XANSYS Message #: 46857

XANSYS Message: 46857 [Go back to message list]
[bookmark on del.icio.us]
No rating yet

Subject: Re: Substructuring-Contact analysis
Author: Joe Metrisin
Date: 2003-02-17 11:13:00

Amar, Attached is a macro I wrote years ago which automates the procedure you are trying to do. Just build the complete model with contact elements included, and create the component names as described in the macro header. The macro puts all the linear elements into a superelement and iterates on the contact elements only. When I wrote this macro, it turned out to be not very useful because the superelement generation pass required the frontal solver which was extremely slow, and negated any advantage of solving the entire model using the sparse or iterative solver. The later versions of ANSYS can now generate superelements with the sparse solver, so it may or may not be beneficial now. One other thing not related to superelements. You mentioned you have a 1 micron clearance between the parts. I don't know the relative scale of your model, but if that initial gap is greater than the pinball radius of the contact elements, you could have rigid body motion on the first iteration. If that occurs, try bringing the two parts into contact with enforced displacements to establish contact before applying the real loading condition. Joseph T. Metrisin Florida Turbine Technologies /com /com Macro to efficiently solve an ANSYS 5 model with gap elements. /com Solution is performed by creating a superelement containing the /com linear portion of the model, then iterating on the nonlinear portion /com in the use pass. This macro performs the superelement generation /com pass, use pass, and expansion pass. /com /com User must predefine components called GAPELEM, and GAPNODES which /com contain all the gap elements, and all the nodes connected to gap /com elements, respectively. /com /com ***Note: MASS MATRIX IS GENERATED! If you do not need the mass matrix, /com change seopt,linear_,2 to seopt,linear_,1. This should speed up your /com analysis. /com /com The linear results are stored in: linear_.db, linear_.rst /com The nonlinear results are stored in: nonlin_.db, nonlin_.rst /com /com Written by: Joe Metrisin /com Date: October 21, 1994. /com /com Revision 1: 11/13/95: Changed default to generate mass matrix. /com /com /com ********************** GENERATION PASS ********************* finish /filnam,linear_ ! Define superelement matrix file name. /solu ! Enter solver. antype,substr ! Select superelement analysis type. cmsel,s,gapnodes ! Select nodes involving nonlinearities. m,all,all ! Set these nodes as master DOF's. cmsel,u,gapelem ! Unselect nonlinear portion (gap elements). seopt,linear_,2 ! Options to generate stiffness matrix only. nsel,all ! Restore all nodes. save,linear_,db ! Save superelement (linear model) database. solve ! Generate superelement matrix. /com /com ********************** USE PASS ********************* fini /clear ! Clear database. /filnam,nonlin_ ! Define use pass job name (nonlinear model). /prep7 ! Enter preprocesser. resu,linear_,db ! Resume superelement database. et,500,matrix50 ! Define superelement element type. type,500 ! Set active element type. se,linear_ ! Define superelement. esel,s,type,,500 ! Select superelement. *get,senum,elem,,num,max ! Retrieve element number of superelement. cmsel,s,gapnodes ! Select nonlinear nodes. cmsel,a,gapelem ! Add nonlinear elements. save ! Save nonlinear model database. finish ! Exit preprocessor. /solu ! Enter solver. antype,static ! Select static analysis. sfe,senum,1,selv,,1.0 ! Apply superelement load vector previously generated. solve ! Solve the nonlinear model. finish /com ********************** EXPANSION PASS ********************* /com /clear ! Clear database. /filnam,linear_ ! Switch file name to linear model. resume ! Resume linear model database. /solu ! Enter solver. expass,on ! Select expanansion pass. seexp,linear_,nonlin_ ! Expand linear model w/results from nonlinear run. expsol,1,1 ! Select loadstep 1, substep 1. solve ! Perform expansion. /com Hello I am doing a 2D contact analysis of a rack driving a gear which is constrained to rotate on a hub. There is a clearance of 1 micron between the gear and hub.The hub is fixed. Displacement is applied to the rack. There is no constraint on the gear. So contact is between the gear teeth and rack and gear and hub.this is with PLANE 42 . Educational version. I am trying this by substructuring. I made the gear a superelement with MDOFs where contact occurs. Now in the Use pass ( the manual isnt quite clear on this) i create the rack and hub ( non-superele). To create the contact elements do i create the gear again and create contact elements and then read in the superelement file? or do i read in the superelement file and create the contact elements at the MDOfs? I am not exactly clear as to how to create the non-superele contact elements? also is substructuring really useful? the manual gives just one example on it. Please advise. Amar Atre student Rochester Inst of Tech Rochester NY 14623 apa5040@r...

Posts possibly associated with message #46857		Author	Date
`46846`	`Substructuring-Contact analysis`	`Amar Atre`	`2003/02/17`
`46857`	`Re: Substructuring-Contact analysis`	`Joe Metrisin`	`2003/02/17`
`46881`	`Re: Substructuring-Contact analysis`	`Riccardo Testi`	`2003/02/18`
`46966`	`Re: Substructuring-Contact analysis`	`Dan Bohlen`	`2003/02/19`