ansys模拟钢管混凝土的极限承载能力

...wd......wd......wd...薄壁钢管混凝土柱轴心受压性能的实例分析建设的单元类型都为solid45号单元，因为计算较为简单的缘故。构件参数d=200，t=5，l=840，fy=265.8e6，fc=27.15e6，ec=21700e6，es=210000e6。一、建设钢管混凝土实体模型并对此模型进展网格划分钢管混凝土单元单元二、材料应力应变关系的定义钢管应力应变关系混凝土材料的应力应变关系〔采用随动硬化模型〕三、施加位移约束和荷载ANSYS加载方式有两种：一种是位移加载，一种是力加载。本文采用的是位移加载方式，采用力加载法在接近应力峰值时会遇到很大的收敛问题，而采用位移加载法比拟容易收敛，且得等到的荷载—位移曲线较好在底部施加固定端约束，同时在顶面施加在面方向的移动，UX、UZ，在顶面的所用节点进展耦合，使其在沿着柱的方向上有一样的位移。然后是施加位移，在顶面所有节点施加位移荷载，UY=0.003大概是这么多。四、求解定义完求解步之后，设置分析选项后，就可进展有限元的计算。五、检查结果钢管的冯米泽斯应力整体的冯米泽斯应力节点位移图六、荷载—应变全程曲线计算节点力的时候是通过顶面节点Y方向节点力求和操作来求解。!钢管与混凝土完全粘接情况下的抗压承载性能，使用面荷载加载方式。fini/clear/prep7wprota,,90,csys,4d=0.2l=0.840t=0.005n=d/tfy=265.8e6fc=27.15e6ec=21700e6es=210000e6p=2000e3!混凝土单元及材料参数et,1,45mp,ex,1,ecmp,prxy,1,0.2tb,kinh,1,,13!混凝土选用的是hongnestad模型tbpt,,0.001,2.17e+07tbpt,,0.0011,2.30e+07tbpt,,0.0012,2.41e+07tbpt,,0.0013,2.50e+07tbpt,,0.0014,2.58e+07tbpt,,0.0015,2.64e+07tbpt,,0.00154,2.66e+07tbpt,,0.00154,2.66e+07tbpt,,0.00176,2.72e+07tbpt,,0.002,2.66e+07tbpt,,0.00246,2.50e+07tbpt,,0.00292,2.34e+07tbpt,,0.00338,2.18e+07!钢管单元及材料参数et,2,solid45mp,ex,2,2.1e11mp,prxy,2,0.3tb,biso,2,1,2tbtemp,0tbdata,,fy,0cyl4,,,(d-2*t)/2,,,,-lcyl4,,,d/2,,(d-2*t)/2,,-lvglue,allcsys,0wpstyl,defawpstyle,,,,,,,,0!划分网格mat,1type,1vsweep,1mat,2type,2vsweep,3!施加约束条件asel,s,loc,y,0da,all,allallsel,allasel,s,loc,y,lnsla,s,1cp,1,uy,allsfa,all,1,pres,-p/(3.14*(d*d)/4)allsel,allfinish!进入求解层、设置求解选项/soluautots,onnsubst,64outres,all,allsolvefini!进入post1后处理*get,rtime,active,0,set,time!进入post26,绘制荷载-位移曲线〔节点的竖向应变与荷载曲线〕/post26nsol,2,71,u,yprod,3,2,,,,,,1/lprod,4,1,,,,,,p/1e3/axlab