ANSYS荷载工况组合计算实例•1相关命令• 1.1 LCDEF• 1.2LCFACT• 1.3SUMTYPE• 1.4LCOPER• 1.5LCASE1• 1.6LCWRITE• 1.7其他命令•2实例在实际工程计算中，往往需要分析多种不同荷载组合总用下的结构响应，比如恒载、活荷载、风荷载等的组合，有些是荷载位置不同，有些则是荷载大小差异。
ANSYS做不同荷载工况组合分析，要么是每一种工况用单独的APDL进行运算，每个工况一套文件；要么就是利用分析结果，在一个计算文件中，用不同的荷载步定义荷载组合，再用工况组合功能来实现我们的分析目标。
下面总结一下实现荷载工况组合的方法1.相关命令1.1. LCDEFLCDEF, LCNO, LSTEP, SBSTEP, KIMG 从结果文件中创建一个工况其中常用参数为：LCNO工况编号，是1~99之间的一个数字，作为指针，将工况与计算文件中的荷载步和荷载子步联系起来LSTEP用于定义工况的荷载步SBSTEP用于定义工况的荷载子步，默认为荷载步的最后一个子步KIMG用于复数分析，0-用实部；1-用虚部1.2.LCFACTLCFACT, LCNO, FACT 定义工况的分项系数其中，Lcno为工况编号，fact为分项系数1.3.SUMTYPESUMTYPE, Label 为工况组合设置数据组合类型Lable参数有两个选项，分别为•COMP—Combine element component stresses only. Stresses such as average nodal stresses, principal stresses, equivalent stresses, and stress intensities are derived from the combined element component stresses. Default. 此选项为只将单元应力进行组合，节点平均应力、主应力、等效应力等则从组合后的单元应力中求解(不知道这样理解是否合适呢。
) •PRIN—Combine principal stress, equivalent stress, and stress intensity directly as stored on the results file. Component stresses are not available with this option.对主应力、等效应力、应力强度等直接根据结果文件进行组合。
所以平时在计算主应力等结果时候多用次选项。
1.4.LCOPERLCOPER, Oper, LCASE1, Oper2, LCASE2 对荷载工况进行操作Oper•ZERO—Zero results portion of database (LCASE1 ignored).结果数据库中为零的部分？•SQUA—Square database values (LCASE1 ignored).数据结果取平方•SQRT—Square root of database (absolute) values (LCASE1 ignored).结果数据开平方根•LPRIN—Recalculate line element principal stresses (LCASE1 ignored). Stresses are as shown for the NMISC items of the ETABLE command for the specific line element type.计算线性主应力•ADD—Add LCASE1 to database values.将工况1增加到求解数据库中•SUB—Subtract LCASE1 from database values.将工况1从求解数据库中删除•SRSS—Square root of the sum of the squares of database and LCASE1.将求解数据库和工况1之和进行开平方•MIN—Compare and save in database the algebraic minimum of database and LCASE1.将数据库和工况1中的代数比较小者存入现有数据库•MAX—Compare and save in database the algebraic maximum of database and LCASE1.将数据库和工况1中的代数较大者存入现有数据库•ABMN—Compare and save in database the absolute minimum of database and LCASE1 (based on magnitudes, then apply the corresponding sign).将数据库和工况1中绝对值较小者存入现有数据库•ABMX—Compare and save in database the absolute maximum of database and LCASE1 (based on magnitudes, then apply the corresponding sign).将数据库和工况1中绝对值较大者存入现有数据库1.5.LCASE1First load case in the operation (if any). See LCNO of the LCDEF command. If ALL, repeat operations using all selected load cases .工况运算的第一个工况，由LCDEF命令指定，如果为all，则对所有已选择的工况重复命令。
Oper2MULT—乘法运算: LCASE1*LCASE2CPXMAX—此选项用于复数运算，将工况1作为实部，工况2作为虚部。
This option does a phase angle sweep to calculate the maximum of derived stresses and equivalent strain for a complex solution where LCASE1 is the real part and LCASE2 is the imaginary part. The Oper field is not applicable with this option. Also, the LCABS and SUMTYPE commands have no effect on this option. The value of S3 will be a minimum. This option does not apply to derived displacement amplitude (USUM). Load case writing (LCWRITE) is not supported. See POST1and POST26 – Complex Results Postprocessing in the Mechanical APDL Theory Reference for more information.LCASE2Second load case. Used only with Oper2 operations.1.6.LCWRITELCWRITE, LCNO, Fname, Ext, —创建工况文件其中lcno为工况编号，fname和ext分别为工况文件名称和后缀名1.7.其他命令•lCDEF,ERASE来删除所有的荷载工况指针和所有的荷载工况文件•LCDEF,LCNO,ERASE删除指定的荷载工况指针LCNO（和相应的文件）。
•LCDEF,STAT查看所有选定的荷载工况(LCSEL)的状态•LCDEF,STAT ,ALL查看所有荷载工况的状态•LCSEL, Type, LCMIN, LCMAX, LCINC 选择指定编号的工况2.实例首先要说明，这个悬臂梁实例本身没有任何工程意义，只是用来熟悉一下相关操作而已。
为了便于理解，实例中只有两个荷载工况，分别为向上的集中力和向下的均布荷载，实际情况可能比实例中更复杂，就需要具体问题具体分析了。
/悬臂梁简单模型finish/clear/prep7et,1,188mp,ex,1,2.1e5mp,prxy,1,0.3sectype,1,beam,I,,0secdata,0.5,0.5,0.7,0.05,0.05,0.05k,1,k,2,10k,3,,20l,1,2latt,1,1,1,,3,,1lesize,all,1lmesh,all/solud,1,allf,2,fy,100lswrite,1fdele,all,allsfbeam,all,,pres,200,200 lswrite,2allsel,alloutpr,all,alllssolve,1,2,1 !对各荷载独立求解finish/post1/eshape,1plnsol,s,1对上述命令流进行改进，设置荷载组合：finish/clear/prep7et,1,188mp,ex,1,2.1e5mp,prxy,1,0.3sectype,1,beam,I,,0secdata,0.5,0.5,0.7,0.05,0.05,0.05k,1,k,2,10k,3,,20l,1,2latt,1,1,1,,3,,1lesize,all,1lmesh,all/solud,1,allf,2,fy,100lswrite,1fdele,all,allsfbeam,all,,pres,200,200lswrite,2allsel,alloutpr,all,alllssolve,1,2,1 !对各荷载独立求解finish/post1/eshape,1!plnsol,s,1/post1lcdef,1,1 !设定工况1=荷载步1，工况2=荷载步2lcdef,2,2!给两个工况设置不同的分项系数lcfact,1,1.2lcfact,2,1.4lcase,1 !读入工况1，database＝1sumtype,prin !指定加操作的类型lcoper,add,2 !荷载组合，database＝database＋2lcoper,lprin !计算线性主应力lcwrite,11 !把database结果写到工况11,即1.2倍竖向力+1.4倍均布荷载lcase,1 !还可以重新读入工况1，database＝1lcfact,1,2!重新定义分项系数lcfact,2,1.5sumtype,prinlcoper,add,2 !荷载组合，database＝database＋2lcoper,lprin !计算线性主应力lcwrite,12 !把database结果写到工况11,即2倍竖向力+1.5倍均布荷载lcase,1!载入工况1plnsol,s,1 !查看该工况下的结构响应荷载工况1的SX计算结果荷载工况2的SX计算结果ansys荷载工况组合若用ANSYS进行设计，往往要计算很多种工况组合，如果加载能分开加载独立计算然后结果叠加（仅限于弹性阶段）则效率可提高不少，下面推荐几个命令即可达到这种效果。