Hypermesh和Abaqus的接口分析实例（三维接触分析）
摘要：
本材料聚焦 HyperMesh 与主流求解器接口的高级应用技术，系统阐述协同建模与后处理全流程。核心内容涵盖接口基础配置，包括输入输出模板、用户自定义菜单与宏命令设置；详解模型数据定义，涉及材料、截面、单元类型、边界条件与载荷的标准化创建流程；重点演示 inp 文件导入、非线性材料定义、局部坐标系、接触配对、幅值曲线及几何载荷映射等高级功能。同时说明利用 HyperView 进行 ODB 结果文件的可视化分析，包括云图、矢量图与历史曲线绘制，结合大量实操案例，完整覆盖从前处理到后处理的技术链路，提升复杂模型的求解效率与分析精度。
In this tutorial, you will learn how to:
Load the Abaqus user profile and model
Define the material and properties and assign them to a component
View the *SOLID SECTION for solid elements
Define the *SPRING properties and create a component collector for it
Create the *SPRING1 element
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. By default, the selected type is ISOTROPIC. If not, click the switch and select
7. ISOTROPIC.
By default, the ELASTICDATACARDS= field value is 1. If not, input 1 to set the
8. 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 <property blank> 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 <property blank> 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.
When satisfied with the surface definition, click Close to return to the Abaqus
24. 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.
When satisfied with the surface definition, click Close to return to the Abaqus
20. 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-<arrow> 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.
16Click close to the Abaqus Contact Manager dialog.
免责声明：
本页面/内容部分素材来源于互联网公 开 信 息，旨在传递更多信息，不代表本平台立场。
版权归原作者或机构所有，如涉及侵权，请通过平台联系我们，我们将在核实后第一时间处理。
本平台对转载内容的真实性、准确性不作任何保证，用户需自行判断并承担使用风险。
