Wing Flutter Analysis using 2-way FSI
Workshop
W i n g F l u t t e r F SI SI
Problem Overview
Training Manual
This problem consists of a mahogany wing at Mach Mach 0.9. The geometry is based on the AGARD 445.6 wing w ing which has been widely studied in literature. The structural and fluid meshes meshes used are quite quite coarse and are not intended to show best practice. The response of the wing to an initial perturbation is analysed using 2-way FSI between ANSYS CFX and ANSYS Mechanical. ANSYS Workbench version 12.1 will be used for the analysis. Basic knowledge of Workbench, CFX and Mechanical is assumed.
W i n g F l u t t e r F SI SI
Workflow Overview
Training Manual
• Import the geometry into Workbench and complete the structural mesh and model • Perform a Modal analysis to verify the expected mode shapes and frequencies • Import the existing fluid mesh which was completed in ICEM CFD • Setup and solve an initial steady state fluid solution with w ith a fixed wing • Setup and solve the coupled FSI analysis • Post-process
W i n g F l u t t e r F SI
Starting the Project and the Structural Model 1.
Start Workbench 12.1 and save the project as A G A R D 4 4 5 _ W o r k s h o p . w b p j in a new working directory –
2.
Saving the project at start up sets the working directory
Add a Transient Stru ctu ral (A NSYS) analysis to the P r o j e c t Schematic
3.
Right-click on the S o l u t i o n cell (A6) and select Delete –
4.
Training Manual
The solution is performed after completing the fluid setup
Right-click on the G e o m e t r y cell and import the file agard445_wing.agdb –
The geometry has already been completed
W i n g F l u t t e r F SI
Structural Material Properties 1.
Double-click the E n g i n e e r i n g Data cell to define the structural material properties
2.
Enter a new material named Mahogany
3.
Double-click on D e n s i t y under P h y s i c a l P r o p e r t i es from the T o o l b o x on the left, then enter the D e n s i t y value as 381.98 kg m^-3
4.
Under Lin ear Elastic doubleclick on O r t h o t r o p i c El as t i c i t y and enter values for the Young’s Modulus and Poisson’s Ratio as shown
Training Manual
W i n g F l u t t e r F SI
Structural Model 5.
Click R e t u r n t o P r o j e c t from the toolbar
Now create the structural mesh and setup 1.
Double-click the M o d e l cell (A4) to open Mechanical and create the structural mesh and model
2.
Select Uni ts > Metric (m , kg , N, s, V, A ) from the main menu
3.
Expand the G e o m e t r y tree in O u t l i n e . Select w i n g .
4.
In the Details view, under Material , change the A s s i g n m e n t from Structural Steel to M a h o g a n y
Training Manual
W i n g F l u t t e r F SI
Structural Model Next create a coordinate frame aligned with the wing corresponding to the orthotropic material properties 1.
Right-click on C o o r d i n a t e S y s t e m s in the O u t l i n e tree and Insert a new Coord inate System
2.
Right-click to R e n a m e the Coordinate System “ L o c a l O r t h o ”
3.
In the Details view, change D ef i n e B y to G l o b a l C o o r d i n a t es
4.
From the Toolbar select the RY icon to rotate about the y-axis, and enter 45o under T r a n s f o r m a t i o n s in the Details view
Training Manual
W i n g F l u t t e r F SI
Structural Model 5.
Now select w i n g again under G e o m e t r y and change the C o o r d i n a t e S y s t e m to Lo cal Ortho
The next step is to create the structural mesh 1.
Right-click on Mesh and select Generate M e s h to create the default mesh –
2.
The default mesh is too coarse, particularly near the leading edge
Select Mesh from the O u t l i n e tree, then in the Details view, under Sizing , set Use A d v a n c e d S i ze F u n c t i o n s to O n : C u r v a t u r e then re-generate the mesh –
This improves resolution at the highly-curved leading edge, but produces too many elements in the swept direction and the elements are too large away from the leading edge.
Training Manual
W i n g F l u t t e r F SI
Structural Model 3.
Right-click on M e s h and select Ins ert > Method
4.
Select the wing from the viewer and click A p p l y in the G e o m e t r y field
5.
Set the M e t h o d to Sweep , and the S w e e p N u m D i v s to 20, then re-generate the mesh –
6.
This gives a more reasonable number of elements in the swept direction, but the elements are still too large away from the leading edge
Select Mesh from the O u t l i n e tree, then in the Details view, under Sizing , set Min Size to 1e-3 m and Max Fac e Size and Max Tet Size to 0.02 m. Generate the mesh. –
This completes the structural mesh
Training Manual
W i n g F l u t t e r F SI
Structural Model The structural boundary conditions and analysis settings can now be defined 1. Under Transient (A 5) select A n a l y s i s S e t t i n g s and set the values as shown –
The transient timestep controls are defined in CFX-Pre. Here we just need to define how many substeps are needed per timestep (almost always 1). The Step End Time is not used. Auto Time Stepping should be off. Time Integration should be on for a true transient. Large Deflection should always be on, even for small deformations.
2. From the toolbar select Inert ial > S t an d a r d E ar t h G r a v i t y then in the Details view set the D i r e c t i o n to –Y Direction
Training Manual
W i n g F l u t t e r F SI
Structural Setup 3.
Insert a Fixed Support at the root surface of the wing
4.
From the Toolbar select L o a d s > Fl u i d Solid Interface and apply to the top AND tip surface of the wing
5.
Create a second Fluid Solid Interface for the bottom surface of the wing
Training Manual
– The Interface Number is shown in the Details view for each Fluid Solid Interface. This number is referenced when applying boundary conditions to the fluid side – In general the interfaces could be combined into a single Fluid Solid Interface. However, when surfaces meet at a sharp angle, as is the case here at the trailing edge, it is a good idea to use separate interfaces to avoid any fluid-solid mesh mapping problems
W i n g F l u t t e r F SI
Modal Analysis
Training Manual
This completes the structural setup. At this point you could write out an input file (Tools > Write Input File) if the case is to be ran on a different machine (e.g. a cluster). Before proceeding with the fluid setup it is a good idea to perform a Modal analysis to verify the modal frequencies are as expected. 1.
Return to the main project page (do not close Mechanical)
2.
Drag and drop a Mod al (ANSYS) system onto the M o d e l cell (A4) of the T r an s i e n t S t r u c t u r a l analysis •
This creates a new Modal analysis, sharing the Geometry and Model from the Transient Structural system
W i n g F l u t t e r F SI
Modal Analysis 3.
Return to the Mechanical window –
A Modal (B5) entry has been added to the Outline tree
4.
Right-click on the F i x e d S u p p o r t under the Transient (A 5) entry and select C o p y
5.
Right-click on the Mo dal (B 5) entry to Paste the Fixed Support into the Modal analysis
6.
Select the Modal A n a ly s i s S et t i n g s and reduce the M a x M o d e s t o F i n d to 4
7.
Right-click on S o l u t i o n (B 6 ) and select Ins ert > Deform ation > Total
8.
Right-click on Mod al (B 5) and select S o l v e –
The first four mode frequencies are shown
Training Manual
W i n g F l u t t e r F SI
Modal Analysis 9.
Training Manual
Select T o t a l D ef o r m a t i o n under Solu tion (B6) from the O u t l i n e tree, then click the A n i m a t i o n Play icon. Stop the animation after viewing.
10. To view the next mode shape, select T o t a l D ef o r m a t io n again, then in the Details view change the M o d e to 2. Right-click on T o t a l D ef o r m a t i o n and select
First Bend ing Mo de at 9.64 Hz
Retrieve This Resu lt.
11. Save the project 12. Close the Mechanical window after viewing the results and return to the main Workbench project page
First Torsional Mo de at 40 Hz
W i n g F l u t t e r F SI
Steady State Fluid Analysis Next you will solve a steady-state fluid solution to provide the starting point for the transient FSI analysis. 1. Add a Fluid Flow (CFX) Analysis System to the P r o j ec t S c h e m a t i c (do not connect it to any other systems) 2. Right-click on the M e s h cell (C3) and select Im p o r t M e s h F i l e 3. Change the File of ty pe: option to ICEM CFD Out pu t File(*.cf x5) then select the file a g a r d _ w i n g 3 . c f x 5 provided with this workshop
Training Manual
W i n g F l u t t e r F SI
Steady State Fluid Analysis 4.
Double-click the Setup cell (C3) to start CFXPre
5.
When CFX-Pre opens, edit the Default D o m a i n and set the following on the B a s i c S e t t i n g s panel: •
Material = A ir Ideal Gas
•
Referenc e Pressu re = 7703 [Pa] (make
sure the units are correct) •
B u o y a n c y O p t io n = B u o y a n t
•
G r av i t y X D i r ec t i o n = 0
•
G r av i t y Y D i r ec t i o n = -g (click the
Expression icon to enter) •
G r av i t y Z D i r e c t i o n = 0
•
B u o y a n c y R e f er e n c e D e n s i t y =
0.0994 [kg m^-3]
Training Manual
W i n g F l u t t e r F SI
Steady State Fluid Analysis 6.
On the Fluid Models panel set: •
Heat Transfer Optio n = Total Energy
•
T u r b u l e n c e O p t i o n = S h e ar S t r e s s Transport
7.
Click OK to complete the domain settings
8.
Insert a boundary condition named Inlet and set the following, then click OK : •
B o u n d a r y T y p e = In l e t
•
L o c a t i o n = O P EN
•
M as s A n d M o m e n t u m O p t i o n = C ar t . V el . C o m p o n e n t s
•
•
U = 269.69 [m s^ -1]
•
V = 0.26969 [m s^ -1]
•
W = 0 [m s ^ -1 ]
Static Tem peratu re = 269.86 [K]
Training Manual
W i n g F l u t t e r F SI
Steady State Fluid Analysis The inlet boundary has a slight V velocity component. This will be removed in the transient analysis providing a perturbation to the flow and the wing. 9.
Insert a boundary condition named Outlet and set the following, then click OK : •
Bo un dary Type = Outlet
•
L o c a t i o n = O U TL E T
•
M as s A n d M o m e n t u m O p t i o n = A v e r ag e S t at i c P r e s s u r e
•
Relative Press ure = 0 [ Pa]
10. Insert a boundary condition named Sy m and set the following, then click OK : •
B o u n d a r y T y p e = S y m m e tr y
•
L o c a t i o n = SY M
Training Manual
W i n g F l u t t e r F SI
Steady State Fluid Analysis
Training Manual
11. Insert a boundary condition named W i n g B t m using the following: •
Bo un dary Type = Wall
•
L o c a t i o n = W IN G B T M
•
All other settings can remain at their default values
12. Insert a boundary condition named W i n g T o p A n d T i p using the following: •
Bo un dary Type = Wall
•
Lo cati on = WINGTOP, WINGTIP
W i n g F l u t t e r F SI
Steady State Fluid Analysis
Training Manual
Next, modify the Solver Controls: 1.
Edit the S o l v e r C o n t r o l object from the O u t l i n e tree and set: •
Max. Iterations to 50
•
2.
Typically you shouldn’t limit the max. iterations too much since a case may stop before it is converged. In this instance it is known that the solution is well converged after 50 iterations.
•
T i m e s c a l e C o n t r o l = P h y s i c a l Ti m e s c a l e
•
Phy sic al Timesc ale = 0.01 [s]
•
Resid ual Target = 1e-6
Click OK
Now create some Monitor Points: 1.
Edit the Output Control object from the O u t l i n e tree. On the M o n i t o r tab enable M o n i t o r O p t i o n s
W i n g F l u t t e r F SI
Steady State Fluid Analysis 2.
3.
4.
Create a new Monitor Point named Drag and set: •
O p t i o n = E x p r e s s i o n
•
Expressio n Value = f o r c e _x ()@ W in g B t m + force_x()@WingTopAndTip
Create a second Monitor Point named L i f t and set: •
O p t i o n = E x p r e s s i o n
•
Expressio n Value = f o r c e _y ()@ W in g B t m + force_y()@WingTopAndTip
Save the case then close CFX-Pre
Training Manual
W i n g F l u t t e r F SI
Steady State Fluid Analysis
Training Manual
You may wish to skip to steps on this page, since the steady-state solution will take approximately an hour to complete. You can open the project A G A R D 4 4 5 _ S t e a d y S o l u t i o n . w b p j and continue from the next page.
1.
In the Project Schematic double-click the Solution cell (C4)
2.
When the Solver Manager opens, enable the D o u b l e P r ec i s i o n toggle, then click Start Run •
The solution will proceed and stop after 50 iterations
3.
Check the residuals are converged, the imbalances are reasonable and the monitor points are showing steady values
4.
Close the Solver Manager then save the project
If you wish, examine the steady state fluid results; detailed instructions are not provided here. The next step is to create the transient FSI analysis.
W i n g F l u t t e r F SI
Transient FSI Analysis 1.
In the P r o j ec t S c h e m a t i c click on the down-arrow in the corner of the Fluid Flow system and select Duplicate. Enter the name for the new system as Transient FSI .
2.
Drag-and-drop the Setup cell of the T r an s i e n t S t r u c t u r a l system (A5) onto the Setup cell of the Transient FSI system (D3) •
3.
This creates the FSI link
Right-click on the Setup cell of the T r an s i e n t S t r u c t u r a l system (A5) and select U p d a t e •
This writes the Mechanical input file in the background and passes it to the Transient FSI system
Training Manual
W i n g F l u t t e r F SI
Transient FSI Analysis 4.
Drag-and-drop the S o l u t i o n cell of the F l u i d Fl o w system (C4) onto the S o l u t i o n cell of the Transient FSI system (D4) •
5.
This uses the initial fluid solution as the starting point for the transient calculation
Double-click the Setup cell of the Transient FSI system (D3) to edit in CFX-Pre
Training Manual
W i n g F l u t t e r F SI
Transient FSI Analysis 1.
In CFX-Pre edit the A n a l y s i s T y p e , set the following, then click OK : •
Total Time = 0.5 [s]
•
T i m e s t e p s = 0.0025 [s]
•
A n a l y s i s T y p e O p t i o n = Transient
2.
Edit the D e fa u l t D o m a in . On the B a s i c S e t t i n g s tab set the M e s h D ef o r m a t io n O p t i o n to R e g i o n s o f M o t i o n S p e c i f i ed .
3.
Expand the M e s h M o t i o n M o d e l section and set the M e s h S t i f f n e s s O p t i o n to Increase N e ar B o u n d a r i es with a M o d e l E x p o n e n t of 2. •
4.
The default value of 10 is often not suitable, since (1 / Boundary Distance)10 may be beyond the number range that can be represented
Click OK
Training Manual
W i n g F l u t t e r F SI
Transient FSI Analysis The message window will show a number of errors because mesh motion boundary conditions now need to be set. 5.
Edit the Inlet boundary. Set the V velocity component to 0 [m s^-1]
6.
The M es h M o t i o n O p t i o n will be set to Stationary by default. Click OK .
7.
Edit the Outlet boundary. The M es h M o t i o n O p t i o n will be set to Stationary by default. Click OK .
8.
Edit the S y m boundary. Under B o u n d a r y Details set the M es h M o t i o n O p t i o n to . Click OK . Stationary
Training Manual
W i n g F l u t t e r F SI
Transient FSI Analysis 9.
Edit the W i n g T o p A n d T i p boundary. Under B o u n d a r y De t ai l s set the M e s h . M o t i o n O p t i o n to AN SYS MultiField
10. Check that FSIN_1 is selected as the A NSYS Interface
•
Total Force will be sent to ANSYS, Total Mesh Displacement will be received
11. Click OK 12. Repeat the last 3 steps for the W i n g B t m boundary, but use FSIN_2 as the A NSYS Interface
Training Manual
W i n g F l u t t e r F SI
Transient FSI Analysis 13. Now edit the S o l v e r Co n t r o l object 14. Set M i n . Co e f f . L o o p s to 1 and Max. C o e f f . L o o p s to 4 •
These are the CFX iterations per coupling iteration. In general don’t use too many – there’s no point in converging CFX too much if the FSI boundary displacements are going to change in the next coupling iteration
15. Set the Residu al Target to 1e-4 (RM S) 16. Switch to the E q u a t i o n C l a s s S et t i n g s tab
Training Manual
W i n g F l u t t e r F SI
Transient FSI Analysis 17. Select the M e s h D i s p l a c e m e n t equation from the list 18. Enable the M e s h D i s p l a c e m e n t check box, the C o n v e r g en c e C o n t r o l check box and the C o n v e r g en c e C r i t e r i a check box 19. Increase the Max. Coeff. Loops to 10 20. Set the Residual Type to MAX These changes set a tighter convergence target for just the Mesh Displacements equations and allow for up to 10 loops to reach that target. It is a good idea to tightly converge the mesh displacement equations to help prevent mesh folding.
Training Manual
W i n g F l u t t e r F SI
Transient FSI Analysis 21. Switch to the E x t e r n a l C o u p l i n g tab 22. Set the Min. Iterations to 2 •
This is the number of coupling iterations per timestep. A minimum of 2 is required for an implicit solution.
23. Set Solve A NSYS Fields to Befo re CFX Fields
•
For transient cases ANSYS should almost always be solved first
24. Set the Under Relaxn. Fac. to 1 •
Under relaxation slows convergence and is generally not necessary. There are better ways to keep the solution stable if required.
25. Click OK
Training Manual
W i n g F l u t t e r F SI
Transient FSI Analysis
Training Manual
26. Edit the O u t p u t C o n t r o l object 27. On the M o n i t o r tab create a new M o n i t o r P o i n t called T i p L E D i s p l a c e m e n t with the following settings: •
O p t i o n = C a r te s i an C o o r d i n a t es
•
O u t p u t V ar i ab l e s L i s t = T o t al M es h D i s p l a c e m e n t
•
Cartesian Coo rdin ates = 0.8075 [m ], 0 [m ], -0.76 [m]
•
You can also pick points from the Viewer. To pick a point on the wing you would need to hide the external boundaries first.
28. Create another M o n i t o r P o i n t called T i p T E D i s p l a c e m e n t at the point (1.1775 [m], 0 [m], -0.76 [m]) 29. Enable the M o n i t o r Co e f f i c i en t L o o p C o n v e r g e n c e check box at the top of the panel •
This produces monitor point data for each inner CFX iteration and allows you to judge the stability of the interface solution.
W i n g F l u t t e r F SI
Transient FSI Analysis
Training Manual
30. Switch to the Tr n R es u lt s tab 31. Create a new T r an s i e n t R es u l t s object with the following settings: •
Optio n = Selected Variables
•
O u t p u t V a r ia b l es L i s t = T o t a l M e s h D i s p l a c em e n t
•
O u t p u t F r eq u e n c y O p t i o n = Co u p l i n g S t e p In t e r v a l
•
Interv al = 4
•
Note that ANSYS will also write data at this frequency
32. Click OK 33. Select Ins ert > Solver > Exp ert Parameter from the main menu 34. On the D i s c r e t i s a t i o n tab enable m e s h d is p d i ff u s io n s c h em e and set the Value to 3 •
This relates to the numerics of the mesh displacement equation. This setting can help avoid mesh folding at sharp corners. In this case the displacements are small, so it likely makes little difference.
W i n g F l u t t e r F SI
Transient FSI Analysis
Training Manual
35. On the I/O Con trol tab enable i n c l u d e p r ef i n fo r c es and set to t •
This includes the CFX reference pressure in the forces sent to ANSYS. In this case it will make little difference since the wing is a closed surface.
36. Click OK 37. Close CFX-Pre then save the project
W i n g F l u t t e r F SI
Transient FSI Solution The next step is to solve the transient FSI case. It will take some time to solve, so is best run overnight. 1.
Double-click the S o l u t i o n cell (D4) of the Transient FSI system to open the Solver Manager
2.
Enable the D o u b l e P r ec i s i o n toggle
3.
Click Start Run
4.
Wait until the solution finishes
Next you will export plot data for use in an FFT chart in CFD-Post: 1.
On the U s e r Po i n t s graph, right-click and select Monitor Properties…
Training Manual
W i n g F l u t t e r F SI
Transient FSI Solution
Training Manual
2.
On the P l o t L i n e s tab turn off all points expect the T i p L E D i s p monitor point
3.
On the R an g e S et t i n g s tab set the T im e s t ep R an g e M o d e to T h i s R u n O n l y then click OK
4.
Select W o r k s p ac e > W o r k s p a c e P r o p e r t i e s from the main menu
5.
On the G l o b a l P l o t S e tt i n g s tab make sure P l o t C o ef f i c i e n t L o o p data is off and set P l o t D a t a B y to S i m u l a t i o n T i m e . Click OK .
6.
Right-click on the monitor plot and select Export Plot Data… . Save the file o u t p u t . c s v (note the saved location).
W i n g F l u t t e r F SI
Transient FSI Solution
Training Manual
7.
Open the o u t p u t . c s v file in Excel (or any program that can process comma separate ASCII data)
8.
Delete the first column of data, so that T i m e is in column A and D i s p l a c e m e n t in column B, then save the file is csv format (not Excel format). It should look as shown. •
9.
Only Time and Displacement data is required for the FFT chart
Close the Solver Manager, return to the main project page and save the project
W i n g F l u t t e r F SI
Transient FSI Post-processing
Training Manual
1.
Double-click cell D5 to view the results in CFD-Post
2.
Turn on visibility for the D e fa u l t B o u n d a r y in the ANSYS results
3.
Edit this boundary. Set the C o l o u r M o d e to Variable , and the Variable to T o t a l M es h D i s p l a c e m e n t .
4.
Right-click on a blank area of the Viewer and select Deformation > Custom
5.
Enter a value of 20 to scale the deformations, then click OK
6.
Use the T im e s t ep S el ec t o r (in the T o o l s menu) to load the results at different timesteps
W i n g F l u t t e r F SI
Transient FSI Post-processing Now create an FFT chart to extract the flutter frequencies: 1.
Select Ins et > Chart from the main menu
2.
Set the T y p e to XY – T r an s i en t o r Sequence
3.
Enable the F as t F o u r i e r T r an s f o r m check box and then the S u b t r a c t m e a n check-box
4.
On the Data Series tab, set the Data Sou rce to File and browse for the o u t p u t . c s v file
Training Manual
