A clamped beam for an RF MEMS switch device is modeled to compute the center deflection for an applied voltage. Forces generated by the electrostatic field will bend the beam towards a ground plane.
SOLID185 brick elements model the beam. A half-width model is constructed with symmetry boundary conditions placed at the plane of symmetry. The beam is clamped at both ends. A surface interface flag (FSIN) is placed on the bottom beam surface. NLGEOM is set for geometric nonlinearities (large deflection and stress stiffening).
SOLID123 tetrahedral elements model the air underneath the beam. Fringing effects are ignored for simplicity. (Fringing effects may be considered by extending the model for the electrostatic domain beyond the boundary of the beam.) A surface interface flag (FSIN) is placed at the top of the electrostatic domain coincident with the structural beam mesh. The morphing command is activated (MORPH,on) to enable the application of structural boundary conditions at the periphery of the electrostatic domain. This is done to prepare the electrostatic domain for mesh movement (morphing) during the coupled field solution. Voltages are applied at the top and bottom surface of the electrostatic domain. A plot of the structural and electrostatic elements is shown in Figure 3. Note that the meshes are dissimilar at the interface between the domains.
The structure model is defined as field number 1; the electrostatic model is defined as field number 2 (MFELEM). Analysis options are defined for both field solutions and written to files (MFCMMAND). A static solution is defined for both fields. For the electrostatic model, 120 volts is applied with a ramped boundary condition (KBC) at 10 volt solution intervals (DELTIM). The field order for the solution is set to solve the electrostatic field first, followed by the structural field (MFORDER). The "time" is set to 120 (MFTIME) to correspond to the voltage level (for convenience) with ANSYS Multi-field solver solutions requested at 10 volt intervals (MFDTIME). Up to 20 stagger iterations are defined (MFITER). Globally conservative load transfer is prescribed (MFINTER). Forces are transferred from the electrostatic domain to the structural domain (MFSURFACE). Displacements are transferred from the structural domain to the electrostatic domain for use in morphing of the electrostatic mesh (MFSURFACE).
The total number of cumulative iterations for 12 converged ramped solutions was 153 (due to geometric nonlinearities in the structural field). Results for each field are stored in separate results files. Each field is postprocessed individually.
The command listing below demonstrates the problem input. Text prefaced by an exclamation point (!) is a comment.
/title, Electrostatic clamped beam analysis /com, ANSYS Multi-field solver /com, globally conservative Load transfer /com, Structure: SOLID185 brick elements /com, Electrostatic: SOLID123 tetrahedral elements /com, uMKSV units bl=150 ! beam length, um bh=2 ! beam height, um bw=4 ! beam width, um gap=2 ! gap, um /prep7 ! Structural model et,1,185,,3 ! 8-node bricks, simplified enhanced strain mp,ex,1,169e3 ! kg/(um)(s)^2 mp,nuxy,1,0.066 mp,dens,1,2.329e-15 ! kg/(um)^3 block,0,bl,0,bh,0,bw ! structural volume aslv lsla lsel,r,loc,x,bl/2 lesize,all,,,20,,,,1 ! 20 bricks along bl lsla lsel,r,loc,y,bh/2 lesize,all,,,2,,,,1 ! 2 bricks along bh lsla lsel,r,loc,z,bw/2 lesize,all,,,1,,,,1 ! 1 brick along bw vatt,1,,1 vmesh,all alls asel,s,loc,y,bh/2 ! clamp beam ends asel,r,loc,z,bw/2 nsla,s,1 da,all,ux da,all,uy da,all,uz alls asel,s,loc,y,bh/2 ! symmetry plane asel,r,loc,z,0 nsla,s,1 da,all,uz alls nsel,s,loc,y,0 sf,all,fsin,1 ! Define Surface interface ! Electrostatics model et,2,123 emunit,EPZRO,8.854e-6 ! pF/um mp,perx,2,1 morph,on ! enable morph bc's block,0,bl,-gap,0,0,bw ! electrostatic volume vsel,s,volu,,2 smrtsiz,2 mshape,1,3D mshkey,0 vatt,2,,2 vmesh,all aslv,s asel,r,loc,x,0 da,all,ux,0 ! Apply structural morphing constraints aslv,s asel,r,loc,x,bl da,all,ux,0 aslv,s asel,r,loc,z,0 da,all,uz,0 aslv,s asel,r,loc,z,bw da,all,uz,0 aslv,s asel,r,loc,y,-gap da,all,uy,0 aslv,s asel,r,loc,y,0 nsla,s,1 sf,all,fsin,1 ! Define Surface interface d,all,volt,120 ! Apply voltage nsel,s,loc,y,-gap d,all,volt,0 ! Apply ground potential allsel,all fini /solu mfan,on ! Activate ANSYS Multi-field solver analysis mfel,1,1 ! structure field mfel,2,2 ! electrostatic field mfor,2,1 ! Order for field solution mfco,all,1.0e-5 ! Convergence settings antyp,stat eqslv,iccg morph,on mfcm,2, ! Electrostatic field analysis options antyp,stat nlgeom,on deltim,10 ! Field loop time increment within a stagger morph,off kbc,0 ! Ramp voltage load mfcm,1 ! Structural field analysis options mfti,120 ! End time mfou,1 ! Write solution every time step mfdt,10 ! Stagger time increment mfit,20 ! Max staggers mfint,cons ! globally conservative load transfer mfsu,1,2,forc,1 ! Transfer forces to structure field mfsu,1,1,disp,2 ! Transfer displacements to electrostatic field solve ! Solve the ANSYS Multi-field solver problem save finish /post1 file,field2,rth ! Select Electrostatic Field results file set,last esel,s,type,,2 ! Select electrostatic elements plns,ef,sum ! Plot electrostatic field fini /post1 file,field1,rst ! Select Structural Field results file set,last esel,s,type,,1 ! Select structural elements nsle,s plns,u,y ! Plot displacement prdisp finish /post26 ! Time-histroy postprocessor file,field1,rst ! Retrieve Structural Field results file n1=node(75,0,0) ! get node at mid-plane nsol,2,n1,u,y ! store UY displacement vs. voltage /axlab,y,UY ! Displacement /axlab,x,Voltage ! Time = voltage prvar,2 ! print displacement vs. voltage plvar,2 ! plot displacement vs. voltage fini