Femap to adina 的螺旋桨分析步骤

podocarpus 2012年12月28日 170001浏览

Direct Femap Interface in ADINA — Structural Analysis Example The ADINA User Interface (AUI) program offers comprehensive pre- and post-processing capabilities for the complete suite of ADINA Solution programs – Structures, Thermal, CFD, Electromagnetics and Multiphysics. However, other third-party pre- and post-processors can also work with the ADINA solvers and may offer certain advantages. For example, Femap contains interfaces to certain CAD packages not currently supported by the AUI, such as interfaces to ACIS, CATIA and Pro/ENGINEER (now called Creo Elements/Pro). With the direct Femap interface in ADINA, users can benefit from their familiarity with Femap and leverage the advantages of Femap in pre- and post-processing with the powerful features of the ADINA solvers. In this Brief, we demonstrate the direct Femap interface in ADINA for a propeller model that involves glueing (which allows different meshes for the glued components), contact and a preload bolt in static analysis followed by a frequency analysis. Figure 1 shows the geometry of the assembly of the propeller model with five components. The bottom of the shaft is fixed and centrifugal loading is applied to the whole model. In addition, pressure load is applied to the three blades.

Figure 1 Schematic of propeller model
As shown in Figure 2, the first glue region is between the blade and blade root and the second one is between the blade root and outer surface of the hub. Two contact regions are also defined between the bottom of the cap and the top of the hub as well as the top of the shaft and the bottom of the hub. In addition, a bolt element (not shown in Figure 2) is employed to connect the cap and the shaft with a preload.

Figure 2 Locations of contact and glue regions
We demonstrate the ease of using the direct Femap interface in ADINA with the following step-by-step analysis. Step 1: Import the geometry model into Femap and clean it up Step 2: Define the material properties and mesh with 3D solid elements

Step 3: Create bolt element and rigid elements that connect the cap and hub to the bolt element

Step 4: Apply bolt preload, body load of rotational velocity in global X direction and pressure load on the three blades

Step 5: Apply constraints at the bottom of the shaft and fix the rotation DOFs of the bolt element Step 6: Define the glueing property with default values. Create the glue regions and the corresponding connectors of glueing

Step 7: Define the contact property with "Friction Param 1=0.2". Create contact regions and the corresponding connectors of contact

Step 8: Perform the nonlinear static analysis using the direct Femap interface in ADINA Enter the Job Name and Heading (if desired) in the ADINA Analyze window, select options as shown, and run ADINA to solve the model.

Step 9: Define settings for frequency/modes analysis Set "Number of Frequency/Mode Shapes" equal to 10.

CFD前处理CAE流体力学及仿真网格建模

Femap to adina 的螺旋桨分析步骤的评论2条

发布

podocarpus 2012年12月28日

0 0

<b>Step 10: Define settings for restart analysis (to calculate frequencies)</b> Check "Restart Previous Analysis" and select "Propeller_a.res" as the file in the field "Restart Data from". <br/><div class="cae-img"><img src="http://img.jishulink.com/caenet/forums/upload/2012/12/28/385/26532270301719.jpg" title="xw-prop-step_10.jpg" alt="xw-prop-step_10.jpg"></div> <br/><b>Step 11: Perform frequency analysis using the direct Femap interface in ADINA</b> <b>Note that the analysis is performed in the deformed configuration corresponding to all loads and contact conditions.</b> Enter the Job Name and Heading (if desired) in the ADINA Analyze window, select options as shown, and run ADINA to solve the model. <br/><div class="cae-img"><img src="http://img.jishulink.com/caenet/forums/upload/2012/12/28/385/26532346809024.jpg" title="xw-prop-step_11.jpg" alt="xw-prop-step_11.jpg"></div> <br/><b>Step 12: Load the results through the Femap neutral file</b> Enter the Femap Neutral File name to load the results for post-processing. <br/><div class="cae-img"><img src="http://img.jishulink.com/caenet/forums/upload/2012/12/28/385/26531970306888.jpg" title="xw-prop-step_12.jpg" alt="xw-prop-step_12.jpg"></div> <br/>Figures 3 and 4 show results obtained from the above two analyses, visualized in Femap. The results of the frequency analysis are also shown in the movie above<br/><div class="cae-img"><img src="http://img.jishulink.com/caenet/forums/upload/2012/12/28/385/26532068708968.jpg" title="xw-prop-fig_3.jpg" alt="xw-prop-fig_3.jpg"></div> <br/><b>Figure 3</b> Band plot of von Mises stress <br/><div class="cae-img"><img src="http://img.jishulink.com/caenet/forums/upload/2012/12/28/385/26532164002452.jpg" title="xw-prop-fig_4.jpg" alt="xw-prop-fig_4.jpg"></div> <br/><b>Figure 4</b> First mode shape with band plot of total translation <br/><b>Finally</b>, users who are familiar with the AUI can also load the results into the AUI for post-processing since it provides some additional features that are not available in Femap. For example, the AUI allows the user to plot<font color="Black"> error indicators</font> as a guide for determining the accuracy of the solution and where the mesh should be refined. The entire analysis, from pre-processing to post-processing, is performed within the Femap environment using the direct Femap interface in ADINA. Users already familiar with Femap can adapt easily to analyses using ADINA, and thereby have access to more analysis options within Femap. We recognize that the <font color="Black">ADINA CAD/CAE interfaces</font> are important and also Femap with<font color="Black"> ADINA CFD</font> and FSI provides a powerful analysis tool.

回复
胡坤 2012年12月28日

0 0

femap for adina插件不好找

回复

Femap to adina 的螺旋桨分析步骤的相关视频课程

Femap to adina 的螺旋桨分析步骤的相关案例教程

ADINA常见问题解答附ADINA有限元经典实例分析下载 2022-05-24

一般问题 Q：怎样改进ADINA-AUI 中实体的显示效果？ A：在某些情况下，ADINA-AUI 显示的实体在边界上不光滑，这仅仅是显示的问题，并不影响几何尺寸的精确度。为了改进显示的效果， 1 点击Modify Mesh Plot 。 2 点击Line Depiction 。 3 将ADINA-M Chord Angle 由默认的0.4改为0.1 并且点击OK。 4 点击Surface Dep

Positive normal definition for conventional shell 2022-06-21

Positive normal definition for conventional shell elements (常规壳单元正法向定义) In finite element analysis, it is very important to determine the unit the teachings to the weak foundation of difficult to accu

Abaqus里应用Python的一些技巧附Python语言在Abaqus中的应用文档下载 2022-05-06

例如：cell4 = mdb.models['block'].parts['crankcase'].cells[4]，要把part模块中编号为4的体赋值给cell4，就需通过路径mdb→models→part→cells（4号体属性），其中'block'、'crankcase'、分别是model和part的名字。在草图Sketch中画线： s = mdb.models[' block '].Co

重型并串式液压机械臂建模与simscape仿真 2023-08-06

一、建模 Hydraulic manipulator Figure 1 shows different constituting parts of the manipulator considered, with every part labeled using numbers from 1 to 10. For each part, a CAD model is provided. Each f

DEP MeshWorks 2021强势发布！ 2022-11-30

New Functions & Enhancements 其实最重要的下面没说：无论是中面网格还是2D表面网格，3D四面体网格，网格划分速度有重大提升，平均提升50%-80%！！！ Check Volume Function This New function can automatically detect and define volumes from an FE-Model or CAD M

podocarpus

关注

影响力

粉丝

NaN

内容

获赞

项目客服

培训客服

podocarpus

关注

0 2 0