Example 9.2-1 Determine the ten least natural frequencies and associated mode shapes for a cantilever beam made of Aluminum 1024. The dimensions of the beam are 10 x 1/2 x 1 in³. E = 10 x 10⁶ psi, r = 0.00026 slugs/in³, and n = 0.33. Compare the three-dimensional results with two-dimensional case with brief discussion.

Solution:

q Discretization

Table 9.2-1 Frequencies of the problem

SET TIME/FREQ LOAD STEP SUBSTEP CUMULATIVE

1 160.01 1 1 1

2 317.38 1 2 2

3 1015.7 1 3 3

4 1952.8 1 4 4

5 2451.3 1 5 5

6 2931.1 1 6 6

7 4955.5 1 7 7

8 5371.4 1 8 8

9 6024.5 1 9 9

10 7460.2 1 10 10

Figure 9.2-2 Vibration modes of a three-dimensional cantilever beam

q Solution steps for the problem

Preference	Structure
Preprocessor	Element Type	Add	Structure Solid
				Ref No = 1
	Material Properties	Material library	Isotropic	Enter properties
	Modeling	Create	Volume / Block	By Dimension	Type in x,y,z-values
	Meshing	Shape & Size	Manual / Lines / Picked Lines	Pick lines (see the mesh)	Enter NDIV = 1 and 10
		Mesh	Volumes / Mapped	4 or 6 sided	Pick the model
Solution	New Analysis	Modal
	Analysis Option	Subspace	No. of modes to extract = 10	Start Freq = 0, End Freq = 10^6	Rigid body motion = none (make sure to have none for no rigid body motion)
	Loads	Apply	Displacement	On Nodes	Select all nodes on fixed side > All DOFs = 0.
	Solve	Current LS (load step)	Close data and click ok
General Post Processor	Results Summary	See all frequencies
	Read Results / First set
	Plot Results	Contour plot / Nodal Solution	DOF Solution / VSUM & Deformed + undef edge	First mode
	Read Result / Next set
	Plot Results	Contour plot / Nodal Solution	Deformed + undef edge	Second mode
	Read Result / Next set
	Plot Results	Contour plot / Nodal Solution	Deformed + undef edge	Third mode
	Repeat the above steps for all other mode shapes.

Note that there are five different modes of vibration; one deflection mode each in x,y,z-directions, one twisting mode, and one axial mode.

The two-dimensional results are shown below. Note that these results are close to three-dimensional case, but show vibrations only in x and y-directions.

Figure 9.2-3 Vibration modes of a two-dimensional cantilever beam

Example 9.2-2 Find the solution of an incompressible viscous flow of fluid with density 1.94 slug/ft³ and viscosity 0.01 lbf-sec/ft² in a duct shown below. The inlet velocity is 0.1 ft/sec and the gauge pressure is zero at outlet. The governing equations are also shown below. Given are W = 10 ft, H = 2 ft, R = 1/4 ft, a = 3 ft, and b = 1/2 ft. Set the pressure at outlet to zero.

Figure 9.2-4 Domain and boundary conditions

Solution:

(a)

(b)

(c)

(d)

(e)

(f) (g)

(h)

Figure 9.2-5 (a) mesh, (b) errors with iteration, (c) flow vectors, (d) pressure, (e) velocity sum contour, (f) flow around the cylinder, (g) pressures around the cylinder, and (h) flow traces

q Solution steps for the problem

Preference	Flotran
Preprocessor	Element Type	Add	Flotran CFD	FLUID141 (2-D Fluid-Thermal, 4 nodes 2-D space, DOF: VX, VY, VZ, PRES, TEMP, ENKE, ENDS)	Ref No = 1
	Modeling	Create	Area	Rectangle by Dimension	Input the values
		Create	Area	Solid circle	Type in the center position and radius
		Operate	Subtract	Areas	Click the rectangle. In a message box, click “ok”. Then, in the area selection dialog, click “apply”. Next select the circle. Click “next” in a message box and then “ok”. Then, in the area selection box, click “ok” (*).
	Meshing	Shape & Size	Lines / Picked Lines	See below for edge controls
		Mesh	Free / Area
Solution	Loads	Apply	Velocity (step-A)	To select all nodes on lines, do the following.^*^*
Utility Menu	Select	Entities	Select [lines] as shown in the dialog (Figure 9.2-41) and click [ok].	Select all line at top and bottom. Note the semicircle is composed of two lines.	Only selected entities are active for selection.
Ansys Input Window	Type in [nsll,,1]		[nsll] command selects all nodes in selected lines.	This could have been done again by [Select > Entities > select Nodes, Attached to, Lines All > Select All]. See below.
Utility Menu	Plot	Nodes			You will see all nodes on selected lines.
Solution			Now continue (step-A)	On Nodes (step-B)	Select all
					Vx=0, Vy=0
Utility Menu	Select	Entities	Everything	Select all to activate them.
	Plot	Elements
	PlotCtrls	Pan,Zoom,Rotate (PZW)	In the dialog, click [zoom] and zoom the inlet.		Click at center of zoom area you want and while holding down the mouse, move the mouse.
Solution			Continue (step-B)	On nodes	Select all middle nodes
					Vx=0.1, Vy=0
			In the PZW dialog, click [Fit] and then zoom the outlet.	Select all nodes along the outlet. Use [box] selection in selection dialog.	Specify all zero pressures, p=0.
	Flotran Setup	Solution Options			Just look at what options are available.
		Fluid properties	Keep all as [constants] -> [ok]	Density = 1.94
				Viscosity = 0.01
	Run Flotran	See the iteration graph above	If the program does not converge, begin with viscosity value 1. Once it converges, reduce it to 0.1 and run it again. Reduce the viscosity value step-by-step and run until the program converges with desired value of viscosity. Sometime, you may also begin with smaller inlet velocity.
General Post Processor	Read Results	Last set
	Plot Results	Vector plot / predefined	DOF solution/ velocity	Ok	See the result above
		Contour plot / Nodal solution	Pressure	Ok	You can turn on / off the element edge plot by [Util Menu / Plot Ctrls > Style > Edge Options > select EDGE = Edge Only > Ok]
		Flow Trace	Define Trace Points	Enter points at (0, 0.2), (0, 0.4), etc. in the input window
			Plot Flow Trace	DOF Solution / Vsum	Ok

* Since ANSYS picks entities at centroid, when two areas share a point for centroids, a message box will appear asking “previous”, “present” or “next”. Click either one until you see what you desire is highlighted. Then just click “ok” to accept it. Then, in the area selection dialog, click “apply”. This will confirm that the area is selected for subtract operation. Do same thing for second area to subtract from the first.

** In this simple example, the feature “nsll” may not be necessary. Instead. Simply lines can be used to apply boundary conditions. But for complicated boundary this feature is very helpful.

The following table shows the list of lines [Util Menu / List > Lines] where NDIV is the number of divisions of the line for meshing and SPACE the spacing ratio. The spacing ratio is the ratio of the last element size to the first one. Note that for rectangle the edge lines are created from bottom left corner counterclockwise and for circle from left corner to right corner. If the ratio is negative, the bias is done in both direction. For inlet and outlet SPACE = -2 is biasing in both directions with ratio of center element size to edge 2.

LIST ALL SELECTED LINES.

NO. KEYPOINTS LENGTH NDIV SPACE #NODES #ELEM MAT REAL TYP ESYS

1 1 2 10.0 25 1.000 24 0 0 0 0 0

2 2 3 2.00 8 -2.000 7 0 0 0 0 0

3 3 4 10.0 25 1.000 24 0 0 0 0 0

4 4 1 2.00 8 -2.000 7 0 0 0 0 0

5 5 6 .393 5 2.000 4 0 0 0 0 0

6 6 7 .393 5 .500 4 0 0 0 0 0

7 7 8 .393 5 2.000 4 0 0 0 0 0

8 8 5 .393 5 .500 4 0 0 0 0 0

Figure 9.2-6 List of selected lines and information

Figure 9.2-7 Edge controls for meshing with SPACE

Figure 9.2-8 Selection dialog for lines and nodes attached to lines

q Discussion

The channel length after the cylinder is long enough for fully developed flow. The convergence of the nonlinear viscous flow problem depends on not only the fluid properties that directly affect the degree of nonlinearity, but also the mesh. Thus, the mesh must be carefully constructed if possible.

Example 9.2-3 (a) A short pressure vessel with spherical caps at both ends is investigated with cylindrical part and cap together. The cylinder that is 4 in high and has 5 in radius with 0.1 in thickness has internal pressure 100 psi. Model it with 1 / 8-th of cylinder and cap. Using the Shell63 element determine the max hoop stress, axial stress, and von Mises stress and its maximum location. (b) Also, compare this case with a vessel of longer size of 8 in height and (c) with an 8 in long vessel with flat caps. Specify the number of divisions on the boundaries as shown in the mesh below and do free meshing. Material properties are E = 10 x 10⁶ psi and n = 0.25.

Figure 9.1-1 Solid model and mesh on the quarter surface

Solution:

q Modeling

1. Create a vertical line and an arc (to be extruded about an axis of rotation) on x-z plane as follows:

2. First, create key points that will used in subsequent modeling to define axis and axis of rotation by [Modeling > Create > Key Points > In Active CS > enter a key point number and coordinates (1 & 5, 0, 0) > repeat to create three others as (2 & 5, 0, 2), (3 & 0, 0, 7), and (4 & 0, 0, 2)]. The first two points will be used for vertical edge of the cylinder and the second, third, and last points are used for an arc for spherical dome.
3. Create > Lines / Straight Lines > select two key points at (5,0,0) and (5,0,2).
4. The entities can be drawn only on working plane. But there are cases in which they can be created based on existing entities like keypoints. Two different ways of creating arc are explained here.

a. Use directly the key points by [Modeling / Create > Lines / Arcs > By End KPs & Rad > pick on starting keypoint and ending keypoint on the screen > Ok > pick on the keypoint at (0, 0, 2) to indicate the side of the center location > Ok > enter Radius of the arc = 5 > Ok]

b. Alternatively, follow the next two steps.

c. Change the WP (working plane) [Util / WorkPlane > Align WP with > Key Points > pick on three key points in sequence to defind the origin at (0,0,2), x-axis by keypoint at top end of the line, and y-axis by key point at (0,0,7)]. This will define WP on vertical plane on which user can draw lines and surfaces.

d. Create an arc on WP with radius of 5 in and 90^o angle [Create > Lines / Arcs > By Center & Radius > pick on the key point at origin (if you selected wrong point, click mouse right button and deselect and restart) > Type in the radius 5 in the input window > in the dialog define 90^o for arc length in degrees].

5. Extrude the lines by [Modeling / Operate > Extrude / Sweep > Lines / About Axis > pick two keypoints starting with at (0, 0, 2) and at the top end of the arc > Ok]. Make sure to select two key points in sequence to define the direction of rotation, which is defined by right-hand rule (i.e., wrapping the axis with your right hand will give you the direction it’s going to rotate). By now you should see the first figure above.

q Meshing

6. Control the mesh by [Shape & Size > Lines / Picked Lines > pick both edges of cylinder > Apply > NDIV = 1 > Apply > pick two horizontal lines > Apply > NIDV = 4 > Apply pick the rest > Apply > NDIV = 3 > Ok].
7. [Meshing / Mesh > Areas > Free > pick on the areas]. This should show the mesh in the above figure.

q Boundary Conditions and Solution

8. Apply boundary conditions [Apply > Displacement > Symmetric B.C. / On Lines > pick all edges (they are all symmetric boundaries). Then, apply pressure on internal surfaces 100 psi.
9. Solve it by [Solve > Current LS > Ok]. If a warning message appears with warping factor, refine the mesh by [Preprocessor / Meshing > Refine > All > Ok] and resolve it.

q General Postprocessing and Discussion

10. To display the hoop stress on the cylinder, change the results coordinate system to global cylindrical coordinate system by [Options for Output > choose Global Cylindrical > Ok]
11. Plot the hoop stress by [Plot Results > Nodal Solution > Stress / SY (i.e., q-component) > Def + undef edge > Ok].

The following figures show the tangential stress and von Mises stress. The max stress occurs at the bottom. This result is not axi-symmetric due to the non-axisymmetric mesh. The max hoop stress is 5408 psi that is about 8 % higher than what was predicted before for a long cylindrical pressure vessel where the end effects were considered negligible. Also observe how the vessel has deformed.

Figure 9.1-2 Hoop stress, von Mises stress, and deformation

Example 9.2-4 Perform the same analysis as in the previous problem with doubled cylinder height and investigate the changes on hoop stress.

Solution:

q Modification and Solution

Further analysis can be performed to see the effect of the length of the cylindrical part.

1. First delete the boundary condition on bottom edge of the cylinder by [Solution / Loads > Delete > Structural / Displacement > On Lines > pick on the line > Ok]
2. Copy a line at edge of the cylinder by [Preprocessor / Modeling > Copy > pick a line at edge of the cylinder > Ok > enter offset distance in Z-direction DZ = -2 > Ok]
3. Extrude the bottom edge of the cylinder along this line by

a. [Modeling / Operate > Extrude / Sweep > Lines / Along Lines > pick on the bottom edge of cylinder > Ok > pick on the copied line > Ok]

4. The area just extruded actually has area normal opposite to the rest area in this case and must be switched by Area Normals. Switch the area normal by [Modeling / Move / Modify > Areas > Area Normals > pick on the areas to change > Ok > Ok].
5. Mesh the new area by [Meshing / Mesh > Areas / Free > pick on the new area > Ok]
6. Before boundary conditions are imposed on newly created edges, delete the line used for extrusion by [Preprocessor / Modeling > Delete > Line and Below > pick the line > (there are two lines at this position and the first one is the one to delete) Ok > Ok]
7. Apply boundary conditions [Solution / Loads > Apply > Structural / Displacement > Symmetric B.C. / On Lines > pick newly created edges > Ok]
8. Apply the pressure boundary condition on the new area
9. Solve the problem

Shown below is the hoop and von Mises stresses for a pressure vessel with 4 inch high cylindrical part (i.e., full height is 8 in). It clearly display smaller hoop stress than shorter vessel above. Can you find the optimum height of the vessel for cylindrical part to be able to ignore the end effect? Actually, this result already shows very close value to theoretical hoop stress 5000 psi.

Figure 9.1-3 Hoop stress and von Mises stress in longer vessel

Example 9.2-5 Perform the same analysis as in the previous problem with varying cylinder height and flat tops, and investigate the effect of the types of cap on the hoop stress.

Solution:

q Modification and Solution

Further analysis can be performed to see the effect of the types of cap.

1. First, clear the mesh on spherical dome and delete the area.without deleting keypoints [Delete > Areas Only]
2. Create the two radial lines [Create > Lines > Straight Line > pick two keypoints for each line]
3. Create the area [Create > Areas > Arbitray > By Lines > pick surrounding lines of the area]

The following results show the end effect on the stresses. The hoop stress exhibits the highest value at the center of the flat cap, compression at joint of cylinder and cap, and theoretical value far away from the end. The axial stress exhibits max compressed value at the joint and theoretical value far away from the end. Results with much longer cylinder shows almost same results. Thus, about 2 ~ 4 in away the end effects can be ignored in calculation of stresses.

(a) (b) (c)

(d) (e) (e)

Figure 9.1-4 (a) Hoop stress, (b) axial stress, (c) von Mises stress, (d) hoop stress, (e) axial stress with flat cap, and (e) hoop stresses in both cases along axial distance from the joint with cap