Hypermesh和Abaqus的接口分析实例(三维接触分析)
In this tutorial, you will learn how to:
ü Load the Abaqus user profile and model
ü Define the material and properties and assign them to a
component
ü View the *SOLID SECTION for solid elements
ü Define the *SPRING properties and create a component collector for
it
ü Create the *SPRING1 element
ü Assign a property to the selected elements
Step 1: Load the Abaqus user profile and
model
A set of standard user profiles is included in the
HyperMesh installation. They include: RADIOSS
(Bulk Data Format), RADIOSS (Block Format), Abaqus, Actran, ANSYS,
LS-DYNA, MADYMO, Nastran, PAM-CRASH, PERMAS, and CFD. When the user
profile is loaded, applicable utility menu are loaded, unused
panels are removed, unneeded entities are disabled in the
find, mask, card and
reorder panels and specific adaptations related to
the Abaqus solver are made.
1.
From the Preferences drop down menu, click User
Profiles....
2.
Select Abaqus as the profile name.
3.
Select Standard3D and click OK.
4.
From the File drop down menu, select Open… or click
the Open .hm file icon.
5.
Select the abaqus3_0tutorial.hm file.
6.
Click Open.
Step 2: Define the material properties
HyperMesh supports many different material models
for Abaqus. In this example, you will create the
basic *ELASTIC material model with no temperature variation. The
material will then be assigned to the property, which is assigned
to a component collector.
Follow the steps below to create the *ELASTIC
material model card:
1.
From the Materials drop down menu,
select Create.
2.
Click mat name = and enter STEEL.
3.
Click type= and select MATERIAL.
4.
Click card image = and choose ABAQUS_MATERIAL.
5.
Click create/edit. The card image
for the new material opens.
6.
In the card image, select Elastic in the option
list.
7.
By default, the selected type is
ISOTROPIC. If not, click the switch and select
ISOTROPIC.
8.
By default, the ELASTICDATACARDS= field value is
1. If not, input 1 to set the
number of datalines.
9.
Click the field beneath E(1) and enter 2.1E5.
10.
Click the field beneath NU(1) and enter 0.3.
11.
Click return to accept the changes to the card
image.
12.
Click return to exit the panel.
Step 3: Define the *SOLID SECTION
properties
1.
From the Properties drop down menu,
select Create.
2.
Click prop name= and enter
Solid_Prop.
3.
Choose a color for the property.
4.
Click on type= and set it to
SOLID SECTION. This ensures that sections pertaining
only to solid elements are available as card image options.
Alternatively, the type = field can be set to ALL
ensuring that all available card images are listed.
5.
Click on card image= and select
SOLIDSECTION.
6.
Click material= and select
STEEL.
7.
Click create.
8.
Click return to exit the panel.
Step 4: Assign the property to the
component
Because the material is assigned to the property,
when you assign the property to a component, the material is
automatically assigned as well.
1.
From the Collectors drop down menu,
select Edit and select Components.
2.
Click the yellow comps button and
select INDENTOR and BEAM from the
list.
3.
Click select.
4.
If necessary, click the toggle to switch
to
property= .
5.
Double-click property= and select the
Solid_Prop.
Notice that the card image= and
material= are already set from the Solid_Prop
property.
6.
Click update.
7.
Click return to exit the panel.
Step 5: View the *SOLID SECTION for solid
elements
HyperMesh supports sectional properties for all
elements from the property collector.
Complete the steps below to view the *SOLID SECTION
card for an existing component:
1.
From the Properties drop down menu,
select Card Edit.
2.
Click props and select
Solid_Prop from the list of property collectors.
3.
Click select to finish the selection process.
4.
Click edit to view the *SOLID SECTION property card
image.
5.
Click return to finish the viewing process.
6.
Click return to exit the panel.
Step 6: Define the *SPRING properties
In Abaqus contact problems, it is common to use
weakly grounded springs to provide stability to the solution in the
first loading step. This section explains how to create these
springs and how to create the *SPRING card.
Complete the steps below to create the *SPRING
card:
1.
From the Properties drop down menu,
select Create.
2.
Click prop name= and type in
Spring_Prop.
3.
Choose a color for the property collector.
4.
Click on type= and set it to
LINE SECTION. This ensures that
sections pertaining only to 1D elements are available as card image
options. Alternatively, the type = field can be set to
ALL ensuring that all available card images are
listed.
5.
Click on card image= and select
SPRING.
6.
Click material= and select
STEEL.
7.
Click create/edit.
8.
In the dof1 field, enter 3.
The dof2 field in the *SPRING card is
ignored by Abaqus for SPRING1 elements.
9.
In the Stiffness field, enter 1.0E-5.
10.
Click return to accept the changes to the card
image.
11.
Click return to exit the panel.
Step 7: Create a component collector for the
*SPRING property
1.
From the Collectors drop down menu,
select Create and select
Components.
2.
Click comp name= and type in
GROUNDED.
3.
Choose a color for the property collector.
4.
If necessary, click the toggle to switch
to
property= .
5.
Double-click property= and select the
Spring_Prop.
Notice that the card image = and material = are
already set from the Spring_Prop property.
6.
Click create.
7.
Click return to exit the panel.
To reset the view for further
processing:
1.
Click the isometric view icon .
Step 8: Create the SPRING1 element
1.
From the Mesh drop down menu, select
Assign and select Element Type.
2.
In the 1D sub-panel, click mass = and
select SPRING1.
In HyperMesh, grounded elements are created and
stored as mass elements since they only have one node in the
element connectivity.
3.
Click return to exit the panel.
4.
On the status bar at the bottom of the window, the
name of the current component is displayed. Click on that name.
5.
Select GROUNDED from the list of component
collectors that appears.
As the spring elements are created, they will be
placed in this component.
6.
From the Mesh drop down menu, select
Create and select Masses.
7.
Click nodes and select by id from the pop-up
menu.
8.
In the id = field, enter 451t460b3 and click Enter
on the keyboard.
This shorthand selects all of the nodes from 451 to
460 in increments of 3.
9.
Click create.
10.
Click return to exit the panel.
定义接触面和相互作用
Step 9: Start the Contact Manager
1.
From the Utility menu, click the
Contact Manager button.
The Abaqus Contact Manager dialog opens.
Step 10: Create the "Indentor-top"
surface
1.
Select the Surface tab in the Abaqus Contact
Manager dialog.
2.
Click the New… button.
The Create New Surface dialog opens.
3.
In the Name: field, enter indentor-top.
4.
Select Element based as the type of
surface.
5.
Click Color and select a color.
6.
Click Create….
The Element Based Surface dialog opens for defining
elements and corresponding faces for the surface.
7.
In the Model Browser, expand the Components folder
to display all the contents. Right-click on indentor and
select Isolate.
8.
Click the user views icon and select top.
9.
In the Element Based Surface dialog, select the
Define tab.
10.
In the Define surface for: list, select 3D
solid, gasket.
11.
Click the Elements button.
This opens the element selector
panel.
12.
Click the elems button.
13.
Select by collector.
14.
Check the indentor component and click
select.
You will see the elements in indentor
component highlighted.
15.
Click proceed to return to the Element Based
Surface dialog.
16.
Select Solid skin option from the Select faces by:
radio buttons.
17.
Select a color from the Solid skin color:
button.
18.
Click the Faces button.
This creates a temporary skin of the selected
elements and opens the element selector panel.
19.
Select an element from the top of the solid
skin.
20.
Click the elems button and select by
face.
You will see all faces at the top of the solid skin
are highlighted.
21.
Rotate the model in HyperMesh interface to verify
all desired faces are selected.
You can deselect any element (by right clicking) or
add more if you like.
22.
When you are satisfied with the element faces
selected, click proceed to return to the Element Based Surface
dialog.
23.
Click the Add button to add these faces to the
current surface.
This creates special "face" elements (rectangles
with dot in the middle) for display.
You can reject the recently added "faces" by
clicking the Reject button. You can also delete "faces" from the
Delete Face page.
24.
When satisfied with the surface definition, click
Close to return to the Abaqus Contact
Manager dialog.
Step 11: Create the "Beam-bot"
surface
1.
Select the Surface tab in the Abaqus Contact
Manager dialog and click the Display None button to undisplay all
surfaces.
2.
Click the New… button.
This opens the Create New Surface dialog.
3.
In the Name: field, enter cylinder-top.
4.
Select Element based as the type of surface.
5.
Click the Color: button and select a color.
6.
Click Create….
The Element Based Surface dialog opens for defining
elements and corresponding faces for the surface.
7.
In the Model Browser, expand the Components folder
to display all the contents. Right-click on Beam and select
Isolate.
8.
In the Element Based Surface dialog, select the
Define tab.
9.
In the Define surface for: list, select 3D solid,
gasket.
10.
Click the Elements button.
This opens the element selector panel.
11.
Click the elems button, select by collector, check
Beam component and click select.
This highlights the elements in Beam
component.
12.
Click proceed to return to the Element Based
Surface dialog.
13.
Select Solid skin from the Select faces by: radio
buttons.
14.
Select a color from the Solid skin color:
button.
15.
Click the Faces button.
This creates a temporary skin of the selected
elements and opens the element selector panel.
16.
Select an element from the solid skin, click the
elems button, and select by face.
You will see faces all around the solid skin are
highlighted.
17.
Rotate the model in the HyperMesh interface to
verify all desired faces are selected.
You can deselect any element (by right clicking) or
add more if you like.
18.
When you are satisfied with the element faces
selected, click proceed to return to the Element Based Surface
dialog.
19.
Click the Add button to add these faces to the
current surface.
This creates special "face" elements (rectangles
with dot at the middle) for display.
You can reject the recently added "faces" by
clicking the Reject button. You can also delete "faces" from the
Delete Face page.
20.
When satisfied with the surface definition, click
Close to return to the Abaqus Contact
Manager dialog.
Step 12: Define the surface interaction
property
In this exercise, you will define the *SURFACE
INTERACTION card with corresponding *FRICTION card.
Complete the steps below to create the
"friction1" surface interaction:
1.
Select the Surface Interaction tab at the
Abaqus Contact Manager dialog.
2.
Click the New… button.
This opens the Create New Surface Interaction
dialog.
3.
In the Name: field, enter friction1.
4.
Click the Create… button.
The Surface Interaction dialog opens.
5.
Select the Define tab.
6.
Select Friction option as surface
interaction property.
That makes the Friction tab active.
7.
Select the Friction tab.
8.
Select the Friction type: as Default and
click the Direct option.
Selecting this option means that the exponential
decay and Anisotropic parameters will not be written to the input
file.
9.
In the No of data lines field, enter 1 and
click set.
A single row appears in the Direct table.
10.
Click the first cell on the Friction Coeff column
and enter 0.05.
For Direct and Anisotropic tables:
•
The column numbers in the table will change with
the No of Dependencies selected. The row numbers can be defined at
the No of data lines entry box. Clicking the corresponding Set
button will update the table to have the specified number of
rows.
•
For placing values in the table, click a cell to
make it active and type in the values. The table works like a
regular spreadsheet.
•
You can also read comma-delimited data from a text
file by clicking the Read From a File button. This button opens up
a file browser window. Select the file and click Open to export the
comma-delimited data. The row number will be set to the number of
data lines found in the file.
•
Right-clicking in the table shows a pull down menu
with copy, cut and paste options. Comma-separated data can be
copied/cut into or pasted from clipboard with these options.
Relevant hot keys (for example, Ctrl-c, Ctrl-x and Ctrl-v in
Windows) will also work.
•
Clicking the left mouse button in a cell activates
that cell. Clicking into an already active cell moves the insertion
cursor to the character nearest the mouse.
•
Moving the mouse while the left mouse button is
pressed highlights a selected area.
•
The left, right, up and down arrows moves the
active cell.
•
Shift- extends
the selection in that direction.
•
Ctrl-left arrow and Ctrl –right arrow move the
insertion cursor within the cell.
•
Ctrl -slash selects all the cells.
•
Back space deletes the character before the
insertion cursor in the active cell. If multiple cells are
selected, Back space deletes all selected cells.
•
Delete deletes the character after the insertion
cursor in the active cell. If multiple cells are selected, Delete
deletes all selected cells.
•
Ctrl -a moves the insertion cursor to the beginning
of the active cell. Ctrl-e moves the insertion cursor to the end of
the active cell.
•
Ctrl –minus (-) and Ctrl –equal (=) decrease and
increase the width of the column with the active cell in it.
•
To interactively resize a row or column, move the
mouse over the border while Button-1 or Button-3 (the right button
on Windows) is pressed.
11.
Click OK to return to the Abaqus Contact
Manager dialog.
Step 13: Create the "Beam-Indentor" contact
pair
1.
Go to the Interface tab of the Abaqus
Contact Manager dialog.
2.
Click the New… button.
This opens the Create New Interface dialog.
3.
In the Name: field, enter Beam-indentor.
4.
Select Contact pair as the type of
interface.
5.
Click the Create… button.
The Contact Pair window opens.
6.
Select the Define tab.
7.
Click the Surface: pull down menu to show a list of
the existing surfaces.
8.
Select indentor from the list and click the
Slave>> button to
identify it as the slave surface and move it into the table.
9.
Click the corresponding Review button.
The selected surface is highlighted in red. If the
surface is defined with sets (display option disabled), the
underlying elements are highlighted. Right-click on Review to clear
the highlighting.
The corresponding New button opens the Create New
Surface dialog for creating a new surface. When you are done
creating and defining the surface, the Contact Pair window returns
with the new surface selected as the slave surface.
10.
Repeat steps 7 and 8, selecting Beam and
clicking the Master>>
button to identify it as the master surface.
Note: To more clearly see the surfaces
available for selection, click the icon. This opens an enhanced
browser where you can easily search for the appropriate item. You
can also click the Filter button to filter the items
displayed.
11.
Click the Interaction: drop down list to see a list
of the existing surface interactions.
Note: To more clearly see the interactions
available for selection, click the icon. This opens an enhanced
browser where you can easily search for the appropriate item. You
can also click the Filter button to filter the items
displayed.
12.
Select friction1 from the list as the
interaction property for the current contact pair.
13.
Select the Parameter tab.
14.
Select SmallSliding from the available
options.
15.
Click OK to return to the Abaqus Contact
Manager dialog.
16
Click close to the Abaqus Contact Manager
dialog.
创建载荷和边界条件
Step 14: Define a *STEP card and specify *STATIC
as the analysis procedure
In this exercise, you will create a *STEP card with
the *STATIC analysis procedure.
1.
On the Utility tab, click Step
Manager.
The Step Manager dialog is displayed.
2.
Click New…
3.
In the Name: text box enter step1.
4.
Click Create to create the step.
This creates a step called step1 and opens the Load
Step edit dialog.
5.
From the tree on the left side of the window,
select Title.
The Step heading: option with a disabled field is
displayed.
6.
Activate the Step heading: check box and
enter 100kN load in the text box.
7.
Click Update to store the heading
information into step1.
8.
From the tree, select Parameter.
9.
Activate the Name and Perturbation check
boxes, and click Update. Notice that name
is already set to step1.
10.
From the tree, select Analysis
procedure.
11.
For Analysis type:, select static and
click Update.
In this exercise, you created a step (*STEP) called
step1 and specified *STATIC as the analysis
procedure.
12.
To add a dataline, go to the Dataline
tab and enable Optional dataline.
13.
To add individual data, such as Initial increment,
enable the appropriate field and enter a value. If one entry field
is not enabled, a space will be added in the ASCII file, and the
Abaqus solver uses the default value.
Next, you will define the loads and boundary
conditions.
Step 15: Create constraints (*BOUNDARY)
1.
From the tree, select Boundary.
2.
Click New… and enter
loads_and_constraints in the Name: text box.
3.
Click Create to create the load
collector.
4.
Optionally, click the button in the Display column
and select a color for the load collector.
5.
Make sure the Status check box for
loads_and_constraints is checked. By selecting this check box, you
are adding this load collector into the loadstep.
6.
Click the loads_and_constraints load
collector in the table.
A set of new tabs is displayed on the right.
7.
From the Define tab, keep Type: set to default
(disp).
8.
Click the Define from ‘Constraints’
panel button.
This takes you to the Constraints panel in
HyperMesh. Use this panel to create
constraints.
Step 16: Create constraints from the Constraints
panel
1.
On the toolbar, click the user views icon and
select right.
2.
Click the yellow nodes button and select
by sets.
3.
select ENDS then Click select
buttom.
4.
Activate dof1, dof2, dof3, unactivate dof4, dof5,
dof6.
5.
Click create.
HyperMesh creates constraints at the nodes you
selected.
6.
Click return.
You are returned to the Step Manager
Load Step dialog.
7.
Look at the Load type: line at the bottom of the
Step Manager dialog. Notice that Bc
(short for BOUNDARY) appears on this line, identifying it as a load
type created in the load_and_constraints load
collector. The corresponding load type on the
tree is also highlighted.
Step 17: Create Forces (*CLOAD)
1.
From the tree, double-click Concentrated loads.
2.
Select CLOAD-Force from the expanded options
under Concentrated loads.
3.
Click New… and enter 100KN_loaded in the
Name: text box.
4.
Click Create to create the load
collector.
5.
Optionally, click the button in the Display column
and select a color for the load collector.
6.
Make sure the Status check box for 100KN_loaded is
checked. By selecting this check box, you are adding this load
collector into the loadstep.
7.
Click the 100KN_loaded load collector in the
table.
A new set of tabs is displayed.
8.
From the Define tab, define CLOAD_Force on:
Nodes or geometry.
9.
From Define tab, click Define from ‘Forces’
Panel.
The HyperMesh Forces panel is
displayed. Use this panel to create forces.
Step 18: Create forces from the Forces
panel
1.
From the graphics area, click the central node on
the front side of the indentor.
2.
In the magnitude: text box, enter –100 kN.
3.
Click the switch next to N1, N2, N3 and select
Y-axis.
4.
Click create.
5.
Click return.
You are returned to the Step Manager
Load Step dialog.
6.
Notice that Cload-f is now added to the Load type:
line, indicating CLOAD-force as another load type created in the
loads_and_constraints load collector. The
corresponding load types on the tree are also highlighted.
7.
From the Load Step dialog, left-click
Review.
The constraints and forces that belong to the
loads_and_constraints load collector are highlighted.
8.
Right-click Review.
The highlighted constraints and forces revert back
to the load collector color.
Steps 19-20: Define Output
Requests(定义输出)
In this exercise, you will specify several output
requests for step1. There are two methods for
defining output request described below.
Step 19: Request ODB file outputs
1.
From the tree, double-click Output request.
2.
Select ODB file from the expanded options under
Output request.
3.
Click New… and enter step1 output in the
Name: text box.
4.
Click Create.
5.
Click step1 output (which you just created).
A new set of tabs is displayed on the right.
6.
From the Output tab, activate the Output check
box. Leave Output set to field.
7.
Activate the Node output and Element
output options.
The Node Output and Element Output tabs are
activated.
8.
Click the Node Output tab.
9.
Click Displacement and activate the U check
box.
U is added to the data line on the
right. You are now requesting displacement
results in the ODB file.
Note: You can manually type in an output
request into this table, including unsupported requests. They will
be written out as entered in the table.
10.
Click Update.
11.
Click the Element Output tab.
12.
Activate the Position check box and set it to
Nodes.
13.
Click Stress and activate the S check box.
S is added to the data line on the
right. You are now requesting stress results in
the ODB file.
14.
Click Update.
Step 20: Request results file (.fil)
outputs
1.
From the tree, under Output request, select Result
file (.fil).
2.
From the Define tab, activate the Node file
and Element file check boxes.
The Node File and Element File tabs are
activated.
3.
From the Node File tab, in the lower
left area, expand Displacement and activate U.
U is added to the data line on the
right. You are now requesting displacement
results in the .fil file.
4.
Click Update
5.
From the Element File tab, activate the Position
check box and set it to averaged at nodes.
6.
In the lower left area, double-click Stress and
activate S.
S is added to the data line on the right. You are
now requesting stress results in the .fil file.
7.
Click Update.
8.
Click Review.
A text-editor showing the output requests you made
is displayed. This is the format used in the
Abaqus input file (.inp).
9.
Click Close on the text-editor window.
10.
Click Close.
The Load Step edit dialog of Step
Manager closes and you are returned to the main Step Manager
dialog. The main Step Manager dialog displays step1
information as we defined in previous exercises.
11.
Click Close to exit the Step Manager dialog.
Steps 21-22: Export the database to an Abaqus
input file
The data currently stored in the database must be
output to an Abaqus .inp file for use with the Abaqus
solver. The .inp file can then be used to perform
the analysis using Abaqus outside of HyperMesh.
Step 21: Export the .inp file
1.
From the File drop down menu, select
Export....
2.
In the File: field, enter
job1.inp.
3.
Click the Export Options down
arrows.
4.
Click the Export: toggle to all.
5.
Click Apply.
6.
Click Close to close the
Export panel.
Step 22: Save the .hm file and quit
HyperMesh
1.
From the File drop down menu, select
Save as….
2.
Select your working directory and for File name:,
enter job1.hm.
3.
Click Save.
4.
From the File drop down menu, select
Exit.