Collection_Abaqus.pdf

Abaqus/CAE (ver. 6.11) Shell Tutorial Problem Description The aluminum arch (E = 70 GPa, ν = 0.3) shown below is completely clamped along the flat faces. The arch supports a pressure of 100 MPa.

In this example, we also practice how to mesh a “portion” of geometry and how to avoid modeling unnecessary segments!

©2012 Hormoz Zareh & Jenna Bell

1

Portland State University, Mechanical Engineering

Analysis Steps 1. Start Abaqus and choose to create a new model database 2. In the model tree double click on the “Parts” node (or right click on “parts” and select Create)

3. In the Create Part dialog box (shown above) name the part and a. Select “3D” b. Select “Deformable” c. Select “Shell” d. Select “Extrusion” e. Set approximate size = 100 f. Click “Continue…” 4. Create the geometry shown below (not discussed here). Units shown are in mm.


2


a. Click “Done” b. Set Depth = 10 c. Click “OK”

5. Double click on the “Materials” node in the model tree

a. Name the new material and give it a description b. Click on the “Mechanical” tabÎElasticityÎElastic c. Define Young’s Modulus and the Poisson’s Ratio (use SI (mm) units) i. WARNING: There are no predefined system of units within Abaqus, so the user is responsible for ensuring that the correct values are specified ii. See the table of consistent units below

Quantity

SI

SI (mm)

Length

m

mm

Force

N

N

Mass

kg

Time

s

Stress

US Unit (ft) US Unit (inch) ft

in

lbf

lbf

tonne (10 kg)

slug

lbf s2/in

s

s

s

3

2

2

Pa (N/m ) MPa (N/mm )

lbf/ft

2

psi (lbf/in2)

Energy

J

mJ (10–3 J)

ft lbf

in lbf

Density

kg/m3

tonne/mm3

slug/ft3

lbf s2/in4

d. Click “OK”


3


6. Double click on the “Sections” node in the model tree a. Name the section “shell_properties” and select “Shell” for the category and “Homogeneous” for the type b. Click “Continue…” c. Select the material created above (aluminum) and set the thickness to 1 (mm). d. Adjust the thickness integration points if necessary i. For Simpson integration the number of points must be odd and between 3 and 15 ii. For Gauss integration the number of points must be between 2 and 15 e. Click “OK”

7. Expand the “Parts” node in the model tree, expand the node of the part just created, and double click on “Section Assignments” a. Select the entire geometry in the viewport and press “Done” in the prompt area b. Select the section created above (shell_properties). c. Specify shell offset if necessary. For this example use the default of “middle surface”. d. Click “OK”


4


8. In the toolbox area click on the “Partition Face: Sketch” icon a. Select all faces and click “Done” b. Select one of the flat faces as the sketch plane c. Specify “Through All” for the projection distance. Note the arrow should encompass the entire part. d. Select “Flip” if the arrow showing the project direction is incorrect, and/or press “OK” e. Select one of the edges on the end of the part as the vertical sketch direction f. Create a sketch that will divide the part into quarters. For example: draw a vertical line, select the equal distance constraint, pick the node at the upper right, pick the node at the upper left, then pick the drawn vertical line. The constraint will move the line to the midpoint. g. Select “Done”


5


9. Expand the “Assembly” node in the model tree and then double click on “Instances” a. Select “Dependent” for the instance type b. Click “OK”

10. Save the model a. This model will be used as a starting place for further tutorials


6


11. Double click on the “Steps” node in the model tree a. Name the step, set the procedure to “General”, and select “Static, General” b. Give the step a description

12. Expand the History Output Requests node in the model tree, and then right click on H-Output-1 (H-Output-1 was automatically generated when creating the step) and select Delete


7


13. Expand the Field Output Requests node in the model tree, and then double click on F-Output-1 (F-Output-1 was automatically generated when creating the step) a. Uncheck the variables “Strains” and “Contact”

14. Because the part is symmetrical and the flat surfaces are fully restrained only a quarter of the arch needs to be modeled. 15. Because the flat surfaces are assumed to be fully restrained we do not need to include them, and can instead fix just the edge. 16. Double click on the “BCs” node in the model tree a. Name the boundary conditioned “Fixed” and select “Symmetry/Antisymmetry/Encastre” for the type


8


b. Select the edge shown below and click “Done”

c. Select “ENCASTRE” for the boundary condition and click “OK”

Note: Restraining the entire surface will be inefficient, requiring unnecessary meshing of the portion of the geometry which will have no influence on the stiffness properties, and thus the result of simulation. Therefore, the restraint is applied to the shown edge to reduce the problem size. Noting this, the geometry creation could have been simplified right from the start!

17. Double click on the “BCs” node in the model tree a. Name the boundary conditioned “Zsymm” and select “Symmetry/Antisymmetry/Encastre” for the type

b. Select the edge shown below and click “Done”


9


c. Select “ZSYMM” for the boundary condition

d. Repeat for the other edge and select “Xsymm” to apply x-dir symmetry condition. 18. Double click on the “Loads” node in the model tree a. Name the load “Pressure” and select “Pressure” as the type


10


b. Select the quarter of the arch surface with the boundary conditions applied to it c. Select the color corresponding to the top surface d. For the magnitude enter 600


11


19. In the model tree double click on “Mesh” for the Arch part, and in the toolbox area click on the “Assign Element Type” icon a. Select the portion of the geometry associated with the boundary conditions and load b. Select “Standard” for element type c. Select “Linear” for geometric order d. Select “Shell” for family e. Note that the name of the element (S4R) and its description are given below the element controls f. Select “OK”

20. In the toolbox area click on the “Assign Mesh Controls” icon a. Select the portion of the geometry associated with the boundary conditions and load b. Change the element shape to “Quad”

21. In the toolbox area click on the “Seed Edges” icon a. Select the shorter edges of the portion of the geometry associated with the boundary conditions and load i. Select “By Number” method and Specify 5 elements


12


b. Repeat step a. for the longer curved edges of the portion of the geometry associated with the boundary conditions and load ii. Specify 10 elements

c. Select “Done” 22. In the toolbox area click on the “Mesh Region” icon

d. Select the portion of the geometry associated with the boundary conditions and load e. Select “Done”


13


23. In the model tree double click on the “Job” node a. Name the job “arch_linear_static” b. Give the job a description

24. In the model tree right click on the job just created (arch_linear_static) and select “Submit” f. Ignore the message about unmeshed portions of the geometry, click “yes” to continue. g. While Abaqus is solving the problem right click on the job submitted (arch_linear_static), and select “Monitor”

h. In the Monitor window check that there are no errors or warnings iii. If there are errors, investigate the cause(s) before resolving iv. If there are warnings, determine if the warnings are relevant, some warnings can be safely ignored


14


25. In the model m tree right click on the e submitted and a successfuully completeed job (arch_linear_static),, and select “Resultss”

26. In the menu m bar clickk on ViewporttÎViewport Annotations A Options a. Uncheck the “Show comp pass option” b. The locationss of viewport items can be e specified onn the correspo onding tab in the Viewport Annotations Options

© ©2012 Hormoz Zarreh & Jenna Bell

15

P Portland State Uniiversity, Mechanical Engineering

27. Display the deformed contour of the (Von) Mises stress overlaid with the undeformed geometry a. In the toolbox area click on the following icons i. “Plot Contours on Deformed Shape” ii. “Allow Multiple Plot States” iii. “Plot Undeformed Shape”

28. In the toolbox area click on the “Common Plot Options” icon a. Set the Deformation Scale Factor to 10 b. Click “OK”


16


29. To determine the stress values, click on the “probe values” icon a. Set the probe to “Nodes” b. In the viewport mouse over the element of interest c. Note that Abaqus reports stress values from the integration points, which may differ slightly from the values determined by projecting values from surrounding integration points to the nodes i. The minimum and maximum stress values contained in the legend are from the stresses projected to the nodes d. Click on an element to store it in the “Selected Probe Values” portion of the dialogue box

30. The field output tool bar can be used to change the output displayed a. The middle drop down tab selects the field output of interest. b. The right drop down is used to select the variant or component.


17


Abaqus/CAE (ver. 6.10) Material Nonlinearity Tutorial Problem Description A rectangular steel cantilevered beam has a downward load applied to the one end. The load is expected to produce plastic deformation. An experimentally determined stress strain curve was supplied for the steel material. We will investigate the magnitude and depth of plastic strain.

©2011 Hormoz Zareh

1



3. In the Create Part dialog box (shown above) name the part and a. Select “2D Planar” b. Select “Deformable” c. Select “Shell” d. Set approximate size = 200 e. Click “Continue…” 4. Create the geometry shown below (not discussed here)

©2011 Hormoz Zareh

2



a. Name the new material and give it a description b. The stress strain data, shown below, was measured for the material used i. This data is based on the nominal (engineering) stress and strain

Nominal Stress (Pa) Nominal Strain 0.00E+00 0.00E+00 2.00E+08 9.50E-04 2.40E+08 2.50E-02 2.80E+08 5.00E-02 3.40E+08 1.00E-01 3.80E+08 1.50E-01 4.00E+08 2.00E-01

Nominal Stress (Pa)

4.00E+08 3.00E+08 2.00E+08 1.00E+08 0.00E+00 -5.00E-16

2.50E-02

5.00E-02

7.50E-02

1.00E-01 1.25E-01 Nominal Strain

1.50E-01

1.75E-01

2.00E-01

ii. Abaqus expects the stress strain data to be entered as true stress and true plastic strain 1. In addition the modulus of elasticity must correspond to the slope defined by the first point (the yield point) iii. To convert the nominal stress to true stress, use the following equation 1. = (1 + ) iv. To convert the nominal strain to true strain, use the following equation 1. = (1 + ) v. To calculate the modulus of elasticity, divide the first nonzero true stress by the first nonzero true strain vi. To convert the true strain to true plastic strain, use the following equation 1.

©2011 Hormoz Zareh

=

−

3


vii. The results should be

True Stress (Pa) Plastic Strain Elastic Modulus (Pa) 2.002E+08 0.000E+00 2.1083E+11 2.460E+08 2.374E-02 2.940E+08 4.784E-02 3.740E+08 9.436E-02 4.370E+08 1.388E-01 4.800E+08 1.814E-01 c. Click on the “Mechanical” tabÎElasticityÎElastic i. Enter the calculated modulus of elasticity, and Poison’s ratio of 0.3 d. Click on the “Mechanical” tabÎPlasticityÎPlastic i. Enter the calculated true stress and plastic strain 1. Note that you can simply copy your calculated values from Excel (or similar) and paste them into Abaqus e. Click “OK”

6. Double click on the “Sections” node in the model tree a. Name the section “PlaneStressProperties” and select “Solid” for the category and “Homogeneous” for the type b. Click “Continue…” c. Select the material created above (Steel) and set the thickness to 5. d. Click “OK”

©2011 Hormoz Zareh

4


7. Expand the “Parts” node in the model tree, expand the node of the part just created, and double click on “Section Assignments” a. Select the entire geometry in the viewport and press “Done” in the prompt area b. Select the section created above (PlaneStressProperties) c. Verify “From section” is selected under “Thickness” d. Click “OK”


©2011 Hormoz Zareh

5


9. Double click on the “Steps” node in the model tree a. Name the step, set the procedure to “General”, and select “Static, General” b. On the Basic tab, give the step a description and change the time period to 2 i. For this analysis neglect the effects of geometric nonlinearities (Nlgeom = Off)

c. On the Incrementation tab, i. Set the initial increment size to 0.05 ii. Set the maximum increment size to 0.2 ©2011 Hormoz Zareh

6


d. Click “OK” 10. Double click on the “BCs” node in the model tree a. Name the boundary conditioned “Fixed” and select “Symmetry/Antisymmetry/Encastre” for the type

b. Select the left edge and click “Done” c. Select “ENCASTRE” for the boundary condition and click “OK”

11. Double click on the “Amplitudes” node in the model tree a. Name the amplitude “Triangular Loading” and select “Tabular” b. Enter the data points shown below

©2011 Hormoz Zareh

7


i. Abaqus multiplies the load by the amplitude definition, therefore 0 is no load and 1 is the full load

12. Double click on the “Loads” node in the model tree a. Name the load and select “Surface traction” as the type

b. Select the right edge

©2011 Hormoz Zareh

8


c. Under Direction, click edit and select the upper-right corner as the first point, and the lower-right corner as the second point d. For the magnitude, enter 5e6 e. For the amplitude, select the amplitude created above (Triangular loading)

©2011 Hormoz Zareh

9


13. In the model tree double click on “Mesh” for the beam part, and in the toolbox area click on the “Assign Element Type” icon a. Select the entire geometry b. Select “Standard” for element type c. Select “Quadratic” for geometric order d. Select “Plane stress” for family e. Note that the name of the element (S4R) and its description are given below the element controls f. Select “OK”

14. In the toolbox area click on the “Assign Mesh Controls” icon a. Select the portion of the geometry associated with the boundary conditions and load b. Change the element shape to “Quad” c. Set the technique to “Structured”

©2011 Hormoz Zareh

10


15. In the toolbox area click on the “Seed Edges” icon

a. b. c. d.

Select the left and right edges, click “Done” Select “By number” Set “Bias” to “None” Under “Sizing Controls” enter 8 elements, Click “OK”

16. In the toolbox area ensure the “Seed Edges” icon is still selected a. Select the top and bottom edges b. Set “Method” to “By number” and “Bias” to “Single” c. Set the number of elements to 50 d. Set the bias ratio to 2

©2011 Hormoz Zareh

11


e. The bias arrows point towards the direction of the smaller elements, so in this case they should point to the left. If they don’t, click the “Select” button located to the right of “Flip Bias”

f.

Select the top and bottom edges and select “Done”

g. The arrows should now point to the left h. Click the “OK” button

17. In the toolbox area click on the “Mesh Part” icon

18. In the model tree double click on the “Job” node ©2011 Hormoz Zareh

12


a. Name the job “plastic_beam” b. Give the job a description

19. In the model tree right click on the job just created and select “Submit” a. Ignore the message about unmeshed portions of the geometry b. While Abaqus is solving the problem right click on the job submitted, and select “Monitor” c.

d. In the Monitor window check that there are no errors or warnings i. If there are errors, investigate the cause(s) before resolving ii. If there are warnings, determine if the warnings are relevant, some warnings can be safely ignored iii. In the far right column, note how Abaqus adjusted the increment

©2011 Hormoz Zareh

13


20. In the model tree right click on the submitted and successfully completed job, and select “Results”

21. In the menu bar click on ViewportÎViewport Annotations Options a. Uncheck the “Show compass option” b. The locations of viewport items can be specified on the corresponding tab in the Viewport Annotations Options

©2011 Hormoz Zareh

14


22. Display the deformed contour of the (Von) Mises stress a. In the toolbox area click on the following icons i. “Plot Contours on Deformed Shape”


24. Click on the arrows on the context bar to change the time step being displayed a. Click on the three squares to bring up the frame selector slider bar

©2011 Hormoz Zareh

15


25. To change the output being displayed, in the menu bar click on ResultsÎField Output a. Select one of the plastic strain related outputs (PE or PEEQ) b. Click “OK”

Alternatively, you can select the output variable from the corresponding toolbar (shown below).

Hint: If you don’t see the toolbar, go to view Æ Toolbars and activate the “Field output” to display the toolbar (a checkmark will appear next to it). Note that PE displays individual plastic strain (similar to principal strain) components, while PEEQ variable provides the equivalent plastic strain value (similar to vonMises equivalent stress).

©2011 Hormoz Zareh

16


Spring 2011

01/21/11

ABAQUS Tutorial 3D Modeling This exercise intends to demonstrate the steps you would follow in creating and analyzing a simple solid model using ABAQUS CAE. Introduction A solid undergoes thermal expansion due to the application of heat along with deformation due to applied load. Model Definition Consider a thin aluminum cylinder of length 1 m and inner and outer radii 0.2 m & 0.21 m respectively. The cylinder is kept fixed at one end and at the other end a tensile load of 200 kPa is applied. The fixed end of the cylinder is at 273.15 K (the ambient temperature) and the free end at 274.15 K (all other sides are insulated). The cylinder expands due to the heat flow.

The various functions within ABAQUS are organized into modules and we are going to use these modules to define the steps in our procedure. 1. >module load abaqus/6.9-2 2. >abaqus cae 3. Once you start ABAQUS CAE select Create Model Database to create a new model. 4. The default module that opens up is the Part Module.

Part Module: This module allows you to create the geometry required for the problem. To create a 3-D geometry you first create a 2-D profile and then manipulate it to obtain the solid geometry. 1. From the Part Toolbox on the left of the viewport select Create Part. 2. You can name the part as cylinder or anything else you like. We are going to create a deformable solid shape in the 3-D modeling space through extrusion so we do not change the default selections. 3. Enter 1 as the approximate size and click Continue.

4. Click Create Circle Center and Perimeter on the drawing toolbox and enter 0, 0 as the center point in field below the viewport and press Enter. Enter the perimeter point as 0.21, 0 and press Enter to complete the circle. Similarly make another circle with the same center and the perimeter point as 0.2, 0. Press Esc to exit the circle definition and then press Done.

5. Enter the extrusion depth as 1 and press OK.

6. Click Auto-Fit View in the toolbar above to zoom out and view all the points.

This finishes our work in the Part module. Select Module: Property from the toolbar above the viewport. Property Module: In this module you define the material properties for your analysis and assign those properties to the available parts. 1. Select Create Material from the Property Toolbox. 2. Enter material name as Aluminum. Click on the General tab and select Density from the drop-down menu. Type in the mass density as 2700. Click on the Mechanical tab and select Elasticity>Elastic from the drop-down menu. Enter the Young’s Modulus as 70E9 and the Poisson’s Ratio as 0.33. Click on the Mechanical tab and select Expansion. Edit the reference temperature to 273.15 and the expansion coefficient to 23e-6. Click on

the Thermal tab and select Conductivity. Enter the thermal conductivity as 160. Click on the Thermal tab and select Specific Heat. Enter the value as 900 and click OK.

3. Select Create Section from the property toolbox. Name the section as you like. We need a solid homogeneous section for our problem. Click Continue. Select the material as Aluminum and click OK.

4. Click Assign Section on the property toolbox and select the part from the viewport. Click Done below. Select the section you had created and click OK.

Our work in the Property module is done and we select the Assembly Module from the toolbar above the viewport.

Assembly Module: This module allows you to assemble together parts that you have created. Even if you have a single part you need to include it in your assembly. 1. Select Instance Part from the Assembly Toolbox. 2. Select the part you have created from the parts list and then select Instance type: Independent. Click OK.

Select Module: Step from the toolbar above. Step Module: This module allows you to select the kind of analysis you want to perform on your model and define the parameters associated with it. You can also select which variables you want to included in the output files in this modules. You apply loads over a step. To apply a sequence of loads create several steps and define the loads for each of them. 1. Select Create Step from the Step Toolbox. 2. Name the step as you want and select Coupled temp-displacement as the procedure. Click Continue.

3. The edit step dialog box lets you choose the solution technique, the solver type and define the time stepping strategy. 4. Under Basic change the Response to Steady-state and click OK.

The Interaction Module allows you to set up interactions (contact, film), constraints, connectors, fasteners and wire feature between parts. Our problem does not involve any of these features but it will be a good idea to explore this module on your own at a later time. Select Module: Load from the toolbar above. Load Module: The Load Module is where you define the loads and boundary conditions for your model for a particular step (indicated in the toolbar above). You can even define loads and boundary conditions as fields like electric potential, acoustic pressure, etc. 1. Select Create Load from the Load Toolbox. Select Surface Traction and click Continue. Select the top face of the cylinder (z=1) (it gets highlighted in red) and click Done.

2. Change the Traction type to General. Click on the Edit tab under Direction in the dialog box. Enter the starting point of the direction vector as (0, 0, 0) and the end point as (0,0, 1). Enter the Magnitude as 2e5 and click OK.

3. Select Create Boundary Condition from the Load Toolbox. Select Symmetry / Antisymmetry / Encastre and click Continue. Select the bottom face (z=0) of the cylinder and click Done. Select Pinned (U1=0, U2=0, U3=0) and click OK.

4. Again select Create Boundary Condition from the Load Toolbox. Switch Category to Other and select Temperature and click Continue. Select the bottom face of the cylinder and press Done. Enter the magnitude as 273.15 and click OK. Similarly put the top face at 274.15.

Now that we have defined the loads and the boundary conditions we move on to mesh the geometry. Select Module: Mesh from the toolbar above the viewport. Mesh Module: The mesh model controls how you mesh your model – the type of element, their size etc. 1. Select Seed Part Instance from the mesh toolbox. Enter the approximate global size as 0.025.

2. Click on Mesh Part Instance and then on Yes to mesh the model.

3. Select Assign Element Type from the mesh toolbox. Under Family select Coupled Temperature-Displacement and switch Geometric Order to Quadratic. Click OK.

When finished select Module: Job from the toolbar above. Job Module: This module allows you to submit your model for analysis. 1. Select Create Job from the Job Toolbox. Name the job as you like. Select your model and click Continue.

2. You can add a description to the job, allocate memory, allot multiple processors and select precision. Use the default values and click OK.

3. Select the Job Manager from the toolbox and click on the Write Input tab.

4. If you are running the job for the first time it is advisable to run Data Check to check the input file for errors. Click OK to overwrite the job files.

5. Once the data check is completed Submit the job for analysis. Click OK to overwrite the job files. You can click Monitor to observe the progress of the solution process. You can see the errors, warnings, data and message file.

6. Once the job is completed click on the Results tab on the job manager. This opens the Visualization Module for postprocessing. Visualization Module: This model allows you to look at your model after deformation. You can also plot values of stress, displacement, reaction forces, etc. as contours on your model surface or as vectors or tensors. 1. Select Plot Deformed Shape from the Visualization toolbox.

2. Select Plot Contours on Deformed Shape to plot stress contours on the model surface.

3. You can see the location of the maximum & minimum stresses by selecting Contour Options>Limits>Show Location.

4. Select Results>Field Output from the main menu. This opens a dialog box that allows you to select the variable you want to plot in the viewport. 5. Select U (Spatial Displacement at nodes)>Magnitude>OK to plot the displacement contours on the model.

6. To plot displacement vectors click on Plot Symbols on Deformed Shape on the toolbox.

7. You can now animate this plot by selecting Animate Harmonic. Mouse Gestures: Ctrl+Alt+Left Click (MB1): Rotate View Ctrl+Alt+Middle Click (MB2): Pan View Ctrl+Alt+Right Click (MB3): Magnify View Use Shift key to select multiple objects. Note on System of Units: ABAQUS has no built-in system of units. Specify all unit data in consistent units. Some common systems of consistent units: SI: m, N, kg, s, Pa, J, kg/m3 SI (mm): mm, N, tonne (1000 kg), s, MPa, mJ, tonne/mm3 US Unit (ft): ft, lbf, slug, s, lbf/ft2, ft lbf, slug/ft3 Questions, comments? Contact: beatnic@aset.psu.edu

ME 455/555 Intro to Finite Element Analysis

Winter ‘09

Abaqus/CAE truss tutorial

Abaqus/CAE Truss Tutorial (Revised January 21, 2009) Problem Description: Solve for displacements of the free node and the reaction forces of the truss structure shown in the figure. This is the sample problem from the lecture note example. Material is Steel with E = 210 GPa and υ =0.25. 1 kN

1000 mm2

1250 mm2

750 mm

©2009 Hormoz Zareh & Jayson Martinez

1



Winter ‘09



3. In the Create Part dialog box (shown above) name the part and a. Select “2D Planar” b. Select “Deformable” c. Select “Wire” d. Set approximate size = 1 e. Click “Continue…” 4. Create the geometry shown below (not discussed here)


2



Winter ‘09



a. Name the new material and give it a description b. Click on the “Mechanical” tabÎElasticityÎElastic c. Define Young’s Modulus and Poisson’s Ratio (use base SI units) i. WARNING: There are no predefined system of units within Abaqus, so the user is responsible for ensuring that the correct values are specified d. Click “OK”


3



Winter ‘09


6. Double click on the “Sections” node in the model tree a. Name the section “HorizontalBar” and select “Beam” for both the category and “Truss” for the type b. Click “Continue…” c. Select the material created above (Steel) d. Set cross‐sectional area = 0.001 (base SI units, m2) e. Click “OK”

f.

Repeat for the “AngledBar” i. Cross‐sectional area=0.00125


4



Winter ‘09


7. Expand the “Parts” node in the model tree, expand the node of the part just created, and double click on “Section Assignments” a. Select the horizontal portion of the geometry in the viewport b. Click “Done” c. Select the “HorizontalBar” section created above d. Click “OK”

e. Repeat for the angled portion of the geoemetry 8. Expand the “Assembly” node in the model tree and then double click on “Instances” a. Select “Dependent” for the instance type b. Click “OK”


5



Winter ‘09


9. Double click on the “Steps” node in the model tree a. Name the step, set the procedure to “General”, and select “Static, General” b. Click “Continue…” c. Give the step a description d. Click “OK”


6



Winter ‘09


10. Expand the Field Output Requests node in the model tree, and then double click on F‐Output‐1 (F‐ Output‐1 was automatically generated when creating the step) a. Uncheck the variables “Strains” and “Contact” b. Click “OK”

11. Expand the History Output Requests node in the model tree, and then right click on H‐Output‐1 (H‐ Output‐1 was automatically generated when creating the step) and select Delete


7



Winter ‘09


12. Double click on the “BCs” node in the model tree a. Name the boundary conditioned “Pinned” and select “Displacement/Rotation” for the type b. Click “Continue…” c. Select the endpoints on the left (“shift” select ) and press “Done” in the prompt area d. Check the U1 and U2 displacements and set them to 0 e. Click “OK”


8



Winter ‘09


13. Double click on the “Loads” node in the model tree a. Name the load “PointLoad” and select “Concentrated force” as the type b. Click “Continue…” c. Select the vertex on the right and press “Done” in the prompt area d. Specify CF2 = ‐1000 e. Click “OK”


9



Winter ‘09


14. In the model tree double click on “Mesh” for the Truss part, and in the toolbox area click on the “Assign Element Type” icon a. Select “Standard” for element type b. Select “Linear” for geometric order c. Select “Truss” for family d. Note that the name of the element (B21) and its description are given below the element controls e. Click “OK”

15. In the toolbox area click on the “Seed Edge: By Number” icon (hold down icon to bring up the other options)

a. Select the entire geometry and click “Done” in the prompt area


10



Winter ‘09


b. Define the number of elements along the edges as 1 and click “Enter” in the prompt region, then “Done” in response to the next prompt. c. 16. In the toolbox area click on the “Mesh Part” icon a. Click “Yes” in the prompt area

17. In the menu bar select ViewÎPart Display Options a. On the Mesh tab check “Show node labels” and “Show element labels” b. Click “OK”


11



Winter ‘09


18. In the model tree double click on the “Job” node a. Name the job “Truss” b. Click “Continue…” c. Give the job a description d. Click “OK”

19. In the model tree right click on the job just created (Truss) and select “Submit” a. While Abaqus is solving the problem right click on the job submitted (Truss), and select “Monitor”


12



Winter ‘09


b. In the Monitor window check that there are no errors or warnings i. If there are errors, investigate the cause(s) before resolving ii. If there are warnings, determine if the warnings are relevant, some warnings can be safely ignored

20. In the model tree right click on the submitted and successfully completed job (Truss), and select “Results”


13



Winter ‘09


21. In the menu bar click on ViewportÎViewport Annotations Options a. Uncheck the “Show compass option” b. The locations of viewport items can be specified on the corresponding tab in the Viewport Annotations Options c. Click “OK”



14



Winter ‘09


23. In the toolbox area click on the “Common Plot Options” icon a. Note that the Deformation Scale Factor can be set on the “Basic” tab b. On the “Labels” tab check “Show element labels”, “Show node labels”, and “Show node symbols” c. Click “OK”


15




Winter ‘09

16




Winter ‘09


24. To determine the stress values, from the menu bar click ToolsÎQuery Æ Probe Values, and click OK. a. Check the boxes labeled “Nodes” and “S, Mises” b. In the viewport mouse over the element of interest c. Note that Abaqus reports stress values from the integration points, which may differ slightly from the values determined by projecting values from the surrounding integration points to the nodes i. The minimum and maximum stress values contained in the legend are from the stresses projected to the nodes d. Click on an element to store it in the “Selected Probe Values” portion of the dialogue box e. Click “Cancel”

25. To change the output being displayed, in the menu bar click on ResultsÎField Output a. Select “Spatial displacement at nodes” i. Component = U2 b. Click “OK”


17



Winter ‘09


26. To create a text file containing the stresses, vertical displacements, and reaction forces (including the total), in the menu bar click on ReportÎField Output a. For the output variable select (Von) Mises b. On the Setup tab specify the name and the location for the text file c. Uncheck the “Column totals” option d. Click “Apply”


18



Winter ‘09


e. Back on the Variable tab change the position to “Unique Nodal” f. Uncheck the stress variable, and select the U2 spatial displacement g. Click “Apply”

h. On the Variable tab, uncheck Spatial displacement and select the RF2 reaction force i. On the Setup tab, check the “Column totals” option j. Click “OK”


19



Winter ‘09


27. Open the .rpt file with any text editor a. One thing to check is that the total downward reaction force is equal to the applied load (1,000 N)


20


Abaqus/CAE (ver. 6.8) Vibrations Tutorial Problem Description

The two dimensional bridge structure, which consists of steel T‐sections, is simply supported at its lower corners. Determine the first 10 eigenvalues and natural frequencies.

1



2


a. Name the new material and give it a description b. Click on the “Mechanical” tabÎElasticityÎElastic c. Define Young’s Modulus and Poisson’s Ratio (use SI units) i. WARNING: There are no predefined system of units within Abaqus, so the user is responsible for ensuring that the correct values are specified

d. Click on the “General” tabÎDensity e. Density = 7800 f. Click “OK”

3

6. Double click on the “Profiles” node in the model tree a. Name the profile and select “T” for the shape i. Note that the “T” shape is one of several predefined cross‐sections b. C lick “Continue…” c. Enter the values for the profile shown below d. Click “OK”

7. Double click on the “Sections” node in the model tree a. Name the section “BeamProperties” and select “Beam” for both the category and the type b. Click “Continue…” c. Leave the section integration set to “During Analysis” d. Select the profile created above (T‐Section) e. Select the material created above (Steel) f. Click “OK”

4

8. Expand the “Parts” node in the model tree, expand the node of the part just created, and double click on “Section Assignments” a. Select the entire geometry in the viewport b. Select the section created above (BeamProperties) c. Click “OK”


5

10. Double click on the “Steps” node in the model tree a. Name the step, set the procedure to “Linear perturbation”, and select “Frequency” b. Click “Continue…” c. Give the step a description d. Select the radio button “Value” under “Number of eigenvalues requested “ and enter 10 e. Click “OK”

11. Double click on the “BCs” node in the model tree a. Name the boundary conditioned “Pinned” and select “Displacement/Rotation” for the type b. Click “Continue…” c. Select the lower‐left vertex of the geometry and press “Done” in the prompt area d. Check the U1 and U2 displacements and set them to 0 e. Click “OK”

f.

Repeat for the lower‐right vertex, but model a roller restraint (only U2 fixed) instead

6

12. In the model tree double click on “Mesh” for the Bridge part, and in the toolbox area click on the “Assign Element Type” icon a. Select “Standard” for element type b. Select “Linear” for geometric order c. Select “Beam” for family d. Note that the name of the element (B21) and its description are given below the element controls e. Click “OK”

13. In the toolbox area click on the “Seed Edge: By Number” icon (hold down icon to bring up the other options)

a. Select the entire geometry and click “Done” in the prompt area b. Define the number of elements along the edges as 5 14. In the toolbox area click on the “Mesh Part” icon a. Click “Yes” in the prompt area

7

15. In the menu bar select ViewÎPart Display Options a. Check the Render beam profiles option b. Click “OK”

16. Change the Module to “Property” a. Click on the “Assign Beam Orientation” icon b. Select the entire geometry from the viewport c. Click “Done” in the prompt area d. Accept the default value of the approximate n1 direction

17. Note that the preview shows that the beam cross sections are not all orientated as desired (see Problem Description)

8

18. In the toolbox area click on the “Assign Beam/Truss Tangent” icon a. Click on the sections of the geometry that are off by 180 degrees

19. In the model tree double click on the “Job” node a. Name the job “Bridge” b. Click “Continue…” c. Give the job a description d. Click “OK”

9

20. In the model tree right click on the job just created (Bridge) and select “Submit” a. While Abaqus is solving the problem right click on the job submitted (Bridge), and select “Monitor”

10

b. In the Monitor window check that there are no errors or warnings i. If there are errors, investigate the cause(s) before resolving ii. If there are warnings, determine if the warnings are relevant, some warnings can be safely ignored

21. In the model tree right click on the submitted and successfully completed job (Bridge), and select “Results”

11

22. In the menu bar click on ViewportÎViewport Annotations Options a. Uncheck the “Show compass option” b. The locations of viewport items can be specified on the corresponding tab in the Viewport Annotations Options c. Click “OK”

23. Display the deformed contour overlaid with the undeformed geometry a. In the toolbox area click on the following icons i. “Plot Contours on Deformed Shape” ii. “Allow Multiple Plot States” iii. “Plot Undeformed Shape”

12

24. In the toolbox area click on the “Common Plot Options” icon a. Note that the Deformation Scale Factor can be set on the “Basic” tab b. On the “Labels” tab check the show node symbols icon c. Click “OK”

13

25. In the menu bar click on Results ÎStep/Frame a. Change the mode by double clicking in the “Frame” portion of the window b. Observe the eigenvalues and frequencies c. Click “OK”

26. In the toolbox area click on “Animation Options” a. Change the Mode to “Swing” b. Click “OK” c. Animate by clicking on “Animate: Scale Factor” icon in the toolbox area d. Stop the animation by clicking on the icon again

27. Click on the “Next” arrow on the context bar to change the mode

14

28. Expand the “Bridge.odb” node in the result tree, expand the “History Output” node, and right‐click on “Eigenfrequency: …” a. Select “Save As…” b. Name = Frequencies

c. Repeat for “Eigenvalue” d. Observe the XYData nodes in the result tree

29. In the menu bar click on ReportÎXY…

a. b. c. d. e. f. g. h.

Select from = All XY data Highlight “Eigenvalues” Click on the “Setup” tab Click “Select…” and specify the desired name and location of the report Click “Apply” Click on the “XY Data” tab Highlight “Frequencies” Click “OK”

15

30. Open the report (.rpt file) with any text editor

16

Abaqus/CAE Vibrations Tutorial Problem Description

The table frame, made of steel box sections, is fixed at the end of each leg. Determine the first 10 eigenvalues and natural frequencies. WARNING: There is no predefined system of units within Abaqus, so the user is responsible for ensuring that the correct values are specified. Here we use SI units

©2009 Jayson Martinez & Hormoz Zareh 1 Portland State University, Mechanical Engineering


3. In the Create Part dialog box (shown above) name the part and a. Select “3D” b. Select “Deformable” c. Select “Wire” d. Set approximate size = 5 (Not important, determines size of grid to display) e. Click “Continue…” f. Create the sketch shown below


4. In the toolbox area click on the “Create Datum Plane: Offset From Principle Plane” icon a. Select the “XY Plane” and enter a value of 1 for the offset

5. In the toolbox area click on the “Create Wire: Planar” icon a. Click on the outline of the datum plane created in the previous step b. Select any one of the lines to appear vertical and on the right c. In the toolbox area click on the “Project Edges” icon d. Select all of the lines in the viewport and click “Done”

6. In the toolbox area click on the “Create Datum Plane: 3 points” icon (click on the small black triangle in the bottom‐right corner of the icon to get all of the datum plane options) a. Select 3 points on the top of the geometry


7. In the toolbox area click on the “Create Wire: Planar” icon a. Click on the outline of the datum plane created in the previous step b. Select any one of the lines to appear vertical and on the right c. Sketch two lines to connect finish the wireframe of the table d. Click on “Done”


a. Name the new material and give it a description b. Click on the “Mechanical” tabÎElasticityÎElastic c. Define Young’s Modulus (210e9) and Poisson’s Ratio (0.25)


d. Click on the “General” tabÎDensity e. Density = 7800 f. Click “OK” 9. Double click on the “Profiles” node in the model tree a. Name the profile and select “Box” for the shape b. Click “Continue…” c. Enter the values for the profile shown below d. Click “OK”

10. Double click on the “Sections” node in the model tree a. Name the section “BeamProperties” and select “Beam” for both the category and the type b. Click “Continue…” c. Leave the section integration set to “During Analysis” d. Select the profile created above (BoxProfile) e. Select the material created above (Steel) f. Click “OK”


11. Expand the “Parts” node in the model tree, expand the node of the part just created, and double click on “Section Assignments” a. Select the entire geometry in the viewport b. Select the section created above (BeamProperties) c. Click “OK”



13. Double click on the “Steps” node in the model tree a. Name the step, set the procedure to “Linear perturbation”, and select “Frequency” b. Click “Continue…” c. Give the step a description d. Select “Lanczos” for the Eigensolver e. Select the radio button “Value” under “Number of eigenvalues requested “ and enter 10 f. Click “OK”

14. Double click on the “BCs” node in the model tree a. Name the boundary conditioned “Fixed” and select “Symmetry/Antisymmetry/Encastre” for the type b. Click “Continue…” c. Select the end of each leg and press “Done” in the prompt area d. Select “ENCASTRE” for the boundary condition (“ENCASTRE” means completely fixed/clamped) e. Click “OK”


15. In the model tree double click on “Mesh” for the Table frame part, and in the toolbox area click on the “Assign Element Type” icon a. Select “Standard” for element type b. Select “Linear” for geometric order c. Select “Beam” for family d. Click “OK”

16. In the toolbox area click on the “Seed Part” icon a. Set the approximate global size to 0.1

17. In the toolbox area click on the “Mesh Part” icon a. Click “Yes” in the prompt area


18. In the menu bar select ViewÎPart Display Options a. Check the Render beam profiles option b. Click “OK”

19. Change the Module to “Property” a. Click on the “Assign Beam Orientation” icon b. Select the portions of the geometry that are perpendicular to the Z axis c. Click “Done” in the prompt area d. Accept the default value of the approximate n1 direction (0,0,‐1) e. Click “OK” in the prompt area

f.

Select the portions of the geometry that are parallel to the Z axis


g. Click “Done” in the prompt area h. Enter a vector that is perpendicular to the Z axis for the approximate n1 direction (i.e. 0,1,0)

i. Click “OK” followed by “Done” in the prompt area 20. In the model tree double click on the “Job” node j. Name the job “TableFrame” k. Click “Continue…” l. Give the job a description m. Click “OK”


21. In the model tree right click on the job just created (TableFrame) and select “Submit” n. While Abaqus is solving the problem right click on the job submitted (TableFrame), and select “Monitor”

o. In the Monitor window check that there are no errors or warnings i. If there are errors, investigate the cause(s) before resolving ii. If there are warnings, determine if the warnings are relevant, some warnings can be safely ignored

22. In the model tree right click on the submitted and successfully completed job (TableFrame), and select “Results”


23. In the menu bar click on ViewportÎViewport Annotations Options p. The locations of viewport items can be specified on the corresponding tab in the Viewport Annotations Options q. Click “OK”

24. Display the deformed contour overlaid with the undeformed geometry r. In the toolbox area click on the following icons iii. “Plot Contours on Deformed Shape” iv. “Allow Multiple Plot States” v. “Plot Undeformed Shape”

25. In the menu bar click on Results ÎStep/Frame s. Change the mode by double clicking in the “Frame” portion of the window t. Observe the eigenvalues and frequencies u. Leave the dialogue box open to be able to switch the mode shapes while animating


26. In the toolbox area click on “Animation Options” v. Change the Mode to “Swing” w. Click “OK” x. Animate by clicking on “Animate: Scale Factor” icon in the toolbox area

27. Click on a different Frame in the “Step/Frame” dialogue box to change the mode 28. Expand the “TableFrame.odb” node in the result tree, expand the “History Output” node, and right‐click on “Eigenfrequency: …” y. Select “Save As…” z. Name = Frequencies


aa. Repeat for “Eigenvalue” bb. Observe the XYData nodes in the result tree

29. In the menu bar click on ReportÎXY…

cc. dd. ee. ff. gg. hh. ii. jj.

Select from = All XY data Highlight “Eigenvalues” Click on the “Setup” tab Click “Select…” and specify the desired name and location of the report Click “Apply” Click on the “XY Data” tab Highlight “Frequencies” Click “OK”


30. Open the report (.rpt file) with any text editor

Note: Eigen values that are identical indicate similar vibration modes, activated in different planes.


ME 455/555 Intro to Finite Element Analysis Winter ‘10 Abaqus/CAE Axisymmetric tutorial

Abaqus/CAE Axisymmetric Tutorial Problem Description A round bar with varying diameter has a total load of 1000 N applied to its top face. The bottom of the bar is completely fixed. Determine stress and displacement values in the bar resulting from the load.

©2010 Hormoz Zareh & Jayson Martinez 1 Portland State University, Mechanical Engineering


Analysis Steps 1. Start Abaqus and choose to create a new model database 2. In the model tree double click on the “Parts” node (or right click on “parts” and select Create) 3. In the Create Part dialog box (shown above) name the part and select a. Axisymmetric b. Deformable c. Shell d. Approximate size = 0.2 4. Create the geometry shown below (not discussed here)




a. Name the new material and give it a description b. Click on the “Mechanical” tabÎElasticityÎElastic c. Define Young’s Modulus and the Poisson’s Ratio (use SI units) i. WARNING: There are no predefined system of units within Abaqus, so the user is responsible for ensuring that the correct values are specified

6. Double click on the “Sections” node in the model tree a. Name the section “AxisymmetricProperties” and select “Solid” for the category and “Homogeneous” for the type b. Select the material created above (Steel)



7. Expand the “Parts” node in the model tree and double click on “Section Assignments” a. Select the surface geometry in the viewport b. Select the section created above (AxisymmetricProperties)

8. Expand the “Assembly” node in the model tree and then double click on “Instances” a. Select “Dependent” for the instance type

9. In the model tree, under the expanded “Assembly” node, double click on “Sets” a. Name the set “Fixed” b. Select the lower edge of the surface in the viewport



c. Create another set named “Symmetry” d. Select the left edge of the surface in the viewport 10. In the model tree, under the expanded “Assembly” node, double click on “Surfaces” a. Name the surface “PressureLoad” b. Select the top edge of the surface in the viewport

11. Double click on the “Steps” node in the model tree a. Name the step, set the procedure to “General”, and select “Static, General” b. Give the step a description



12. Expand the Field Output Requests node in the model tree, and then double click on F‐Output‐1 (F‐Output‐1 was automatically generated when creating the step) a. Uncheck the variables “Strains” and “Contact”

13. Expand the History Output Requests node in the model tree, and then right click on H‐Output‐1 (H‐Output‐1 was automatically generated when creating the step) and select Delete



14. Double click on the “BCs” node in the model tree a. Name the boundary conditioned “Fixed” and select “Symmetry/Antisymmetry/Encastre” for the type

b. In the prompt area click on the Sets button c. Select the set named “Fixed”

d. Select “ENCASTRE” for the boundary condition



e. Repeat the procedure for the symmetry restraint using the set named “Symmetry”, select “XSYMM” for the boundary condition 15. Double click on the “Loads” node in the model tree a. Name the load “Pressure” and select “Pressure” as the type

b. Select surface named “Pressure” c. For the magnitude enter



16. In the model tree double click on “Mesh” for the Bar part, and in the toolbox area click on the “Assign Element Type” icon a. Select “Standard” for element type b. Select “Linear” for geometric order c. Select “Axisymmetric Stress” for family d. Note that the name of the element (CAX4R) and its description are given below the element controls

17. In the toolbox area click on the “Assign Mesh Controls” icon a. Change the element shape to “Quad” b. Change the Algorithm to “Medial axis” for a more structured mesh





20. In the model tree double click on the “Job” node a. Name the job “Bar” b. Give the job a description



21. In the model tree right click on the job just created (Bar) and select “Submit” a. While Abaqus is solving the problem right click on the job submitted (Bar), and select “Monitor”

b. In the Monitor window check that there are no errors or warnings i. If there are errors, investigate the cause(s) before resolving ii. If there are warnings, determine if the warnings are relevant, some warnings can be safely ignored 22. In the model tree right click on the submitted and successfully completed job (Bar), and select “Results”

23. In the menu bar click on ViewportÎViewport Annotations Options a. Uncheck the “Show compass option” b. The locations of viewport items can be specified on the corresponding tab in the Viewport Annotations Options



24. Display the deformed contour of the (Von) Mises stress a. In the toolbox area click on the “Plot Contours on Deformed Shape” icon

25. To determine the stress values, from the menu bar click ToolsÎQuery ©2010 Hormoz Zareh & Jayson Martinez 12 Portland State University, Mechanical Engineering


a. Check the boxes labeled “Nodes” and “S, Mises” b. In the viewport mouse over the element of interest c. Note that Abaqus reports stress values from the integration points, which may differ slightly from the values determined by projecting values from surrounding integration points to the nodes i. The minimum and maximum stress values contained in the legend are from the stresses projected to the nodes d. Click on an element to store it in the “Selected Probe Values” portion of the dialogue box

26. To change the output being displayed, in the menu bar click on ResultsÎField Output a. Select “Spatial displacement at nodes” i. Invariant = Magnitude

27. To create a text file containing the stresses and reaction forces (including total), in the menu bar click on ReportÎField Output a. For the output variable select (Von) Mises ©2010 Hormoz Zareh & Jayson Martinez 13 Portland State University, Mechanical Engineering


b. On the Setup tab specify the name and the location for the text file c. Uncheck the “Column totals” option d. Click Apply

a. b. c. d.

Back on the Variable tab change the position to “Unique Nodal” Uncheck the stress variable, and select the RF1 reaction force On the Setup tab, check the “Column totals” option Click OK



28. Open the .rpt file with any text editor a. One thing to check is that the total reaction force is equal to the applied load.


Abaqus/CAE (ver. 6.11) Nonlinear Buckling Tutorial Problem Description This is the NAFEMS1 proposed benchmark (Lee’s frame buckling) problem. The applied load is based on the normalized (EI/L2) value of F = 996.389 N. The analysis will investigate post-buckling nonlinear behavior of the frame at the applied load location. This tutorial will also describe x-y plotting capability in Abaqus/CAE, including combining variables to generate load-displacement plots. E = 71.74×109 N/m2 ν = 0.0

0.2 L

0.8 L

L = 1.2 m

F

L 0.02

0.03

1

National Agency for Finite Element Methods and Standards, NAFEMS Non-Linear Benchmarks (Glasgow: NAFEMS, Oct., 1989, Rev. 1.) Test No. NL7.


1





2


5. Double click on the “Materials” node in the model tree a. Name the new material and give it a description b. Click on the “Mechanical” tabÎElasticityÎElastic i. Enter a Young’s modulus of 71740000000, and Poisson’s ratio of 0 c. Click “OK”

6. Double click on the “Profiles” node in the model tree a. Name the profile and select “Rectangular” b. Click “Continue…” c. Enter “0.03” for “a” and “0.02” for “b” d. Click “OK”


3


7. Double click on the “Sections” node in the model tree a. Name the section “beam” and select “Beam” for the category and “Beam” for the type b. Click “Continue…” c. Select the profile created above (rect_beam) and the material created above (Material-1) d. Click “OK”

8. Expand the “Parts” node in the model tree, expand the node of the part just created, and double click on “Section Assignments” a. Select the entire geometry in the viewport and press “Done” in the prompt area b. Select the section created above (beam) c. Click “OK”

9. In the toolbox area click on the “Assign Beam Orientation” button a. Select all the geometry b. Click “Done”


4


c. d. e. f.

Leave the default values of o “0.0,0.0,-1..0” Press the “En nter” key The beam no ormals should d be oriented as shown be low. Click “OK” to o confirm

10. Create a set for the upper-center vertex u a. Expand the Assembly A nod de in the model tree, and tthen double cclick on sets g for the type, Clicck “Continue… …” b. Name the set and select geometry ertex where th he load is app plied, Click “D Done” c. Select the ve

©22011 Hormoz Zareeh & Jenna Bell

5

P Portland State Unniversity, Mechaniccal Engineering

11. Expand the “Assembly” node in th he model tree e and then doouble click on n “Instances” a. Select “Depe endent” for th he instance tyype b. Click “OK”

12. Double click on the “Steps” node in the model tree a. Name the ste ep, set the prrocedure to “G General”, andd select “Stattic, Riks”, Clickk “Continue… …” b. On the Basic tab escription and d i. Give the step a de g non nlinearities on (Nlgeom = O ON) ii. Set geometric iii. Unde er “Stopping criteria” c checck “Maximum m load proporrtionality facto or” and set to o 30


6


c. On the Incrementation tab, i. Set the initial arc length increment size to 0.1 ii. Set the maximum arc length increment size to 2 iii. Set the maximum number of increments to 200

d. Click “OK” 13. Double click on the “BCs” node in the model tree d. Name the boundary conditioned “Pinned” and select “Displacement/Rotation” for the type e. Click “Continue…” f. Select the two free ends of the frame and click “Done” i. Note: to select multiple items, hold the shift key g. Select “U1” and “U2” and set to zero, click “OK”


7


14. Double click on the “Loads” node in the model tree a. Name the load and select “Concentrated force” as the type b. Click “Continue…”

c. Select the point along the top beam near the corner, Click “Done” d. Set “CF1” to 0 and “CF2” to -996.389 e. Click “OK”


8


15. In the model m tree double click on “Mesh” for th he frame partt, and in the ttoolbox area click on the ““Assign Elementt Type” icon a. Select the en ntire geometrry b. Select “Stand dard” for elem ment type c. Select “Lineaar” for geome etric order m” for family d. Select “Beam e. Note that the e name of the e element (B2 21) and its deescription are given below the element controls f. Click “OK”


9


16. In the toolbox area click on the “Seed Part” icon h. Enter 0.08 for “Approximate global size” , click “OK”

17. In the toolbox area click on the “Mesh Part” icon, Click “Yes”

18. Expand the History Output Requests node in the model tree, and then right click on H-Output-1 (H-Output-1 was automatically generated when creating the step) and select Delete

19. Double click on the History Output Requests node i. Name the history and select “Continue…” j. Set the domain to “Sets” and select the set created above k. Leave the frequency set to every increment (n=1) l. For the output variables select the U2 displacement


10


20. In the model tree double click on the “Job” node a. Name the job “frame_buckle” b. Give the job a description


11


21. In the model tree right click on the job just created and select “Submit” m. While Abaqus is solving the problem right click on the job submitted, and select “Monitor”

n. In the Monitor window check that there are no errors or warnings i. If there are errors, investigate the cause(s) before resolving ii. If there are warnings, determine if the warnings are relevant, some warnings can be safely ignored iii. In the far right column, note how Abaqus adjusted the increment


12



23. Display the deformed contour of the (Von) Mises stress a. In the toolbox area click on the following icons i. “Plot Contours on Deformed Shape” b. Note that when including the effects of geometric nonlinearities, the deformation scale factor defaults to a value of 1

24. Click on the arrows on the context bar to change the time step being displayed a. Click on the three squares to bring up the frame selector slider bar


13


25. On the results tree, expand the History Output node and double click on the displacement history created a. Notice that displacement it plotted against Arc Length, not Load or Load Proportionality Factor. b. To plot load against displacement, we will need to extract the values for Load and displacement from the Field Outputs.

26. In the Toolbox area click on the “Create XY Data” icon a. Choose “ODB field output” for “Source” and click “Continue…” b. On the “Variables” tab i. Select “Unique Nodal” for “Position” ii. Expand “CF: Point loads” and select “CF2” iii. Expand “U: Spatial displacement” and select “U2”


14


c. Select the “Elements/Nodes” tab iv. Select “Node Sets” for “Method” v. Select the set created earlier “Top”


15


d. Click “Save”, then “OK” on the next window e. Click “Dismiss” on the “XY Data from ODB Field Output” window 27. Expand the “XY Data” node on the results tree. a. There should now be two sets of data under the node as shown.

b. Double click the “XY Data” node c. For “Source” select “Operate on XY data” d. From the “Operators” list select “combine(X,X)”, It should appear in the expression box at the top of the window. vi. The combine(X,X) operator combines two sets of saved XY data vii. The Y values of the first argument become the X values of the new XY data viii. The Y values of the second argument become the Y values of the new XY data ix. The values are combined wherever the X values of the two arguments align x. For more detail see “Abaqus/CAE User’s Manual” section 45.4.39, “Combining two X-Y data objects”


16


e. Select “U:U2 P1: PART….” From the “XY Data” section and click “Add to Expression” f. Select “CF:CF2 PI: PART….” From the “XY Data” section and click “Add to Expression” g. Since the load and displacement both increase in the negative direction, they need to be multiplied by -1 to make load and displacement increase in the positive direction. h. The final expression should look like:

i. j.

Click “Save As…”, name it “load-displacement”, click “OK” Close the “Operate on XY Data” window

28. Right click on “load-displacement” under the “XY Data” node and select “Plot” k. The buckling behavior can be seen in the plot.


17


29. This data can also be copied into Excel or other programs. l. Right click on “load-displacement” under the “XY Data” node and select “Edit” m. Select all the data in the edit window, right click and choose “Copy” n. Open Excel, right click in an empty cell and choose “Paste”


18


Abaqus CAE (ver. 6.9) Contact Tutorial Problem Description

Note: You do not need to extrude the right vertical edge of the sensor.

©2010 Hormoz Zareh

1



3. In the Create Part dialog box (shown above) name the part and a. Select “3D” b. Select “Deformable” c. Select “Shell” d. Select “Extrusion” e. Set approximate size = 50 f. Click “Continue…” 4. Create the geometry shown below (not discussed here)

©2010 Hormoz Zareh

2


a. Click “Done”

b. Set Depth = 2 c. Click “OK” 5. Double click on the “Materials” node in the model tree

a. b. c. d.

Name the new material and give it a description Click on the “Mechanical” tabÎElasticityÎElastic Define Young’s Modulus and the Poisson’s Ratio (use SI (mm) units) Click “OK”

6. Double click on the “Sections” node in the model tree

©2010 Hormoz Zareh

3


a. Name the section “ShellProperties” and select “Shell” for the category and “Homogeneous” for the type b. Click “Continue…” c. Select the material created above (Steel) and set the thickness to 0.15 d. Click “OK”

7. Expand the “Parts” node in the model tree, expand the node of the part just created, and double click on “Section Assignments” a. Select the entire geometry, except for the vertical face, in the viewport and press “Done” in the prompt area b. Select the section created above (ShellProperties) c. Specify shell offset if necessary d. Click “OK”


©2010 Hormoz Zareh

4


9. Double click on the “Steps” node in the model tree a. Name the step, set the procedure to “General”, select “Static, General”, and click “Continue…” b. Accept the default settings

10. Double click on the “BCs” node in the model tree a. Name the boundary conditioned “Fixed” and select “Symmetry/Antisymmetry/Encastre” for the type

b. Select the horizontal edges on the vertical surface and click “Done” c. Select “ENCASTRE” for the boundary condition and click “OK”

©2010 Hormoz Zareh

5


11. Double click on the “BCs” node in the model tree a. Name the boundary conditioned “Disp” and select “Displacement/Rotation” for the type b. Select the top edge of the triangular portion of the geometry c. Set the y‐displacement to ‐3

©2010 Hormoz Zareh

6


12. Double click on the “Interaction Properties” node in the model tree a. Name the interaction properties and select “Contact” for the type

b. On the Mechanical tab Select “Tangential Behavior” i. Set the friction formulation to “Frictionless” c. On the Mechanical tab Select “Normal Behavior” i. Because the surfaces do not start in contact, change the constraint enforcement method to “Penalty”

13. Double click on the “Interactions” node in the model tree a. Name the interaction, select “Surface‐to‐surface contact”, and click continue b. For the master surface select the lower portion of the geometry and click done i. While applying the fixed displacement, the nodes at the tip of the upper portion of the geometry will make contact at an unknown location on the lower surface ii. Nodes on the slave surface cannot penetrate the surface formed by the element faces on the master surface c. Select the color of the surface corresponding to the top surface d. For the slave surface, set the slave type to “Surface” e. Select the upper portion of the geometry at the free end and click done f. Select the color of the surface corresponding to the bottom surface g. Change the contact interaction properties to the one created above (if not already done)

©2010 Hormoz Zareh

7


©2010 Hormoz Zareh

8


14. In the model tree double click on “Mesh” for the Arch part, and in the toolbox area click on the “Assign Element Type” icon a. Select the portion of the geometry associated with the boundary conditions and load b. Select “Standard” for element type c. Select “Linear” for geometric order d. Select “Shell” for family e. Note that the name of the element (S4R) and its description are given below the element controls f. Select “OK”

15. In the toolbox area click on the “Assign Mesh Controls” icon a. Select the portion of the geometry associated with the boundary conditions and load b. Change the element shape to “Quad” c. Change the technique to “Structured”

©2010 Hormoz Zareh

9



17. In the toolbox area click on the “Mesh Region” icon

b. Select the entire geometry, except for the vertical face c. Select “Done”

18. In the model tree double click on the “Job” node a. Name the job “switch” b. Give the job a description

©2010 Hormoz Zareh

10


19. In the model tree right click on the job just created and select “Submit” d. Ignore the message about unmeshed portions of the geometry e. While Abaqus is solving the problem right click on the job submitted, and select “Monitor”

f.

In the Monitor window check that there are no errors or warnings i. If there are errors, investigate the cause(s) before resolving ii. If there are warnings, determine if the warnings are relevant, some warnings can be safely ignored


©2010 Hormoz Zareh

11




23. To change the output being displayed, in the menu bar click on ResultsÎField Output a. Select the contact pressure at surface nodes (CPRESS) b. Click “OK”

©2010 Hormoz Zareh

12


©2010 Hormoz Zareh

13


ME 455/555 Intro to Finite Element Analysis Winter ‘10 Abaqus/CAE Heat Transfer Tutorial

Abaqus/CAE (ver. 6.9) Heat Transfer Tutorial Problem Description

The thin “L‐shaped” part shown above is exposed to a temperature of 20 oC on the two surfaces of the inner corner, and 120 oC on the two surfaces of the outer corner. A heat flux of 10 W/m2 is applied to the top surface. Treat the remaining surfaces as insulated.




3. In the Create Part dialog box (shown above) name the part and a. Select “3D” b. Select “Deformable” c. Select “Shell” d. Select “Planar” e. Set approximate size = 20 f. Click “Continue…” 4. Create the geometry shown below (not discussed here)




a. Name the new material and give it a description b. Click on the “Thermal” tabÎConductivity c. Define the thermal conductivity (use SI units) i. WARNING: There are no predefined system of units within Abaqus, so the user is responsible for ensuring that the correct values are specified d. Click “OK”



6. Double click on the “Sections” node in the model tree a. Name the section “ShellProperties” and select “Shell” for the category and “Homogeneous” for the type b. Click “Continue…” c. Select the material created above (Steel) and set the thickness to 1 d. Click “OK”

7. Expand the “Parts” node in the model tree, expand the node of the part just created, and double click on “Section Assignments” a. Select the surface geometry in the viewport and press “Done” in the prompt area ©2010 Hormoz Zareh & Jayson Martinez 4 Portland State University, Mechanical Engineering


b. Select the section created above (ShellProperties) c. Click “OK”


9. In the model tree, under the expanded “Assembly” node, double click on “Sets” a. Name the set “OutsideTemp” b. Click “Continue…” c. On the selection toolbar, from the drop down menu select “Edges” d. Select the two surfaces on the outside of the corner (left and bottom edges) in the viewport and press “Done” in the prompt area



e. Create another set named “InsideTemp” f. Select the two surfaces on the inside of the corner in the viewport and press “Done” in the prompt area 10. In the model tree, under the expanded “Assembly” node, double click on “Surfaces” a. Name the surface “HeatFlux” b. Click “Continue…” c. Select the surface in the viewport and press “Done” in the prompt area d. Choose the “Brown” side

11. Double click on the “Steps” node in the model tree a. Name the step, set the procedure to “General”, and select “Heat Transfer” b. Click “Continue…” c. Give the step a description d. Set the reponse to “Steady‐state” e. Click “OK”



12. Double click on the “BCs” node in the model tree a. Name the boundary conditioned “OutsideTemp” and select “Temperature” for the type b. Click “Continue…”

c. In the prompt area click on the Sets button d. Select the set named “OutsideTemp” e. Click “Continue…”



f. Set the magnitude to 293 g. Click “OK”

h. Repeat the procedure for the inside temperature using the set named “InsideTemp”, set the magnitude to 393 13. Double click on the “Loads” node in the model tree a. Name the load “HeatFlux” and select “Surface heat flux” as the type b. Click “OK”

c. Select surface named “HeatFlux” ©2010 Hormoz Zareh & Jayson Martinez 8 Portland State University, Mechanical Engineering


d. For the magnitude enter 10 e.

f. Note that any edge or surface without a boundary condition or load are treated as insulated 14. Expand the “Parts” node in the model tree, expand the node of the “Bracket” part, and double click on “Mesh” 15. In the toolbox area click on the “Assign Element Type” icon a. Select “Standard” for element type b. Select “Linear” for geometric order c. Select “HeatTransfer” for family d. Note that the name of the element (DS4) and its description are given below the element controls e. Click “OK”



16. In the toolbox area click on the “Assign Mesh Controls” icon a. Change the element shape to “Quad” b. Change the algorithm to “Medial axis” to produce a more uniform mesh for this geometry

17. In the toolbox area click on the “Seed Part” icon a. Set the approximate global size to 5 b. Click “OK”


19. In the model tree double click on the “Job” node a. Name the job “HeatFlux” b. Click “Continue…” c. Give the job a description and accept all default parameters d. Click “OK” ©2010 Hormoz Zareh & Jayson Martinez 10 Portland State University, Mechanical Engineering


20. In the model tree right click on the job just created (HeatFlux) and select “Submit” While Abaqus is solving the problem right click on the job submitted (HeatFlux), and select “Monitor”

In the Monitor window check that there are no errors or warnings. If there are errors, investigate the cause(s) before re‐solving 21. In the model tree right click on the submitted and successfully completed job (HeatFlux), and select “Results”



22. To change the output being displayed, in the menu bar click on ResultsÎField Output a. Select “NT11 Nodal temperature at nodes” b. Click “OK”

23. Display the contour of the temperatures a. In the toolbox area click on the “Plot Contours on Deformed Shape” icon

24. To determine the temperature values, from the menu bar click ToolsÎQuery a. Change the probe option to “Nodes” b. Check the boxes labeled “Node ID” and “NT11” c. In the viewport mouse over the node of interest d. When done click “Cancel”


Abaqus CAE (ver. 6.12) Impact tutorial Problem Description

An aluminum part is dropped onto a rigid surface. The objective is to investigate the stress and deformations during the impact.

©2013 Hormoz Zareh

1



3. In the Create Part dialog box (shown above) name the part “Bracket” a. Select “3D” b. Select “Deformable” c. Select “Solid” d. Set approximate size = 200 e. Click “Continue…” 4. Create the geometry shown below (not discussed here). Dimensions are in millimeters. a. Extrude the shape to a depth of 20.

©2013 Hormoz Zareh

2


5. In the Create Part dialog box (shown above) name the part “Rigid” a. Select “3D” b. Select “Analytical rigid” c. Set approximate size = 200 d. Click “Continue…” 6. Create the geometry shown below (not discussed here). Dimensions are in millimeters.

a. Set the extrusion depth to 200 mm.

7. Create a datum point at the center of the plate (midway between diagonal points).

8. From the menu bar select Tools  Reference Point

©2013 Hormoz Zareh

3


a. Select the datum point just created. b. The reference point will be created as shown.

9. Create a surface on the rigid plate. a. Click on the ToolsSurfaceCreate … b. Select the rigid plate. c. You will be prompted to pick a side for internal faces. Pick the color that is likely candidate as the impact surface. In this example, “Brown” has been selected. 10. Double click on the “Materials” node in the model tree

a. Name the new material “Aluminum” and give it a description b. Click on the “Mechanical” tabElasticityElastic c. Define Young’s Modulus and the Poisson’s Ratio (use SI (mm) units) i. Young’s modulus = 70e3, Poisson’s ratio = 0.33 d. Since this is an explicit model, material density must also be defined e. Click on the “General” tab Density i. Density = 2.6 e‐6 f. Click “OK”

©2013 Hormoz Zareh

4


11. Double click on the “Sections” node in the model tree a. Name the section “bracket_sec” and select “Solid” for the category and “Homogeneous” for the type b. Click “Continue…” c. Select the material created above (Aluminum) and Click “OK” 12. Expand the “Parts” node in the model tree, expand the node of the part “Bracket”, and double click on “Section Assignments” a. Select the entire geometry in the viewport and press “Done” in the prompt area b. Select the section created above (bracket_sec) c. Click “OK”

©2013 Hormoz Zareh

5


13. Expand the “Assembly” node in the model tree and then double click on “Instances” a. Select “Dependent” for the instance type b. Select the parts: “Bracket “and “rigid” c. Select “Auto‐offset from other instances” d. Click “OK”

14. Now, rotate the bracket so that the impact will occur at the lower right corner. This will ba accomplished by rotating the object first with respect to the z‐axis followed by rotation about x‐axis. a. Select “Rotate Instance” icon. b. Select the Bracket c. Accept the default values of starting point (0,0,0) by pressing “Enter” d. Enter (0,0,1) for the end point of rotation axis. e. Enter ‐15 (degrees) for Angle of Rotation. The assembly should look similar to the screen shot below. Be sure to confirm the final rotated position by clicking on OK at the prompt region!

15. Now, rotate the bracket about the x‐axis. a. Select “Rotate Instance” icon. b. Select the Bracket c. Accept the default values of starting point (0,0,0) by pressing “Enter” d. Enter (1,0,0) for the end point of rotation axis. e. Enter ‐15 (degrees) for Angle of Rotation. Be sure to confirm the final rotated position by clicking on OK at the prompt region!

©2013 Hormoz Zareh

6


The assembly should look similar to the screen shot below.

16. In the toolbox area click on the “Translate Instance” icon a. Select the “Bracket” geometry, click “Done” b. Select the bottom corner of the bracket as shown. c. Select the reference point on the”Rigid” member as the end point. d.

Click “Ok”

e. The completed assembly should now look like is shown below.

©2013 Hormoz Zareh

7


17. Double click on the “Steps” node in the model tree a. Name the step, set the procedure to “General”, select “Dynamic, Explicit”, and click “Continue…” b. On the “Edit Step” page under the “Basic” tab, set the time period to 0.02 seconds.

18. Double click on the “BCs” node in the model tree a. Name the boundary condition “fix_rigid_plate” and select “Symmetry/Antisymmetry/Encastre” for the type. b. Select the reference point on the bracket geometry and click “Done” c. Select “ENCASTRE” for the boundary condition and click “OK”

19. Open “Field Output Requests” node in the model tree a. Double‐click on the “F‐Output‐1”. b. Change the value of “Interval” to 100. This allows for capturing of more output increments so that impact can be better visualized. c. You may wish to also change the “History output Requests” to allow for better resolution of history output plots.

©2013 Hormoz Zareh

8


20. Select the “Create Predefined Field” icon under the Load module. a. Name the predefined field. b. Pulll down “Initial” step under the Step selection (see figure). c. Set the Category to “Mechanical” and be sure “Velocity” is selected. d. Note the prompt region asks you to select the regions. e. Rotate the image on the screen so that the bracket can be highlighted. Be sure the rigid plate is not selected! f. Click “Done” in the prompt region. g. When prompted, Enter ‐500 [mm/s] in the V2 field of the “Edit Predefined Field” window. The velocity vectors should now be displayed on the screen.

©2013 Hormoz Zareh

9


21. Double click on the “Interaction Properties” node in the model tree a. Name the interaction properties and select “Contact” for the type, click “Continue…”

b. On the Mechanical tab Select “Tangential Behavior” i. Set the friction formulation to “Penalty” ii. Set Friction Coefficient to 0.5 c. On the Mechanical tab Select “Normal Behavior” d. Accept defaults, Click “OK”

22. Double click on the “Interactions” node in the model tree a. Name the interaction, select “General Contact (Explicit) (Explicit)” and click “Continue…” b. Select “All* with self” on the Edit Interactions Window. c. Be sure to assign the appropriate interaction property under “Global Property assignment in the Contact Properties tab of the window. d. Change the contact interaction properties to the one created above (if not already done) e. Click “OK”

©2013 Hormoz Zareh

10


23. Open the “Field Ouput‐1” and change the Interval for the output request to 100.

24. In the model tree double click on “Mesh” for the Bracket part, or use the Module section of the icon panel as shown. a. Select “Explicit” for element type b. Select “Quadratic” for geometric order c. Select “3D Stress” for family d. Select “Tet” tab and be sure the element is C3D10M e. Select “OK”

You may check the “Mesh Control” to be sure only TET elements are being used in meshing. 25. In the toolbox area click on the “Seed Part” icon a. Under “Sizing Controls” set Approximate global size to 2, Click “OK”


©2013 Hormoz Zareh

11


a. Click “Yes”

Caution: The mesh will exceed the ability of student version of the software to solve. You need to use either Academic version or the Research version to be able to run the job. 27. In the model tree double click on the “Job” node a. Name the job b. Give the job a description, click “Continue…” c. Accept defaults, click “OK”

28. In the model tree right click on the job just created and select “Submit” a. While Abaqus is solving the problem right click on the job submitted, and select “Monitor” b. In the Monitor window check that there are no errors or warnings i. If there are errors, investigate the cause(s) before resolving ii. If there are warnings, determine if the warnings are relevant, some warnings can be safely ignored. An example is “information” warning message below: The option *boundary,type=displacement has been used; check status file between steps for warnings on any jumps prescribed across the steps in displacement values of translational dof. For rotational dof make sure that there are no such jumps. All jumps in displacements across steps are ignored

©2013 Hormoz Zareh

12


29. In the model tree right click on the submitted and successfully completed job, and select “Results” 30. 31. To see the effect of impact, you can either animate the deformed shape, or step through each time step of the solution. Here the step‐by‐step method is discussed. a. In the toolbox area click on the following icons i. “Plot Contours on Deformed Shape” ii. Switch to the “First” step of the solution. iii. Click on the “Next” step. iv. Repeat a few times and observe the change in the stress contours, and also be sure the contact does not extend into the rigid surface. You’all also notice that the Bracket will start to separate from the rigid plate!

©2013 Hormoz Zareh

13


32. You may also wish to see the behavior of the system energy, specifically making sure the artificial strain energy is not a substantial percentage of the overall (Internal) energy of the system. a. Click on the “Create XY Data” icon. b. Be sure the “Source” is “ODB History output” then click “Continue…” c. Hold the “CTRL” key and select the energy terms you wish to plot. IN the example below Internal and Artifical energy terms have been selected.

You’ll note that Artificial Energy is a very small portion of the overall Internal Energy, thus the model seems to be valid, at least from the standpoint of element behavior and possibility of errors due to meshing.

©2013 Hormoz Zareh

14


Collection_Abaqus.pdf

Recommend Documents