).
Third-Party Software See the legal information in the product help files for the complete Legal Notice for ANSYS proprietary software and third-party software. If you are unable to access the Legal Notice, contact ANSYS, Inc. Published in the U.S.A.
Welcome and Introduction to FENSAP-ICE GUI
Welcome and Introduction to FENSAP-ICE GUI The objective of this tutorial is to get familiar with the graphical environment of FENSAP-ICE. Launch FENSAP-ICE either by typing fensapiceGUI in a terminal (LINUX, UNIX) or by selecting FENSAPICE in your application directory (WINDOWS).
Project Management Window At start FENSAP-ICE lists all recent projects with icons. This is the project management window. Create a new project directory by clicking on the icon:
Enter Tutorial_01 under Project name, and browse to position this directory in your account. Select any location at the exception of the directory ../workshop_input_files/Input_Grid/ that contains all input files for the tutorials, and the directory ../completed_workshop_files/ that contains all solution files for post-processing. You will then be asked to assign a unit system to this new project. Select the default (metric) unit system by clicking on OK.
Run Management Window When a new project is created you are automatically transferred to its run management window that lists all calculations associated to this project.
Create a New Run Create a new run, or calculation, by clicking on the icon:
Select FENSAP as the flow solver and name the run FLOW. Click OK. Each run contains three different sets of icons, here shown in grey since they have not yet been assigned: • The icons listed on the left side of the config icon contain the input files, in this case a grid file. • The configuration icon allows entering the input parameters and monitoring the calculation. • The icons placed on the right side of the config icon are all output files from this calculation (solution, ice shape, displaced grid, etc.).
Release 18.1 © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
1
Welcome and Introduction to FENSAP-ICE GUI
Assign a Grid File Assign a grid file by right-mouse clicking on the grid icon and by selecting Define. Browse to the file ../workshop_input_files/Input_Grid/Naca0012/naca0012.grid. The grid icon is now shown in white since a file is assigned to it.
Note The config icon is now colored in blue since all input files are assigned properly, allowing you to set the input parameters of FENSAP and to run this calculation. Click the grid icon. On the right side of the interface, under Properties, click Read... to display some grid-related information such as the total number of nodes (65,424), of elements (32,364) and all boundary conditions. The boundary condition tags in FENSAP-ICE are defined as follows: • 10 to 19 and 1,000 to 1,999 for inlets (internal flow) or far-fields (external flow); • 20 to 29 and 2,000 to 2,999 for walls; • 30 to 39 and 3,000 to 3,999 for outlets (not required with a far-field inlet BC); • 40 and 4,000 for general symmetry planes; • 41 and 4,100 for X-symmetry planes; • 42 and 4,200 for Y-symmetry planes; • 43 and 4,300 for Z-symmetry planes; • 60 to 69 and 6,000 to 6,999 for actuator disks.
Drag & Drop Create a new DROP3D run and name it DROPLET. You do not need to re-enter all input parameters when you create a new run. Simply drag & drop the config icon of FLOW onto the config icon of DROPLET. All input parameters that are common to both FENSAP and DROP3D are automatically copied and, both grid and flow solution files are transferred from one directory to the other.
Note • You still need to edit the input parameters of DROP3D since only the parameters that are common to both software were copied during the drag & drop. • The input flow solution file required by DROP3D is shown in grey since there is no flow solution in the FLOW directory. This icon will be colored in white once the associated file is created, allowing you to run DROP3D.
Create a new ICE3D run and name it ICE.
2
Release 18.1 © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Welcome and Introduction to FENSAP-ICE GUI
Drag & drop the input parameters of DROPLET onto ICE. All input parameters common to both software are then copied and, the grid, flow and droplet solution files are transferred from one directory to the other.
Note • You still need to edit the input parameters of ICE3D since only the parameters that are common to both software were copied during the drag & drop. • The input flow and droplet solution files required by ICE3D are shown in grey since there are no flow and droplet solutions in, respectively, the FLOW and DROPLET directories. Each icon will be colored in white once the associated file is created, allowing you to run ICE3D.
List of Runs You can change the order in which the runs are listed by left-mouse clicking on one run and by moving it upward or downward with your mouse. You can also change the listing by clicking on:
to get a hierarchical view, for example, all runs listed with their associated directory and files. Click again to change to a chronological view (listed by calculation dates). Click again to return to the original view. Go back to the project management window by clicking on:
Import from FLUENT or CFX Create a new project NACA0012_FLUENT and select the default (metric) unit system. Create a new DROP3D run. You can assign a grid file by right-mouse clicking on the grid icon and by selecting Define. This option imports Fluent, CFX or CGNS grid & solution files. Select the file ../workshop_input_files/Input_Grid/Naca0012/naca0012_clean.cas and begin your import.
Note The *.DAT file must be located in the same directory as the *.CAS file and share the same file name.
Release 18.1 © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
3
Welcome and Introduction to FENSAP-ICE GUI
The converter allows you to modify the boundary condition tags between Fluent and FENSAP-ICE. For now, keep the boundary conditions as automatically detected by FENSAP-ICE. Both grid and flow solution will then be imported into the run directory.
Note The grid file provided to FENSAP-ICE should always be in meters.
Project Management Go back to the project management windows. Additional project information can be displayed on the right side, under Info, by clicking on the project icon, the project creation and modification dates, as well as comments under Notes. Enter some (positive!) comments about Tutorial_01.
List of Projects Click the following icon to change the project listing:
All projects are now listed in a tree structure. You can regroup projects by assigning them to a category. To do this, right-mouse click Tutorial_01 and select Set category. Click Add and enter the category Tutorials.
Import a Project Import an existing project with File → Open project. Select the directory GLC305 provided under ../workshop_input_files/Input_Grid/ You have now been transferred to the associated run management window that contains one FENSAP, one DROP3D and one ICE3D calculation.
Run Management Archival Right-mouse click FENSAP and select Archive run. This option allows you to save this calculation in an archive file that can be retrieved later on. Name your archived run Archive_FENSAP_GLC305. All output icons are now shown in grey, and you can repeat the calculation without overwriting the previous flow solution. Note that all input files of DROP3D and ICE3D, linked to the output files of FENSAP, are now shown in grey. Double-click the archive icon to see the archive data and to manage them easily. Select To current to replace the solution with the selected archive data. The solution icons are now shown in white.
4
Release 18.1 © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Welcome and Introduction to FENSAP-ICE GUI
Global Settings Go to Settings → Units to change the unit system of all runs listed under this project. You can choose between the Metric and Imperial systems, or change the unit of one specific variable, for example temperature from Kelvin to Celsius. For now click Cancel. Go to Settings → Preferences. Under Postprocessing, FENSAP-ICE supports different post-processing packages, such as FIELDVIEW, EnSight, Tecplot, etc. Select Viewmerical, ANSYS' own post-processing package, for these tutorials.
Basic Post-processing FENSAP Solution Right-mouse click the flow solution file of FENSAP, soln, and select View with Viewmerical. A new window opens with basic post-processing tools to display the grid and flow solution. Remove (uncheck) BC_1000 (far-field), BC_2000, BC_2001, BC_2002 and BC_2003 (walls). Leave only BC_4300 (Z-symmetry plane). Use the left mouse button to rotate the view, the middle mouse button to pan it, and the right mouse button to zoom on it. You can also use control + left-mouse click to draw a zoom box. Right-mouse click the axis marker and select Top (Z) view. Select data-soln in the Objects panel.
Note The grid name is displayed on the left (bottom left) of the status bar. Select Wireframe under Object to show the grid on the symmetry plane. You may need to draw different bounding boxes to zoom in progressively on the wing. Select Colored under Objects to show the density field. Change, under Data, the flow variable to Mach number to see the boundary layer and wake. In the Objects panel, choose the Z-coordinate cutting and set the max value to 1.5. To display the Mach number at different wing cross-sections, scroll the bar beneath the min and the max values. Deactivate the cutting plane option when this is done by selecting None under cutting plane. To show pressure coefficient on the wing: • Under Objects, remove BC_4300 and activate BC_2000 to BC_2003 (walls); • Under Data, change the flow variable to Pressure Coefficient; • Under Query, activate the 2D Plot option; • Select a cutting plane along the Z-axis, and change the X-axis of the plot, located at the bottom left of the plot, to the X-coordinate of the grid. • Scroll the bar located beside the Cutting plane to see the pressure coefficient at different wing sections.
Release 18.1 © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
5
Welcome and Introduction to FENSAP-ICE GUI
Close this window to return to the run management window.
DROP3D Solution Right-mouse click the droplet solution file of DROP3D, droplet, and select View with Viewmerical. Display the LWC on the symmetry plane by only keeping the BC_4300 checked. A shadow zone can be observed behind the wing (dark blue region). Select BC_2000 to BC_2003 (remove all other boundaries). Right-mouse click the axis and select Fit to view. Select Colored under Object. Change under Data, the default variable, Droplet LWC (kg/m3), to Collection efficiency-Droplet to see the non-dimensional mass of water that impacts the wing, as well as the impingement limits. You may need to rotate the wing. To show the collection efficiency on the wing: • Under Query, activate the 2D Plot option; • Select a cutting plane along the Z-axis, and change the X-axis of the plot to the Y-coordinates of the grid. • Scroll the bar located beside the Cutting plane to see the collection efficiency at different wing sections. Close this window to return to the run management window.
ICE3D Solution Right-mouse click the ice solution file of ICE3D, swimsol, and select View ICE, a special version of Viewmerical that displays only the ice shapes. Take a first look at the ice shape. Under Data → ICE3D, change the display mode from Ice cover to Ice cover - Shaded. ICE3D outputs a 3D CAD of the ice shape, either for manufacturing purpose or for assessing handling qualities. To display the CAD, change the display mode to CAD output. The CAD can then be simplified to remove any ice below a given height or to smooth sharp edges and saved as a point cloud or STL file. Close this window to return to the run management window.
Input Parameters and Convergence FENSAP Input Parameters Double-click the config icon of FENSAP to open its main driver. This window is divided into two sections: left for the graphical display (similar to Viewmerical); right for all input parameters listed per category. To activate the graphical display, click on the bottom left grey cube and select Full view. Take a quick look at the different input parameters of FENSAP by shifting from one category (panel) to the other. We would like to emphasize three important input parameters for glaze icing: • Under Model you will find Surface Roughness. FENSAP allows imposing an equivalent sand-grain surface roughness on a wall to model its impact on turbulence. Roughness is a crucial aspect of glaze icing, as it
6
Release 18.1 © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Welcome and Introduction to FENSAP-ICE GUI
modifies the heat flux distribution. Here roughness is set uniformly to 0.5 mm (not 0.5 m!). Different correlations can also be selected, but remember that they may not be suitable for all applications. • Go to Boundaries and click Wing - LE. The procedure for computing ice accretion with FENSAP-ICE requires imposing a constant temperature on all walls (T_ref + 10 K is recommended) that is greater than the reference air temperature (here 266.48 K). The flow solution then outputs a heat flux distribution; imposing a higher temperature ensures a good sign of the heat fluxes computed by FENSAP. ICE3D will then read this heat flux distribution and compute heat transfer coefficients from the reference air temperature.
Note You cannot solve an adiabatic flow and expect to get an ice shape. Convective heat transfer is required for icing and, therefore, the full energy partial differential equation must be solved. To do this, the energy equation should be set to Full PDE under the Model panel.
Close this window and do not save the input parameters.
Convergence of FENSAP Right-mouse click the FENSAP run and select View previous log/graph. This option allows you to look at the convergence of the calculation, shown under Graphs: • Averaged residual of the governing equations (mass, momentum and energy combined). This is the L2-norm of the residual vector of the linear matrix system. You should try to converge to machine accuracy, or a very low value, for most applications. Such convergence implies that the primitive variables (for example, density, pressure, velocity and temperature) are not varying anymore. • True residual of each governing equation (mass and momentum, energy, turbulence). • Integrated quantities, such as the lift and drag coefficients, and the total heat computed using the gradient of temperature, referred to as Classical in FENSAP-ICE, or using a Gresho formulation. Total mass and enthalpy inflow, outflow and deficit are also monitored. The integrated values are computed each time a solution file is written. • Convergence of the GMRES linear matrix solver for each governing equation. If the true residual is not converging, first check the convergence of the linear matrix solver. If it is not converging enough per iteration, reduce the CFL number to increase the diagonal-dominance of the matrix. Click in the convergence graphic to display local values. Shift + left-mouse click and draw a box to zoom on a section of the convergence curve. Middle mouse click to return to the previous view setting. Close this window.
DROP3D Input Parameters Double-click the config icon of DROP3D. Take a first look at all the different input parameters by shifting from one category to the other. We will describe them in the next tutorials. Close this window and do not save the input parameters.
Release 18.1 © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
7
Welcome and Introduction to FENSAP-ICE GUI
Convergence of DROP3D Right-mouse click the DROP3D run and select View previous log/graph. This option allows you to look at the convergence of past calculations, shown under Graphs: • Averaged residual or Droplets – Residual - Average of the governing equations (mass and momentum combined). This is the L2-norm of the residual vector of the linear matrix system. You should try to converge to machine accuracy, or a very low value, for most applications. Such convergence implies that the primitive variables (for example, LWC, velocity) are not varying anymore. • The total collection efficiency on all surfaces or Droplets - Total Beta should converge to a constant value. • Change in total collection efficiency. The total collection efficiency will generally converge quite fast to a constant value.
Note LWC may not yet be fully converged since the shadow zone behind the body may still be developing.
• True residual of each governing equation (mass and momentum or Droplets – Residual LWC and Residual - Momentum). • Convergence of the GMRES linear matrix solver for each governing equation. If the true residual is not converging, first check the convergence of the linear matrix solver. If it is not converging enough per iteration, simply reduce the CFL number to increase the diagonal-dominance of the matrix. Close this window.
ICE3D Input Parameters Double-click the config icon of ICE3D. Take a first look at all the different input parameters by shifting from one category to the other. We will describe them in the next tutorials. Close this window and do not save the input parameters.
8
Release 18.1 © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.