Modal analysis of a submerged gate

Transcription

1 CDIF UPC ENSTA PARIS TECH Modal analysis of a submerged gate PPL Report Gabriel Cerdan Fernandez 6/10/2010 Tutors: Olivier Doare (ENSTA Paris Tech) Eduard Egusquiza (CDIF UPC)

2 Abstract Hydraulic power station have on the entrance off their water circuit a gate to avoid the entrance of animals, tree leaves and other massive bodies that could break the turbine blades. These gates have some fatigue problems induced by the vibration stimulated by the water flow of the circuit. It s very important to take account of the vibration behavior of these structures in order to minimize the effects of it. In this project a modal analysis of a reduced scale gate will be performed. This analysis will be made by two different methods: simulation and experimentation in order to create a model that could properly substitute the experimental analysis more costly in time and money. The simulation will be made using the modal analysis block of ANSYS. The experimental analysis method used in this project will be the roving hammer method because of its simplicity and efficiency. In the first part of the project the different bars of the structure will be welded together by a unique point. The model will be proved to be able to draw the different mode shapes but not for predicting their frequencies. The cause of these errors will seem to be the weak union between the bars of the structure. In fact, in this first part, the bars are embedded together and welded in a unique point that will seem to be no stiff enough to hold properly the bars together. This hypothesis will be proved to be correct in a second part of the project. The bars will be welded together in all their edges and the structure will be stiff enough to consider the structure as a unique body, as done in the model, and the results will prove that the hypothesis was right and the model can be used to predict the modal behavior a well welded gate. For future analysis of real scale gates this model will be able to substitute the experimental analysis in order to save money and time to the university department. It will also be interesting to create in a posterior project a new model that could take account of these weak unions using friction coefficient between embedded bars. 2

3 Table of Contents 1 Introduction Motivation Objective of the project Structure to modelize Modelisation Air Geometry Meshing Boundary conditions Analysis properties Results Water Geometry Meshing Boundary conditions Analysis properties Mesh adjustment Results Experimental Analysis Experimental setup

4 4.1.1 Gate Accelerometer Hammer Acquisition card Computer software Experimental method Obtaining the FRFs Drawing the mode shapes Results Air Water Comparison of simulation and experimental analysis results Hypothesis verification Conclusion

5 1 Introduction 1.1 Motivation At the entrance of the water circuit there is a gate. Its goal is to avoid the entrance of animals, tree leaves or other similar bodies into the liquid circuit. In fact, the aim of the water that goes into the system is to give energy to turbines that produces electricity. So one can imagine that the fluid hits at a very fast speed the turbine blades and any kind of object in the current can break the blades. In some occasions these gates can broke because of the fatigue induced by the vibration caused by the water flowing through. In fact the turbulence appearing after the gate can excite the structure at its vibration modes frequencies inducing high displacements. After several cycles of charging these fatigue effects appears weakening the structure. 1.2 Objective of the project The aim of this project is to find a reliable model to calculate the modal behavior of these structures and to determine in which conditions it can be used. This is very important because modal analysis it s a fundamental step in the designing of these type of structures. 5

6 2 Structure to modelize Figure 2.1. : Reduced scale gate This last is a photo of the gate that is going to be analyzed. It s a steel structure formed by 7 bars that are welded together. In the following graphic one can see the dimension, in mm, of the gate. Figure 2.2. : Sketch of the structure 6

7 3 Modelisation The modelisation of the structure has been done in two different environments: air and water. In the first case the purpose is to analyze the free vibration behavior of the structure. Then in order to establish the effect of the water in the vibration modes of the gate a second simulation is carried out. In this one, the structure is no longer alone, but surrounded by a water volume that modifies the modal behavior. 3.1 Air Geometry The first thing to do was to define the geometry of the gate. In a first approach a unique and massive volume is considered. Figure 3.1. : Geometry This volume has been built by adding the different parts of the structure merging below entities. 7

8 3.1.2 Meshing The next step was to define the material properties and the type of element to be used. The material was set as elastic > linear > isotropic > E=1.525E11 Pa, ν=0.3, ρ=7800 kg/m 3. These properties are used in order to make the first mode frequency coincide with the one obtained in the posterior experimental analysis. The type of element used in a first approach was SOLID 92. The next step was to mesh the volume using the SOLID 92 element described above. For this the meshtool was used. Using different smart sizes the mesh has been improved in order to detect the good mesh size. M1 Solid 92 SS7 M2 Solid 92 SS 6 M 3 Solid 92 SS1 M 4 Solid 92 SS7+Rafinage1 Mode Freq (Hz) Mode Freq (Hz) errf(%) Mode Freq (Hz) errf(%) Mode Freq (Hz) errf(%) 1 270, , ,48 0, ,99 1, , ,58 0, ,45 0, ,96 1, , ,67 0, ,36 0, ,81 1, , ,13 0, ,73 0, ,27 1, , ,38 0, ,77 0, ,39 1, EN = 8011 EN = 9487 EN = EN = Time = 9s Time = 9s Time = 10s Time = 1min 12s Figure 3.2. : Mesh adjustment table In this last table we can see the frequencies calculated for different sizes of the as well as the relative difference between the values obtained with one mesh and the precedent. errf = f i 1 f i 1 f i x100 It appears that M1, M2 and M3 have no big differences in the results given and take more or less the same time to calculate. The fourth mesh gives more accurate results but the difference with the third is not significant. Indeed the values of the material and geometry characteristics can t be measured with more than 10% precision and a 2% difference between the models can be considered insignificant. In 8

9 addition to that the time token for the calculation is 7 times the three others. As this parameter is very important for a model that has to be used several times the selected mesh is M3. After selecting the mesh size another element type has been tested: SOLID 95. M3 Solid 92 SS1 M5 Solid 95 SS 1 Mode Freq (Hz) Mode Freq (Hz) errf(%) 1 270, , , , , , , , , ,77 0 EN = EN = Time = 10s Time = 11s Figure 3.3. : Element choosing table In this last table one can see the results for both elements SOLID 92 and 95 for the same mesh size. It appears that the result is the same as well as the time elapsed for the simulation. The difference between these elements is that 92 has only 10 nodes and 95 has 20. This implies that SOLID 95 has functions of a higher degree than 92. Knowing that a higher degree can involve interpolation problems the element type chosen is SOLID 92. Finally the chosen mesh is made of SOLID 92 element with a smart size of 1. 9

10 Figure 3.4. : Final mesh Boundary conditions There are no boundary conditions to apply because the structure is totally free Analysis properties The analysis type used is the modal analysis using the Block Lanczos extraction method. The number of modes to extract has been settled to 6. Finally the initial shift was 1 Hz in order to avoid the calculation of the solid body oscillation modes Results In the following pictures one can see the different mode shapes resulting from the ANSYS simulation. 10

11 Figure 3.5. : First vibration mode Figure 3.6. : Second vibration mode 11

12 Figure 3.7. : Third (left) and Fourth (right) vibration modes Figure 3.8. : Fifth vibration mode The frequencies associated to the previous mode shapes are the following. M3 Solid 92 SS1 Mode Freq (Hz) 1 270, , , , ,77 Figure 3.9. : Natural frequencies table 12

13 3.2 Water Once the free solid modelisation has been done the next step was to include the water environment in the model. For this the gate has been introduced into a fluid volume simulating the water tank described in the first point of this report Geometry The starting point for the new geometry definition was the previous one. Then in order to modelize the tank a cube has been defined. The gate has been located at the center of it. Finally using the modeling function VSBV, that subtracts a volume to another, without separating the interface surface the solid volume has been subtracted from the water one Meshing Figure : Water environment geometry First it should be noticed that the solid volume has to be meshed again because VSBV function requires unmeshed volumes. Gate material properties still the same. Water has been chosen as an acoustic fluid with ρ=1000 kg/m 3 and c=1497 m/s. Furthermore to types of water has been created. The first has a boundary admission 13

14 mu=1 and the second a mu=0. The first one is for the water elements in contact with the gate and the second one for the others. In fact mu represents the capacity of absorbing efforts and displacements from solids. The element type for the solid still the same, SOLID 92, and for the water it s the FLUID 30. As well as the material properties two types of FLUID 30 are defined: one for the interface and the other for the rest of the water. Once the material properties and element types has been defined it s the moment to mesh the volumes. The first to be meshed is the solid because it will define the nodes on the interface. As seen on the previous part the best meshing size for the gate is smart size 1 and that s the one used. Then the fluid has to be meshed. A smart size of 5 is first tried because the water volume being big generates a lot of elements when meshed and this affects the solving time. This mesh will be refined in a posterior section Boundary conditions Fluid Structure interface The interaction between water and gate has to be defined on the nodes of the interface as well as on the water elements attached to the surface. Nine steps have to be followed for this. First one has to select the nodes of the surface: Select > Entities > Volumes > By picking > From Full > Pick the gate Select > Entities > Areas > Attached to Volumes > From Full Select > Entities > Nodes > Attached to Areas > From Full Now that the interface nodes are selected one has to select the water elements of the interface: Select > Entities > Elements > By attributes > Element Type > 3 > From Full Select > Entities > Elements > Attached to Nodes > Reselect 14

15 The result of these operations is the following: Figure : Nodes and Elements of the interface Once the interface elements selected they have to be switched to material nº2 (water with mu=1) and element type nº2 by using the following function from the left menu of ANSYS: Preprocessor > Modelling > Move / Modify > Elements > Modify Attrib > Pick All > Change both element type and material Now that the water volume is separated in two zones one has to set the nodes of the interface as the FSI (Fluid Structure Interface) by using the following function from the left menu of ANSYS: Preprocessor > Loads > Define Loads > Apply > Fluid/ANSYS > Field Surface > On Nodes > Pick All The final result of these operations is the following: 15

16 Figure : FSI network on the left and both element plus FSI on the right Fluid boundary conditions Two types of conditions have to be set up for the fluid: on the top surface of the cube the pressure has to be 0 because it s the free surface of the water. Furthermore a Real Constant has to be defined for both FLUID 30 elements to settle the reference pressure to Pa. Then on the other sides of the cube the displacement has also to be set at 0 because the tank doesn t allow any displacement. In order to apply these conditions one has first to select the nodes of the appropriate area then to apply the restriction: Select > Entities > Areas > By Pick > From Full Select > Entities > Nodes > Attached to Areas > From Full Preprocessor > Loads > Define Loads > Apply > Fluid/ANSYS > Pressure DOF > On Nodes > Pick All Preprocessor > Loads > Define Loads > Apply > Structural > Displacement > On Nodes > Pick All 16

17 Figure : Boundary Conditions Analysis properties Once again the analysis type performed is Modal Analysis. However because of the boundary conditions of the fluid the system is no longer symmetric so the mode extraction method has to be unsymmetric. Finally the number of modes to extract is 6 and the frequency initial shift 1Hz to avoid the unwanted modes Mesh adjustment To be sure of the suitability of the mesh one has to try different sizes in a decreasing order. By evaluating the differences introduced by the size in the frequencies as it has been done with the natural mode shapes. The solid mesh was the same that was used in the previous study and the one from the fluid was the one modified. The values obtained for different mesh sizes as well as simulation time and element number are presented in the following table. 17

18 M1 S92/F30 SS 5 M3 S92/F30 SS 3 M4 S92/F30 SS 1 M5 S92/F30 SS 1 + Raf 1 Mode Freq (Hz) Mode Freq (Hz) errf(%) Mode Freq (Hz) errf(%) Mode Freq (Hz) errf(%) 1 240, ,15 0, ,04 0, ,64 0, , ,6 0, ,57 0, ,01 0, , ,45 0, ,32 0, ,86 0, , ,33 0, ,61 0, ,9 2, , ,65 0, ,89 0, ,81 2,1226 EN = EN = EN = EN = Time = 16 s Time = 16 s Time = 17 s Time = 12 min 58 s Figure : Element size comparison table It appears that the first three models give similar results, less that 1% difference between consecutive sizes. The simulation times is also very similar and around 17s. Therefore between these three models the third has been chosen. The last one causes some problems. In one hand it clearly appears that the model describes much better the high frequencies modes, there is a difference of more than 2 % in the fourth and fifth mode frequency and 1,8% in the sixth. In the other hand it took 13 min to solve the simulation what represents 45 times the time token for the third. As calculation time is a very important parameter in a numerical model and the difference in the results, even if big, it s not enormous compared to measurement errors one can have in an experimental analysis the model chosen for subsequent analysis is the third: Solid: Solid 92 element and Smart Size 1 Fluid: Fluid 30 element and Smart Size 1 18

19 3.2.6 Results The final results of the simulation using the third model are presented below. Figure : First vibration mode Figure : Second vibration mode 19

20 Figure : Third (left) and fourth (right) vibration modes Figure : Fifth vibration mode Frequencies associated to the previous modes shapes are the following. M4 S92/F30 SS 1 Mode Freq (Hz) 1 240, , , , ,89 Figure : Water submerged frequencies table 20

21 4 Experimental Analysis In order to validate the results obtained during the simulation an experimental analysis has been performed. There are two different types of analysis that can be carried out: the roving accelerometer method and the roving hammer method. For this experiment the second method is used because it s easier to impact in different locations keeping the accelerometer in the same place rather than moving this last. The method consists on exciting the structure with a hammer in several points, capturing the response with a sensor and extracting with PULSE LabShop software the FRF (frequency response function). As the hammer excitation leads to a broad band excitation of the structure, which means that it shows a constant power spectrum up to a given frequency value, all the modes in this range will be excited. By exciting different points and different directions one can use ME scopeves to draw the different mode shapes of the structure. 4.1 Experimental setup To perform this analysis the following elements have been used: gate accelerometer hammer computer with PULSE LabShop and ME'scopeVES Brüel & Kjaer acquisition card 21

22 4.1.1 Gate The gate is the one presented on the first part of the report. It has been suspended from the hook of a little crane using a rope. Figure 4.1. : Gate fastening This setup allows the gate to vibrate in all directions with minimum interference and it's the best founded way to simulate the free vibration behavior. The crane allows moving up and down the structure so it can be introduced into the water container Accelerometer The vibration has been captured by an accelerometer placed in different positions depending on the vibration mode to detect. It s a piezoelectric sensor from Brüel & Kjaer. The type is 4394 and its characteristics can be found in the annex of this report. 22

23 Figure 4.2. : Accelerometer glued to the gate In the picture below one can see the accelerometer subjected to the gate by quick action glue. In fact it is very important to be able to change the sensors position and this method was simple and efficient Hammer The structure has been excited by a hammer with a sensor in its hitting tip. With this sensor it has been possible to record the excitation signal that has been used later to calculate the different FRFs. This sensor is a Brüel & Kjaer nº and its characteristics are described in the annex. 23

24 Figure 4.3. : Hammer Acquisition card The signals have been recorded using a Brüel & Kjaer acquisition card with several modules. The recording module was the 3038, the controller module was the 7537A and finally the power module was the Like the sensors their characteristics are described in the annex. Figure 4.4. : Acquisition card 24

25 4.1.5 Computer software To record, store and analyze the multiple signal obtained from the experimental analysis two different programs have been used. First of all the modal analysis module from PULSE LabShop was used to record and calculate the FRFs of the different excitation points. Then, by transferring the FRFs to ME scopeves the mode shapes were drawn. Figure 4.5. : PULSE LabShop on the left and ME scopeves on the right 4.2 Experimental method Obtaining the FRFs In order to characterize the mode shapes and their frequencies the structure has been excited in different point for different directions. In fact the accelerometer can only capture the movements in its axis direction. So, as seen in the simulation, the different vibration modes take place in different directions and it s indispensable to excite these three directions. In the following table one can see the directions of different mode shapes vibration. 25

26 Mode Direction Figure 4.6. : Mode shapes vibration directions Then in order to draw the mode shapes with ME sopeves it is necessary to excite multiple points for each direction. Indeed to have a good precision in this drawing it s necessary to excite a consistent number of points. Finally the more mode shapes to characterize in a same direction the more precision is needed. This is why the first direction has been hit in 30 points, direction two in 7 points and finally direction three in 8 points. Just like for the excitation the accelerometer has also to be moved to capture each direction displacements. For direction 2 and 3 there is no problem with the position where to fasten it because there is only one mode to characterize and the sensor will be placed in the highest displacement point of the mode. However for the first direction there are 3 modes to draw with ME scope and it would be a waste of time to change the sensor for each of them so it has to be located in a point where all the vibration modes can be detected. Both excitation and caption points are shown in the graphic below Drawing the mode shapes Once the FRFs calculated they have to be saved in a standard format and transferred to ME scopeves. In this last, after drawing the structure, the FRFs have to be matched with the corresponding points. Then after meshing and interpolating the measured displacements the different mode shapes can be reconstructed. For each of these points two things have to be specified: the FRF corresponding to the excitation point and the direction of this excitation. 26

27 4.3 Results Air After this experimental analysis the vibration modes obtained in air are the following. Figure 4.7. : First (left) and second (right) mode shapes Figure 4.8. : Third (left) and fourth (right) mode shapes 27

28 Figure 4.9. : Fifth mode shape In this next table are presented the frequencies associated to the presented mode shapes. Mode Freq (Hz) 1 268, Figure : Vibration modes frequencies 28

29 4.3.2 Water The same analysis has been carried out in a water medium and the results are the following. Figure : First (left) and second (right) mode shapes Figure : Third (left) and fourth (right) mode shapes 29

30 Figure : Fifth mode shape The frequencies associated to the previous mode shapes are presented in the following table. Mode Freq (Hz) Figure : Frequencies of the different mode shapes. 30

31 5 Comparison of simulation and experimental analysis results In order to evaluate the suitability of the model used in the simulation, its results have to be compared with the experimental ones. The differences can appear in to different ways: modes shapes and frequencies associated to this last. The mode shapes in both air and water environment are well predicted by the simulation. In fact all the first sixth mode shapes are exactly the same in the simulation and experimentation. But the differences appear in their frequencies. These aren t well predicted as one can see in the following table. Simulation freq Experimentation (Hz) freq (Hz) Difference (%) Mode Air Water Air Water Air Water 1 270,48 240,04 268, , , ,45 268, , , ,36 380, , , ,73 445, , , ,77 474, , ,76667 Figure 5.1. : Frequencies comparison In the previous table are presented both simulation and experimentation frequencies in both air and water environments as well as the difference between simulation and experimentation for the two mediums. The first thing to notice is that first and second mode frequencies are similar in the simulation and experimentation. The difference is smaller than 10% and by consequent smaller than the standard error of experimentation measures. However for the rest of mode frequencies the difference between simulation and experimentation overcome this 10% threshold and the results of the model can t be validated. Because of that this model can t be used to predict frequencies and has to be modified. Multiple causes of those differences can be extracted from this comparison and so the model can be adjusted to correct the errors committed. Three groups of causes have to be analyzed: numerical causes, problems due to material properties and boundary conditions differing from reality. 31

32 Numerical errors can be introduced by an inappropriate size of the mesh. However a sensibility analysis of the mesh size has been carried out during the simulation process and numerical errors are unlikely to be the principal cause of the difference between simulation and experimentation. Another possible cause is the material properties used in the simulation. The material has been considered as elastic and isotropic. This is totally consistent with reality because the material of the gate is steel without any posterior treatment like forging that could affect the isotropy of the mechanical properties of the metal. Then the characteristics of the steel (Young modulus, poison modulus and density) have been adjusted to make the first mode shape frequency obtained by the simulation match with the one obtained with experimentation. Because of that it s possible that the material properties aren t the one from the steel. However the use of these wrong properties is forced by the simulation errors and material properties are unlikely to be the cause of the difference between simulation and experimentation. Finally the boundary conditions that join the different parts of the structure seem to be the cause of the differences between the results. In fact in the simulation the bars of the gate are perfectly joined and the structure is considered as a unique body. On the other hand the real structure is made of bars embedded and welded in two small points, one on each side of the longitudinal bar. This welding is there only to ensure that the bars don t move one against the other but it doesn t give to the structure any additional stiffness. Unique welding point Figure 5.2. : Zoom of the welding point As the frequencies of the different mode shapes depend on the rigidity of the structure and the union is the week point for the stiffness of the structure it s probable that the union between the bars causes the differences on the results. 32

33 Another parameter that seems to indicate this fact it the difference between air and water frequencies. d a w = f a f a f w x100 In the following table one can see this parameter for the different modes. Difference a w(%) Mode Sim Exp 1 11, , , , ,2883 8, ,31 28, , , , ,5042 Figure 5.3. : Difference between the frequencies in air and water It appears that this parameter is very similar in both simulation and experimentation and the effect of added mass introduced by water seem to be well represented by the simulation. Because of that the only probable cause of the bad suitability of the model is the union between the bars of the structure. 33

34 6 Hypothesis verification There are two different ways to confirm this hypothesis. The first is to increase the stiffness of the union and to see if the results of the simulation are more similar to the experimental. The other way is to try to improve the model used in ANSYS to include that welding point and the embedded bars. In this case the first one is chosen because of its simplicity. By consequent the structure has been welded strongly as described in the following picture. New welding beads Figure 6.1. : Photo of the new welding of the structure In this picture one can see that each bar is welded to its perpendicular by two new welding beads on each side (the same additional welding has been made on the other side). This new union made of tungsten gives reinforced stiffness to the structure. As a result of that it vibrates as it was a unique body as it s modeled in ANSYS. A new experimental modal analysis has been carried out with this new union. It has been compared with the simulation model using now the real properties of steel: E=2.1E11 Pa, ν=0.3, ρ=7800 kg/m 3. 34

35 The results of this comparison are presented in the following table. Experimentation Simulation Comparison Air Water Air Water Air Water Mode Frequency (Hz) Difference (%) ,8 317,5 282,5 2, , ,5 308,3 318,5 314,24 0, , ,3 436, ,74 1, , ,8 487, , , , , , Figure 6.2. : Comparison table It clearly appears that with this new union the results of the simulation and the experimentation are much more similar. In fact the biggest error is of 7,8% which is an acceptable value for a model given the experimental uncertainty. Finally it s confirmed that errors observed in the previous point are introduced by the union between the bars. In fact with the new welding the model can properly predict the vibration behavior of the structure. 7 Conclusion In a first approach the model has been compared to a gate where the bars were welded together by a unique welding point. This union has been proved to be not stiff enough to consider that the structure was a unique body. As a result of that the errors between the model, where the gate was considered as it, and the real behavior were too big to confirm the suitability of the mathematical description. In order to confirm the hypothesis of the weak union as the cause of these differences the structure has been welded properly in all unions. In this new case the model has been proved to properly predict the vibration behavior of the real structure. This model can now be used to perform new modal analysis of bigger gates where the bars are properly welded together. It will be now interesting to create a new model considering the structure not as unique body but as different bars welded in a single point. These bars should also present at their union a friction coefficient to take account of this effect. In fact in the first structure analyzed in this project the bars were embedded together and could move one against each other. Even if this movement was limited by the welding point the bars could still doing it by deforming the welding and the friction effect appeared. 35