当前位置:首页 >> 机械/仪表 >>

abaqus与hypermesh接口教程


Lab 2 Finite Element Analysis of a Cantilever Beam
y

P = 40000 lb.

12 in. x 96 in

PROBLEM STATEMENT Consider a 96 in. x 12 in. cantilever beam as shown i

n the above figure. The beam is loaded at the right end by a force P = 40000 lb. The beam is isotropic with Young’s modulus E = 3x107 psi and Poisson’s ratio ν = 0.3. Using Hypermesh and ABAQUS, perform the analysis outlined below. Start out by creating a relatively coarse mesh of 4-node quadrilateral elements (try a mesh of rectangular elements with 6 divisions in the x direction and 2 divisions in the y direction). Apply the appropriate boundary conditions, and run the problem assuming plane stress.

Instructions for Lab#2 Using Hypermesh and ABAQUS for the analysis of a beam in bending.

Figure 1. Main Window in Hypermesh. Circled is the command toolbar that allows the user to access sub menus. Getting Acquainted 1) Fire up Hypermesh from the menu controls. 2) Familiarize yourself with the command toolbar to your right. By clicking next to each title as circled above, you will be brought to several sub-menus where you may perform a variety of tasks. Click on each and analyze each sub-menu. 3) Identify commands that appear self-explanatory, such as file, automesh, nodes, lines, ect.... 4) Notice that the file command exists in every toolbar. 5) Click on the file command. This is where you name the hypermesh files you would like to save using a *.hm extension. Also, this is where importing and exporting occurs. 6) Also notice the template command. This is where the solvers are invoked. Hypermesh has the capability of exporting mesh information for a variety of solvers. Keep in mind, Hypermesh is purely a mesh generator and the mesh information must be translated into the format of the desired solver to be used, therefore picking the correct solver from the template is a necessary step before continuing with any other steps

Geometry In this exercise we will generate the geometry of a beam to be deformed by applying a tip point load and by fixing one end. After completion of the geometry generation, a 3-dimensional mesh of the beam will be created and a stress analysis on the beam will be performed. 1) Like all mesh generators, in order to create a mesh, some geometry must exist. Generally nodes are required from which lines are created. Surfaces must be created from a set of lines that form a closed loop. It is those surfaces that will be meshed. 2) Click on the “Geom” icon to your right and notice the various menus. In particular, notice the “nodes” icon. Clicking on that will allow to create several nodes in a variety of modes. For example, by co-ordinates (most popular one), on lines, ect.. 3) Once the nodes exist, one can create lines from those nodes by clicking on the “line” button. Note the options available for the different type of lines that can be created. Go ahead and create lines from the existing nodes. 4) With the lines created, surfaces can be generated by clicking on the “surface edit” button and by selecting the filler surface option. Create a surface using all existing lines. 5) At this point the geometry has been created and mesh generation should be the next step. Mesh generation In this phase of the exercise the geometry created above will be meshed. The first step will be to mesh the two-dimensional surface with 2-D elements. Two meshes will be generated, a biased mesh and regular mesh. Samples can be seen in the figures below. When that is done, the two meshes will be extruded to create the threedimensional brick element meshes.

Figure 2. A simple quad mesh with no biasing.

Figure 3. A biased quad mesh focused toward one end.

Creating a 2-D mesh. 1) With all surfaces created, it is time to mesh. 2) Prior to creating elements, the concept of “collectors” must be reviewed. Hypermesh has the ability to store groups of elements under different names called collectors. In this manner, it is possible to modify parts of a mesh on a group basis. We will practice using these collectors to store the two meshes that will be generated for the same part. In one collector we will store the elements for the mesh in figure 2 and in another collector we will store the mesh for figure 3. To create collectors, click on the “collectors” button and create the two collectors using two different names and two different colors. 3) You can toggle between the two collectors by using the “global button” in the right hand bottom corner and selecting the collector you wish to work in. It is important that you know which collector is being used as default and changing it will be necessary as the meshing progresses. Further you may display the desired collectors by using the “display” command in the bottom right corner and by clicking and un-clicking on each collector that is available. With that done we may proceed to create the two meshes. 4) Make sure you know which collector is currently set to default. To begin meshing, click on the 2D toolbar to your right. 5) There are a variety of options available. We will use the automesh option. 6) By clicking on automesh, several parameters are required as well as the necessity to select the surfaces one wants to mesh. 7) Select the surface by clicking on each and supply a rough idea of the element size and element type you would like to use. Also make sure you are in the interactive mode. 8) Once that is done, clicking the mesh button will generate a tentative idea of how your mesh will look along the geometry borders. You may enhance your mesh by improving on the coarseness, adding bias, ect... By clicking on the number of divisions for each line you may increase that value using the left button or decrease that value using the right button. Similar things can be done if one wants to change the bias or other parameters. 9) With that done, clicking on the mesh button will create the mesh. Accept the mesh by clicking return or reject it by clicking reject. 10) The above steps must be repeated to create a biased mesh toward the fixed location. To do that repeat steps 3-8, but ensuring yourself that you are in the appropriate collector. Also, when the tentative divisions on the border of your surface appear, you can add bias by clicking on the bias button and giving positive or negative bias values. Note: Your part may consist of several surfaces and you may mesh them all at once or separately. You may also allocate each meshed portion to different collectors, so as to be able to have control over your model based on the different portions meshed.

Creating a 3-D mesh. 1) The next step involves extruding the mesh from its 2-D version, thus creating a 3-D mesh. 2) The first step is two create two additional collectors into which the two 3-D meshes will be saved. 3) With that done, click on the “3D” button and click on the drag button. 4) The drag button allows the user to drag a set of 2-dimensional elements into 3dimensional elements so long that a drag direction and distance are supplied, as well as the intended number of divisions to be created on the way. 5) Select the elements to be dragged by component and define a drag direction and distance. Supply the intended number of divisions. With that done, click on the drag button. Your 3-dimensional mesh will be created within the chosen collector. 6) Do the same for the second 2-dimensional mesh and ensure that it is put in the appropriate collector. 7) With that done, it will be necessary to delete the unnecessary 2-dimensional meshes. To do so press the F2 key and delete elements by component and select the two components to be deleted. Click on “delete” to approve deletion of the two selected components. Boundary conditions Once the mesh has been created, it is necessary to create the required boundary conditions. Boundary conditions can be created within Hypermesh for use in ABAQUS, however the complexity of the steps within Hypermesh, outweighs the ease of typing in boundary conditions within the ABAQUS file, provided that the appropriate node sets and element sets are available. This is what will be done in the next steps. 1) We need two sets. A node sets for those nodes that will be fixed and a node set for those nodes onto which the load will be applied. 2) To do so, click on the BCs menu. There you will create entity sets. Entity sets is simply a manner to groups nodes or elements under one common name. In ABAQUS, boundary conditions can be applied to those sets. 3) Click on entity sets and create a node set called “fixed”. Select the nodes on the left end of the beam by using the window select. When done click on create. If the set is created, click on RESET. 4) Change the name to “load” and select the nodes onto which the load will be applied and click on create. 5) This will be it! With the mesh completed you may now export your file using the ABAQUS template and saving the file under a *.inp extension. You can do this by clicking on file and then selecting the export command. MAKE SURE YOU ARE USING THE “ABAQUS STANDARD” TEMPLATE. Be careful here!

NOTE: Remember you have two meshes on top of each other. Before you export each mesh as *.inp file, you must create to separate Hypermesh files. In each file save only the mesh you desire. This is done by deleting the unwanted mesh and saving under a different name. Deleting elements or nodes is accomplished using the F2 command. It is also a good idea to go ahead and renumber your mesh when you are ready to finalize it. Renumbering is accomplished by clicking on the tools icon and then clicking on the renumber button. Do this for each mesh. Now we are ready for ABAQUS.

IN ABAQUS The general ABAQUS file follows your typical format for any FEA solver. It contains nodal information and connectivity as well as element type information. At the end are the boundary conditions and the solution procedure. This can be observed below. Open the *.inp file that was created. It should look as follows: ** ** ABAQUS Input Deck Generated by HyperMesh Version3.0 ** ** Template: ABAQUS/STANDARD ** *** THIS IS THE NODAL INFORMATION *NODE 1, 0.0 , 2.221825 , -7.778174 : : : : : : : : : 9843, 6.7033386359838, 3.648821000031 , 0.0539689803571 *** THIS IS THE ELEMENT INFORMATION. C3D8= 8 noded brick element. *ELEMENT,TYPE=C3D8,ELSET= threeD 1, 1858, 1857, 1878, 1879, …………. : : : : : : : : : 8470, 478, 522, 9807, 9774, ………. ** SECTION DEFINITION: assign material and thickness if necessary for shells. *SOLID SECTION, ELSET= threeD, MATERIAL= ALUMINUM

*** HERE ARE THE ENTITY SETS TO BE USED FOR THE B.C.’s

*NSET, NSET= 1, 2, 9, 10, *NSET, NSET= 448, 449,

fixed 3, 4, 5, 6, 7, 8, 11, 12, 13, 14, 15, 16, load 450, 451, 452, 453, 454, 455,

**** MATERIAL PROPERTIES *MATERIAL, NAME= MAT1 *ELASTIC, TYPE = ISOTROPIC 10000000.0,0.22,0.0 ********THIS IS WHAT YOU ADD MANUALLY LOAD STEP INFORMATION, BOUNDARY CONDITION INFORMATION, AND OUTPUT INFORMATION.***** *STEP *STATIC --- TYPE OF ANALYSYS *CLOAD --- TYPE OF LOAD load,1,-1.0 *BOUNDARY --- TYPE OF DISPLACEMENT BC fixed,1,3,0.0 *EL FILE --- ELEMENT OUTPUT TO BE VIEWED IN HYPERMESH SINV *NODE FILE --- NODAL OUTPUT TO BE VIEWED IN HYPERMESH U *EL PRINT, ELSET=threeD --- ELEMENT OUTPUT TO BE LISTED IN DATA FILE S11,S22,S33,S12,S13,S23 E11,E22,E33,E12,E13,E23 *NODE PRINT, NSET=fixed --- NODAL OUTPUT TO BE LISTED IN DATA FILE U,RF *END STEP With this in mind, you should modify your file to include necessary analysis information and boundary conditions. When that is done, you can run your two ABAQUS files

VIEWING THE RESULTS IN HYPERMESH. Once the ABAQUS run is complete, you need to convert the *.fil into a hypermesh *.res file. Do this by using the hmabaqus command within your unix template. Now open Hypermesh. 1) Retrieve one of the models and click on the global button. 2) You will see a path for the results file. Enter the filename assigned above. 3) Exit this menu and click on the POST icon and view your results by using the contour button.

Some contour plots of a beam in bending. You may create displacement contours, stress contours, ect…

Figure 4. The displacement contour plot for a beam in bending.

Figure 5. Von-Mises Stress Contour for a beam in bending.

General Tips: 1) When meshing a model in separate portions it is necessary to create a collector for each portion and making sure one has selected the correct collector before meshing a surface so that those elements created are fed into the desired collector 2) Also, one must always check for duplicate elements or nodes. This can be done with appropriate commands in the tools toolbar available at your right. We will explore these commands in class.


相关文章:
ABAQUS与Hypermesh接口流程(原创)
ABAQUS与Hypermesh接口流程(原创)_计算机软件及应用_IT/计算机_专业资料。原创总结...hypermesh-abaqus论坛常... 6页 免费 hypermesh-abaqus教程 40页 1下载券 hyperm...
ABAQUS与Hypermesh接口教程
ABAQUS与Hypermesh接口教程_计算机软件及应用_IT/计算机_专业资料。ABAQUS与Hypermesh接口教程 ABAQUS 与 Hypermesh 接口教程本文分两种情况。第一种:在 HM中对几何模型...
hypermesh与abaqus接口连接经典实例
hypermesh与abaqus接口连接经典实例_机械/仪表_工程科技_专业资料。hypermesh与abaqus...接下来的教程用来指导接触对的创建过程。 3.  在 ABAQUS Contact ...
hypermesh与abaqus接口问题
(教程皆来源于 SIMWE 论坛) hg_boy 的 hypermesh_to_abaqus 接口视频教程,在 FTP 中有下载,刚出来的,版本较新,适合 abaqus 大家学习。 (教程不要做多,选...
Altair HyperMesh与Abaqus Explicit接口实例
Altair HyperMeshAbaqus Explicit 接口实例 本实例版权属本人所有,可供在任何免费网站或论坛传播。 本教程的目的在于帮助 Abaqus 用户更方便地利用 HyperMesh 的强...
hypermesh与ansys接口连接经典实例
hypermesh与ansys联合仿... hypermesh与abaqus接口连...1/2 相关文档推荐 ...(Real Constans);在 Hypermesh ” Manager 中也称为“实常数(Real Constans)。...
hypermesh导入abaqus问题集(绝对原创——总结各种情况)
hypermesh导入abaqus问题集(绝对原创——总结各种情况)_工学_高等教育_教育专区。绝对原创,解决abaqus与hypermesh接口 Hypermesh to abaqus surface 研究 两个 PART ...
hypermesh-abaqus论坛常见问题汇总
hypermesh-abaqus论坛常见问题汇总_机械/仪表_工程科技_专业资料。hypermesh-abaqus论坛常见问题汇总 HM———ABA 接口问题 接口问题 ——简洁一些,引用小宝斑竹在接口...
联合Hypermesh与abaqus分析发动机橡胶悬置垫过程2
hypermesh-abaqus教程 40页 2财富值 Hypermesh与abaqus接口实例... 15页 10财富...联合Hypermesh与abaqus分析发动机橡胶悬置垫过程2联合Hypermesh与abaqus分析发动机橡胶...
如果你觉得Abaqus前处理功能不强,你可以学习HyperMesh进阶提高
hypermesh-abaqus 2页 1下载券 hypermesh-abaqus教程 40页 1下载券 hypermesh and Abaqus 21页 1下载券 Hypermesh与abaqus接口实... 15页 4下载券 hypermesh与ab...
更多相关标签:
hypermesh abaqus | hypermesh导入abaqus | hypermesh abaqus实例 | hypermesh与abaqus | hypermesh和abaqus | hypermesh abaqus pdf | hypermesh abaqus视频 | abaqus hypermesh焊缝 |