abaqus中实体单元的内力提取方法汇总.doc

实体单元建的模型，要提取截面的内力有什么好方法呢？我看过别人的一个帖：对于一般的实体单元结构可以定义surface 然后用section file 输出其中，这个surface可以在cae中定义，也可以在inp中定义，但是由于涉及到边的编号问题，所以在inp中容易出错。section file 的结果直接在dat中可见。需要编制小程序将其数据提取。？一定要编个程序才可以提取吗？在dat文件里没有找到什么section file是输出在*.fil文件中。要直接得到截面的total force，moment，heat flux可以在inp中添加：*SECTION PRINT,name=*,surface=*SOF,SOM在dat文件中可以找到总内力和弯矩我做钢筋混凝土的问题，模型分为两个part，分别是钢筋和混凝土，然后Assembe在一起，将钢筋embeded到混凝土内。我在keywords编辑器End assemble前定义*surface, type=cutting surface,name=surface_1-21.5,0,0,1,0,0怎么也不成，总说定义的截面没有相交(坐标计算没有错误)。第三行空着（帮助文档说表示截断整个模型）也不行，写上钢筋或混凝土的单元组名（没有另建组，直接用的keywords编辑器中钢筋或混凝土生成单元的组名）也不行。请问是怎么回事？哪位有相关的例子给我一个，我的QQ：40735053。还望不吝赐教，谢谢。Displaying a free body cutYou can define a free body cut to view the resultant forces and moments transmitted across a selected surface of a model. Force vectors are displayed with a single arrowhead and moment vectors with a double arrowhead.To create a free body cut:1. To display the entire model in the viewport, selectToolsDisplay GroupPlotAllfrom the main menu bar.2. From the main menu bar, selectToolsFree Body CutManager.3. ClickCreatein theFree Body Cut Manager.4. From the dialog box that appears, select3D element facesas theSelection methodand clickContinue.5. In theFree Body Cross-Sectiondialog box, selectSurfacesas theItemandPick from viewportas theMethod.6. In the prompt area, set the selection method toby angleand accept the default angle.7. Select the surface, highlighted inFigure 433, to define the free body cut cross-section.a. From theSelectiontoolbar, toggle off theSelect the Entity Closest to the Screentooland ensure that theSelect From All Entitiestoolis selected.b. As you move the cursor in the viewport, Abaqus/CAE highlights all of the potential selections and adds ellipsis marks (.) next to the cursor arrow to indicate an ambiguous selection. Position the cursor so that one of the faces of the desired surface is highlighted, and click to display the first surface selection.Figure 433Selected faces for the free body cross-section.c. Use theNextandPreviousbuttons to cycle through the possible selections until the appropriate vertical surface is highlighted, and clickOK.8. ClickDonein the prompt area to indicate your selection is complete. ClickOKin theFree Body Cross-Sectiondialog box.9. In theEdit Free Body Cutdialog box, accept the default settings for theSummation Pointand theComponent Resolution. ClickOKto close the dialog box.10. ClickOptionsin theFree Body Cut Manager.11. From theFree Body Plot Optionsdialog box, select theForcetab in theColor & Styletabbed page. Click the resultant color sampleto change the color of the resultant force arrow.12. Once you have selected a new color for the resultant force arrow, clickOKin theFree Body Plot Optionsdialog box and clickDismissin theFree Body Cut Manager.The free body cut is displayed in the viewport, as shown inFigure 434.Figure 434Free body cut displayed on the connecting lug.Generating tabular data reports for subsets of the modelTabular output data were generated earlier for this model using printed output requests. However, for complicated models it is convenient to write these data for selected regions of the model using Abaqus/Viewer. This is achieved using display groups in conjunction with the report generation feature. For the connecting lug problem we will generate the following tabular data reports: Stresses in the elements at the built-in end of the lug (to determine the maximum stress in the lug) Reaction forces at the built-in end of the lug (to check that the reaction forces at the constraints balance the applied loads) Vertical displacements at the bottom of the hole (to determine the deflection of the lug when the load is applied)Each of these reports will be generated using display groups whose contents are selected in the viewport. Thus, begin by creating and saving display groups for each region of interest.To create and save a display group containing the elements at the built-in end:1. In the Results Tree, double-clickDisplay Groups.2. ChooseElementsfrom theItemlist andPick from viewportas the selection method.3. Restore the option to select entities closest to the screen.4. In the prompt area, set the selection method toby angle; and click the built-in face of the lug. ClickDonewhen all the elements at the built-in face of the lug are highlighted in the viewport. In theCreate Display Groupdialog box, clickReplacefollowed bySave As. Save the display group asbuilt-in elements.To create and save a display group containing the nodes at the built-in end:1. In theCreate Display Groupdialog box, chooseNodesfrom theItemlist andPick from viewportas the selection method.2. In the prompt area, set the selection method toby angle; and click the built-in face of the lug. ClickDonewhen all the nodes on the built-in face of the lug are highlighted in the viewport. In theCreate Display Groupdialog box, clickReplacefollowed bySave As. Save the display group asbuilt-in nodes.To create and save a display group containing the nodes at the bottom of the hole:1. In theCreate Display Groupdialog box, selectAllfrom the item list, and clickReplaceto reset the active display group to include the entire model.2. In theCreate Display Groupdialog box, chooseNodesfrom theItemlist andPick from viewportas the selection method.3. In the prompt area, set the selection method toindividually; and select the nodes at the bottom of the hole in the lug, as indicated inFigure 435. ClickDonewhen all the nodes on the bottom of the hole are highlighted in the viewport. In theCreate Display Groupdialog box, clickReplacefollowed bySave As. Save the display group asnodes at hole bottom.Figure 435Nodes in display groupnodes at hole bottom.Now generate the reports.To generate field data reports:1. In the Results Tree, click mouse button 3 onbuilt-in elementsunderneath theDisplay Groupscontainer. In the menu that appears, selectPlotto make it the current display group.2. From the main menu bar, selectReportField Output.3. In theVariabletabbed page of theReport Field Outputdialog box, accept the default position labeledIntegration Point. Click the triangle next toS: Stress componentsto expand the list of available variables. From this list, selectMisesand the six individual stress components:S11,S22,S33,S12,S13, andS23.4. In theSetuptabbed page, name the reportLug.rpt. In theDataregion at the bottom of the page, toggle offColumn totals.5. ClickApply.6. In the Results Tree, click mouse button 3 onbuilt-in nodesunderneath theDisplay Groupscontainer. In the menu that appears, selectPlotto make it the current display group. (To see the nodes, toggle onShow node symbolsin theCommon Plot Optionsdialog box.)7. In theVariabletabbed page of theReport Field Outputdialog box, change the position toUnique Nodal. Toggle offS: Stress components, and selectRF1,RF2, andRF3from the list of availableRF: Reaction forcevariables.8. In theDataregion at the bottom of theSetuptabbed page, toggle onColumn totals.9. ClickApply.10. In the Results Tree, click mouse button 3 onnodes at hole bottomunderneath theDisplay Groupscontainer. In the menu that appears, selectPlotto make it the current display group.11. In theVariabletabbed page of theReport Field Outputdialog box, toggle offRF: Reaction force, and selectU2from the list of availableU: Spatial displacementvariables.12. In theDataregion at the bottom of theSetuptabbed page, toggle offColumn totals.13. ClickOK.Open the fileLug.rptin a text editor. A portion of the table of element stresses is shown below. The element data are given at the element integration points. The integration point associated with a given element is noted under the column labeledInt Pt. The bottom of the table contains information on the maximum and minimum stress values in this group of elements. The results indicate that the maximum Mises stress at the built-in end is approximately 330 MPa. Your results may differ slightly if your mesh is not identical to the one used here.*SECTION PRINTDefine print requests of accumulated quantities on user-defined surface sections.This option is used to provide tabular output of accumulated quantities associated with a user-defined section. Depending on the analysis type the output may include one or several of the following: the total force, the total moment, the total heat flux, the total current, the total mass flow, or the total pore fluid volume flux associated with the section. This option is not available for eigenfrequency extraction, eigenvalue buckling prediction, complex eigenfrequency extraction, or linear dynamics procedures.Product:Abaqus/StandardType:History dataLevel:StepReferences: “Output to the data and results files,”Section 4.1.2 of the Abaqus Analysis Users Manual “Abaqus/Standard output variable identifiers,”Section 4.2.1 of the Abaqus Analysis Users ManualRequired parameters:NAMESet this parameter equal to a label that will be used to identify the output for the section. Section names in the same input file must be unique.SURFACESet this parameter equal to the name used in the*SURFACEoption to define the surface.Optional parameters:AXESSetAXES=LOCALif output is desired in the local coordinate system. SetAXES=GLOBAL(default) to output quantities in the global coordinate system.FREQUENCYSet this parameter equal to the output frequency, in increments. The output will always be printed at the last increment of each step unlessFREQUENCY=0. The default isFREQUENCY=1. SetFREQUENCY=0 to suppress the output.UPDATESetUPDATE=NOif output is desired in the original local system of coordinates. SetUPDATE=YES(default) to output quantities in a local system of coordinates that rotates with the average rigid body motion of the surface section. This parameter is relevant only ifAXES=LOCALand theNLGEOMparameter is active in the step.Optional data lines:First line:1. Node number of the anchor point (blank if coordinates given).2. First coordinate of the anchor point (ignored if node number given).3. Second coordinate of the anchor point (ignored if node number given).4. Third coordinate of the anchor point (for three-dimensional cases only; ignored if node number given).Leave this line blank to allow Abaqus to define the anchor point.Second line:1. Node number used to specify pointainFigure 18.51(blank if coordinates given).2. First coordinate of pointa(ignored if node number given).3. Second coordinate of pointa(ignored if node number given).The remaining data items are relevant only for three-dimensional cases.4. Third coordinate of pointa(ignored if node number given).5. Node number used to specify pointb(blank if coordinates given)6. First coordinate of pointb(ignored if node number given).7. Second coordinate of pointb(ignored if node number given).8. Third coordinate of pointb(ignored if node number given).Leave this line blank to allow Abaqus to define the axes.Third line:1. Give the identifying keys for the variables to be output. The keys are defined in the “Section variables” section of“Abaqus/Standard output variable identifiers,”Section 4.2.1 of the Abaqus Analysis Users Manual.Omit both the first and second data lines forAXES=GLOBALor to allow Abaqus to define the anchor point and the axes forAXES=LOCAL. Repeat the third data line as often as necessary: each line defines a table. If this line is omitted, all appropriate variables (“Output to the data and results files,”Section 4.1.2 of the Abaqus Analysis Users Manual) will be output.Figure 18.51User-defined local coordinate system.SOFTotal force in the section.dat: yes .fil: yes .odb Field: no .odb History: no SOMTotal moment in the section.dat: yes .fil: yes .odb Field: no .odb History: no SOCFCenter of the total force in the section.dat: yes .fil: yes .odb Field: no .odb History: no 24.4 实体单元的截面力/弯矩/转角url=/forum/viewthread.php?tid=724857/forum/viewthread.php?tid=724857/url问：求助：请问abaqus里面怎样看一个构件截面（如：钢骨混凝土压弯柱）的内力啊请问：SRC柱模拟后，如何提取截面内力:如某一截面处的轴力、弯矩、剪力等内容，谢谢。答：你的 axialandsideforce1.inp中的*surface,type=cutting surface,name=halfheight500,0,0,1000,0,0改为*surface,type=cutting surface,name=halfheight60.,50.,500.,0,0,1意思是截面通过点60.,50.,500., 法向为0,0,1。分析后得到的 axialandsideforce1.dat文件中有THE FOLLOWING TABLES ARE PRINTED SOFM SOF1 SOF2 SOF3 SOMM SOM1 SOM2 SOM3 1.0002E+041.0000E+04-200.0 1.6233E-091.0052E+062.0000E+041.0000E+06 -9.9879E+04在dat文件中看到*ERROR: SURFACE ASSEMBLY_HALFHEIGHT COULD NOT BE GENERATED BECAUSE THE GIVEN DATUM PLANE DOES NOT INTERSECT THE ELEMENT SETS SPECIFIED UNDER THE *SURFACE, TYPE=CUTTING SURFACE OPTION.应该在 60.,50.,500.,0,0,1下面加一个空行，即*surface,type=cutting surface,name=halfheight60.,50.,500.,0,0,1*End Assembly见 ABAQUS Keywords Reference Manual *SURFACE：Data lines to define a surface using a plane cutting through the given element sets when the TYPE=CUTTING SURFACE parameter is used: Second line:List of elements or element set labels to be cut by the cutting plane to generate an element-based surface that is an approximation to the cutting plane. A blank data line can be specified to generate a surface by cutting the whole model.有两种方法：方法1： 在ABAQUS/cae中，菜单model / edit keywords，添加上述*surface和*section print语句，然后在ABAQUS/CAE中submit job.方法2： 手工修改inp文件，然后在WINDOWS中点击 开始 程序 ABAQUS 6.5-1 ABAQUS Command，在ABAQUS Command窗口中输入以下命令：abaqusjob=inp文件名称url=/forum/viewthread.php?tid=731075/forum/viewthread.php?tid=731075/url问：请教section print的问题用section print可以求得实体单元上的弯矩。比如我求桩上的弯矩，inp文件的命令流如下：SimWe仿真论坛 K x ?(X1j1G _*Section Print, name=xixi, surface=ding, axes=local仿真分析,有限元,模拟,计算,力学,航空,航天,ANSYS,MSC,ABAQUS,ALGOR,Adina,COMSOL,FEMLAB,Matlab,Fluent4k.H7Fd r e:s*Q¬o|S|仿真|设计|有限元|虚拟仪器 T J q g4_*blSOM, SOFSOM SOF分别代表the tatal force和the tatal moment。从帮助中可知：output variable SOM is computed with respect to the origin of the coordinate system considered.我可以求出实体单元桩上的弯矩，但是不知道abaqus 是如何求出的。是如何从应力求出截面的弯矩来的？答：应该是按照材料力学的基本原理吧：弯矩 = 总和 （各个单元的截面力 * 受力点到局部坐标轴的距离） url=/forum/viewthread.php?tid=702302/forum/viewthread.php?tid=702302/url问：进行了桩土分析计算，结果是应力与变形，不知如何反算桩身轴力和侧摩阻力？敬请各位版友赐教，谢谢！答：在本版搜索轴力。侧摩阻力： history output中有CFS（摩擦应力的合力），不知是不是你想要的。 solong答：我做桩身轴力曲线是先用 *surface，type=cuttingsurface在桩身上定义截面，然后用*section print输出这些截面上的sof（具体请参考手册）桩侧摩擦力我也是输出的整个摩擦界面的sof试一下看看。url=/forum/viewthread.php?tid=679893/forum/viewthread.php?tid=679893/url问：实体单元模拟桩，如何才能输出弯矩？还有土抗力？答：先用 *surface，type=cuttingsurface在桩身上定义截面，然后用*section print 输出这些截面上的SOF（截面力）和SOM（截面力矩）.url=/forum/viewthread.php?tid=706787/forum/viewthread.php?tid=706787/url问：我关注的模型是个环型的砼基础,里面配有环向的钢筋,混凝土用的是实体单元,钢筋用的是杆单元,现想知道杆单元沿环向的力以及实体径、环方向的力,请问大家怎么才能得到,谢谢了.答：Beam的轴力: 在step的field output中加上SF。实体的截面力: url=/forum/viewthread.php?tid=702302/forum/viewthread.php?tid=702302/urlurl=/forum/viewthread.php?tid=706985/forum/viewthread.php?tid=706985/url-本帖最后由 shclmy 于 2010-12-23 11:04 编辑 经过两个星期的摸索与学习，今天终于学会了桩轴力的输出。现总结如下，希望后来人少走些弯路。1.主要步骤是先定义截面cutting surface，然后用section print输出轴力sof。2.所有操作均是在inp文件中进行修改的，而不是ABAQUS/CAE中的编辑关键词（edit keywords）。原因：在CAE中编辑关键词是可以修改inp文件，但CAE并不能识别所有的inp文件关键词，下面将举例说明。3.最后提交的inp文件也不是在CAE中导入模型文件（import model），然后提交job进行运算的，而是在ABAQUS命令窗口（小黑屏）进行的。原因同2中的一样，CAE并不能识别关键词*section print。好了，下面开始详细的步骤讲解吧！第一步：定义截面（cutting surface），具体的关键语句为：*surface,type=cutting surface,name=cutsurf-10.6,25,0,0,1,0Set-pile解读：第一行，定义surface、surface类型以及名称。第二行，定义截面上的一点（0.6,25,0）以及截面的法向量（0,1,0）。法向量不一定是单位向量。第三行，截面所在的单元或集合。这个集合可以是事先在CAE里定义好的。需要注意的是，这个cutting surface是垂直于桩径方向的一个桩截面，而不是桩的侧表面。我一开始理解错了！此关键句在inp文件中的位置是在*Assembly, name=Assembly这一行之后，我试了下在放在材料定义之后，运算不成功。估计是因为我的Set-pile是在assembly里定义的，而不是在part里定义的单元集。若是在part里定义了桩的集合，是不是可以将此关键句移动到材料定义之后，这个我倒没试。如果是在CAE中通过编辑关键词来添加上述语句，将会有下面的错误提示：第二步：定义输出（section print），具体的关键语句为：*section print,name=secprint-1,surface=cutsurf-1sof,som解读：第一行，定义输出的名称及截面。第二行，定义输出选项，sof为截面合力，som为截面弯矩。注意，此处第一行surface=*必须是上一步中cutting surface的名称（name=*），因为要输出的就是第一步定义的截面轴力及弯矩。如果此处乱写surface=？的话，估计到最后什么也输出不了了。有些人还在第一句后面加上了axes=local,frequency=1,update=yes，由于我的模型较简单，也就没管这几个东西。除了命名之外，inp文件中的大小写英文字符，是没有区别的。所以大家不要再犹豫写*SECTION PRINT还是*section print此关键句在inp文件中的位置是最后一个* HISTORY OUTPUT: H-Output-3之后，*Output, history, variable=PRESELECT之前。也就是我的inp文件中的倒数第四和第三行。如果放错了位置，估计也会引起不识别等问题，最终导致无输出结果。如果是在CAE中通过导入inp文件来进行运算，在导入时，CAE下方窗口将会有下述警告信息：WARNING: The following keywords/parameters are not yet supported by the input file reader:-*SECTIONPRINTThe model Job-20101215 has been imported from an input file. Please scroll up to check for error and warning messages.这再次验证了，ABAQUS/CAE是不能识别关键词*section print的。强制提交job是可以运算的，但是在最后的dat结果文件里没用任何输出结果。第三步：保存并提交inp文件。在保存之前需要仔细检查上面关键语句的位置及拼写，以及是否含有中文字符。然后就可以在ABAQUS命令窗口提交inp文件进行运算了。具体操作是：开始所有程序Abaqus 6.9.1Abaqus Command输入：abaqus job=*.inp（就是你刚才修改的inp文件名）回车即可。然后黑屏窗