Buckling Analysis Tutorial PDF

Preview

Summary

Tutorial for Lecture 10...

Description

Tutorial Problem Statements A good tutorial problem should focus on the logical steps in FEM modeling and demonstrate as many aspects of the FEM software as possible. It should also be simple in mechanics with an analytical solution available for validation. Three tutorial problems are covered in this learning module. Tutorial Problem 1 A 3.5m long column made of AISI 304 steel has a square cross-section with dimensions of 100mm x 100mm. This column is used to support a 10 MPa pressure load in multiple setups with varying end conditions. Use FEM analysis to find the buckling load factor (BLF) and critical pressure load (Pc) of the column in each separate circumstance. The end conditions are as follows: a) b) c) d)

One fixed end and one free end (fixed-free) Two fixed ends (fixed-fixed) One fixed end and one pinned end (fixed-pinned) Two pinned ends (pinned-pinned)

1

Tutorial Problem 2 A 3.6 m long L-shaped column made of AISI 304 steel has dimensions as shown in the figure below. The column contains sixty 60 mm diameter holes as seen in the figure below. This column is used to support a 6 MPa pressure load in multiple setups with varying end conditions. Use FEM analysis to find the buckling load factor (BLF) and critical pressure load (Pc) of the column in each separate circumstance. The end conditions are as follows: a) One fixed end and one free end (fixed-free) b) Two fixed ends (fixed-fixed)

2

Tutorial Problem 3 Honeycomb structures are known for their high strength to weight ratios. For simplicity, consider a single honeycomb component with a foil thickness (t) of 0.025mm, a cell size (l) of 3.175mm and a core height (h) of 12.7mm. The material used for the manufacturing of the honeycomb structure is Ti-8Al-1Mo-1V Titanium Alloy and the structure is loaded with a 200,000 Mpa pressure load. For this problem, compare the nominal stress and stress/weight ratio of this honeycomb data to a solid block of the same dimensions.

Honeycomb

Solid Block

3

Attachment C1. SolidWorks-Specific FEM Tutorial 1 Overview: In this section, three tutorial problems will be solved using the commercial FEM software SolidWorks. Although the underlying principles and logical steps of an FEM simulation identified in the Conceptual Analysis section are independent of any particular FEM software, the realization of conceptual analysis steps will be software dependent. The SolidWorks-specific steps are described in this section. This is a step-by-step tutorial. However, it is designed such that those who are familiar with the details in a particular step can skip it and go directly into the next step.

Tutorial Problem 1. A pressure loaded column is subjected to four different environments with different end conditions

0. Launching SolidWorks SolidWorks Simulation is an integral part of the SolidWorks computer aided design software suite. The general user interface of SolidWorks is shown in Figure 1. Main menu

Frequently used command icons

Help icon

Roll over to display “File”, “Tools” and other menus

Figure 1: General user interface of SolidWorks. In order to perform FEM analysis, it is necessary to enable the FEM component, called SolidWorks Simulation, in the software.

4

Step 1: Enabling SolidWorks Simulation o Click "Tools" in the main menu. Select "Add-ins...". The Add-ins dialog window appears, as shown in Figure 2. o Check the boxes in both the “Active Add-ins” and “Start Up” columns corresponding to SolidWorks Simulation. o Checking the “Active Add-ins” box enables the SolidWorks for the current session. Checking the “Start Up” box enables the SolidWorks for all future sessions whenever SolidWorks starts up.

Check “SolidWorks Simulation” boxes Figure 2: Location of the SolidWorks icon and the boxes to be checked for adding it to the panel.

Because this tutorial problem is divided into four parts, this tutorial will be formatted slightly different than in the other available learning modules. The problem requests four different column buckling studies; fixed-free, fixed-fixed, fixed-pinned and pinned-pinned. It is possible to create four separate studies within one part file. However, this greatly reduces the performance of the simulation software and leads to a significant increase in the time required to complete this LM. Thus, only one study will be created. This study will be modified throughout the module to simulate each individual setup and end conditions. The first setup to be evaluated is the fixed-free condition.

Fixed-Free End Conditions 1. Pre-Processing Purpose: The purpose of pre-processing is to create an FEM model for use in the next step of the simulation, Solution. It consists of the following sub-steps:  Geometry creation  Material property assignment  Boundary condition specification  Mesh generation.

5

1.1 Geometry Creation The purpose of Geometry Creation is to create a geometrical representation of the solid object or structure to be analyzed in FEM. In SolidWorks such a geometric model is called a part. In this tutorial, the necessary part has already been created in SolidWorks. The following steps will open up the part for use in the FEM analysis. Step 1: Opening the part for simulation. One of the following two options can be used. o Option1: Open the part file, “Plain_Column.SLDPRT,” in SolidWorks.

The SolidWorks model tree will appear with the given part name at the top. Above the model tree, there should be various tabs labeled “Features”, “Sketch”, etc. If the “Simulation” tab is not visible, refer back to steps 1 and 2 in order to enable the SolidWorks Simulation package. Step 2: Creating a Study o Click the “Simulation” tab above the model tree

o Under the drop-down menu select “New Study” o In the box under “Name” type in “Plain Column Buckling Study” o Select “Buckling” underneath “Type” as in Figure 3 o Click

to create the study

Figure 3: Creating a buckling study

6

1.2 Material Property Assignment The next step in FEM analysis is to apply the material properties to the column. The material is given in the problem as AISI 304 and the SolidWorks libraries can be used to apply the material properties. Step 3: Applying the material

Select in the upper left hand corner of the Simulation ribbon In left-hand section, expand the “SolidWorks Materials” folder Expand the “Steel” section and choose “AISI 304” Make sure the “Linear Elastic Isotropic” option is selected under “Model Type” and units are in SI o Verify the settings with Figure 4 and click “OK”

o o o o

Figure 4: Material property manager in SolidWorks

7

1.3 Boundary Condition Specification Since this is a buckling study, the boundary conditions will consist of fixed and/or pinned connections of the column known as fixtures. The following steps will apply the different end conditions to the column using fixtures. The first step will be to apply the boundary conditions for the column with fixed-free end conditions. Because the top end of the column is free, only one fixture will be applied to the bottom face of the column for this study. Step 4: Applying the fixed end condition to the bottom face

o Click on the icon in the upper left corner of the simulation ribbon to drop down the fixture menu o Select “Fixed Geometry” o With the colored box highlighted, select the lower face of the column as seen in Figure 5 o Click

to create the fixed boundary condition

Figure 5: Applying a fixed boundary condition

The next step is to load the column with the designated pressure load. Due to the nature of columns, the pressure load will be applied to the top face of the column.

8

Step 5: Applying the pressure load

o Click on the icon in the upper left corner of the simulation ribbon to drop down the external load menu o Select “Pressure” o With the colored box highlighted, select the upper face of the column as seen in Figure 6 o Ensure that units of N/mm^2 (MPa) are selected and enter 10 for the magnitude o If necessary, check the “Reverse direction” box such that the arrows are pointing down on the top face o Click

to create the pressure load

Figure 6: Applying the pressure load 1.4 Mesh Generation Purpose: The purpose of the Mesh Generation sub-step is to discretize the part into elements. The mesh consists of a network of these elements. Because a fine mesh is not needed in this example, large element sizes will be used to decrease the required solver running time. Step 6: Meshing the model o Right click on the icon in the model tree o Select “Create Mesh” o Drag the mesh density bar to the “Coarse” setting as shown in Figure 7 o Click

to create the mesh

9

Figure 7: Meshing the model

2. Solution Purpose: The Solution is the step where the computer solves the simulation problem and generates results for use in the Post-Processing step. Step 1: Running the simulation o Within the simulation ribbon, click o When the analysis is finished, the

icon will appear on the model tree

3. Post-Processing Purpose: The purpose of the Post-Processing step is to process the results of interest. For this problem, the buckling load factor (BLF) will need to be acquired in order to calculate the critical pressure load of the column. This BLF value can also help describe the presence of buckling in the column. The following table is SolidWorks’ interpretation of possible BLF values.

BLF Value

Buckling Status

1 < BLF

Buckling not predicted

0 < BLF < 1

Buckling predicted

BLF = 1

Buckling predicted

BLF = -1

Buckling not predicted

-1 < BLF < 0 BLF < -1

Buckling not predicted Buckling not predicted

Notes The applied loads are less than the estimated critical loads. Buckling is not expected. The applied loads exceed the estimated critical loads. Buckling is expected. The applied loads are exactly equal to the estimated critical loads. Buckling is expected. The buckling occurs when the directions of the applied loads are all reversed. For example, if a bar is under tensile load, the BLF should be negative. The bar will never buckle. Buckling is predicted if you reverse all loads. Buckling is not expected even if you reverse all loads.

10

SolidWorks makes it very easy to acquire the BLF of any loaded part. Follow the next step in order to observe this data. Step 1: Displaying the Buckling Load Factor o Right click on the icon in the model tree o Select “List Buckling Load Factors…” o Observe the BLF value o Select “Save” to save the BLF value Now that the buckling load factor has been determined, it can be used to calculate the critical load of the column. In order to do this, simply multiply the BLF by the applied load. This will give the critical load of the column. Therefore: Pcr = Critical Pressure Load = BLF x Applied Load = 3.1929(10MPa) = 31. 31.93 93 MP MPa a

4. Validation Purpose: The purpose of the Validation step is to compare FEM solutions with analytical solutions, or known published results, to validate the correctness of the FEM model. To check the validity of the SolidWorks answers, hand calculations must be carried out to determine the theoretical critical/buckling load of the column. Euler’s formula will be used to carry out these calculations. This formula is as follows:

Where C is the end condition constant, E is the material’s modulus of elasticity, I is the second moment of inertia (or area moment of inertia), l is the column length, and A is the cross-sectional area. The end condition constant C can be determined from the table below. Column End Conditions Fixed - Free Fixed - Fixed Fixed - Pinned Pinned - Pinned

Theoretical Value ¼ 4 2 1

Conservative Value ¼ 1 1 1

Recommended Value ¼ 1.2 1.2 1

From this table, it can be determined that the end condition constant C has a value of ¼ for the fixed-free boundary conditions. The modulus of elasticity (E) value for AISI 304 steel is also defined as 193 GPa while the length of the column is given in the problem statement as 3.5 m. The column’s area moment of inertia (I) is calculated by the equation: ⁄

11

Where b is the base dimension and h is the height dimension of a rectangular cross-section. Because the column has a square cross section, b = h = 100 mm. Therefore: ⁄

⁄

Therefore, the critical pressure load can be calculated as: ⁄

The SolidWorks and hand calculated results are shown in the below table along with the percent difference in results.

Pcr

SolidWorks 31.93

Hand Calculations 32.40

Percent Difference -1.45%

Fixed-Fixed End Conditions

1. Pre-Processing Because many of the steps necessary for this study have already been covered in the fixed-free study, these steps will be skipped in the following three studies. 1.1 Geometry Creation These steps were completed in the fixed-free study and, therefore, need not be repeated. 1.2 Material Property Assignment The material properties were already assigned in the previous study. Because the same material is being used in each study, this step can be skipped. 1.3 Boundary Condition Specification The previous study was composed of fixed-free boundary conditions on the column. In this study, fixed-fixed end conditions are required. Since a fixed boundary condition was applied to the bottom face in the previous study, one of the fixed end conditions is completed. Next, it is time to apply the fixed end condition to the top face of the column. The top fixture must be modified in order to allow free vertical displacement. To allow only vertical displacement, a boundary condition must be applied to each side face to prevent horizontal

12

displacement. If a fixed geometry were used, each side would be completely restrained and the column would exhibit no buckling behavior. Therefore, the approach is to apply a reference geometry to a small portion of each side face near the top of the column to prevent horizontal movement. The length of each face to be fixed will be setl to half of the column’s crosssectional dimension, or 50 mm. A new plane will be used to create a split line which will enable the use of this approach. Step 1: Creating a new plane for the split line o On the main menu, go to “Insert” -> “Reference Geometry” -> “Plane” o With the “First Reference” box highlighted, expand the model tree and select the Top Plane as shown in Figure 8 o Enter 50 for the offset distance o Check the “Flip” box if plane was created above the Top Plane o Click

to create the plane

Figure 8: Creating a new plane

Step 2: Creating a split line o On the main menu, go to “Insert” -> “Curve” -> “Split Line” o Under the type of split, select “Intersection” o With the first colored box highlighted, expand the model tree and select the plane created in the previous step o With the second colored box highlighted, select each side of the column as shown in Figure 9 o Click

to create the split line

13

LM-BK-1

Figure 9: Creating a split line

Now that a split line has been created, it is possible to apply a reference geometry to each upper side face created by the split line. This reference geometry will allow vertical displacement but not horizontal displacement. Step 3: Applying the fixed end condition to the top face

o Click on the icon in the upper left corner of the screen to drop down the fixture menu o Select “Advanced Fixtures” o With the first colored box highlighted, select the four upper side faces created by the split line o With the second colored box highlighted, select a top edge traveling in the z-direction as shown in Figure 10 o Under “Translations,” enter 0 for the allowable displacement distance o Click to create the reference geometry o Repeat these steps once more using another top edge that is perpendicular to the one used above (should travel in the x-direction)

14

Figure 10: Creating reference geometry The next step of the pre-processing procedure would typically be to apply any external loads on the member as required by the problem statement. However, the external load for this study is exactly the same as the previous study. This means that this step can be skipped as it has already been completed. Therefore, the next step in the process is mesh generation. 1.4 Mesh Generation Any time that changes are made within a study, the model must be re-meshed before the simulation can be run. This is done in the same way as described in the previous study. If needed, refer back to step 6 in the fixed-free study for a description on how to create the mesh.

2. Solution Step 1: Running the simulation o Within the simulation ribbon, click o When the analysis is finished, the

icon will appear on the model tree

3. Post-Processing Just as in the previous study, use SolidWorks to display the BLF of the fixed-fixed column. Now that the buckling load factor has been determined, it can be used to calculate the critical pressure load of the column. Pcr = Critical Pressure Load = BLF x Applied Load = 49.892(10MPa) = 498 498.92 .92 M MPa Pa

15

4. Validation Finally, hand calculations will be carried out and the solutions will be compared to the FEM results. Once again, Euler’s formula will be used for these calculations.

Because the cross-sectional dimensions and material properties have not changed since the previous study, the values of E, I and A will remain the same. However, due to the different end conditions, the value of the end condition constant C will change. This new value can be determined from the table below. Column End Conditions Fixed - Free Fixed - Fixed Fixed - Pinned Pinned - Pinned

Theoretical Value ¼ 4 2 1

Conservative Value ¼ 1 1 1

Recommended Value ¼ 1.2 1.2 1

When designing a column, a recommended value of 1.2 should be used for C as it instills somewhat of a safety factor against failure. However, the theoretical value will be used in these calculations as it will yield results much closer to the actual critical pressure load. The theoretical C value from the table can be observed as 4. Also, because 50 mm of the column’s length was used as a fixture, the column’s length is no longer considered to be 3.5 m. The new length of the column is 3.5 m minus 50 mm, or 3.45 m. Therefore, the critical pressure load can be calculated as:

The SolidWorks and hand calculated results are shown in the below table along with the percent difference in results.

Pcr

SolidWorks 498.92

Hand Calculations 533.47

16

Percent Difference -6.48%

Fixed-Pinned End Conditions

1. Pre-Processing Because many of the steps necessary for this study have already been covered and completed in the previous two studies, these steps will not be described in detail and sometimes will be skipped altogether. 1.1 Geometry Creation These steps were completed in the fixed-free study and, therefore, need not be repeated. 1.2 Material Property Assignment Material properties were assigned in the first study. Because the same material is being used in each study, this step can be skipped. 1.3 Boundary Condition Specification The previous study was composed of fixed-fixed boundary conditions on the column. In this study, fixed-pinned end conditions are desired. Once again, the steps necessary to apply the fixed boundary condition to the bottom face can be i...