1. 9.0 New Features Large Deformation Analysis of thin plate assembly spotwelded together Workshop 2 Spotwelds

2. 9.0 New Features Workshop ANSYS v9.0 © 2004 ANSYS, Inc. October 1, 2004 Inventory #002157 WS2-2 Goal Build spotwelded assembly, run and post process a large deflection analysis. Model Description 3D model of three plates spot welded together. – 12 Degree sector with two symmetry planes – Three Plates meshed with SHELL181 Spot weld 12 deg sector 0.50 dia Spot weld 0.15 0.10 Typ Spot weld 12.9 R 14.00 R 15.00 R 4.00 Displacement Fixed

3. 9.0 New Features Workshop ANSYS v9.0 © 2004 ANSYS, Inc. October 1, 2004 Inventory #002157 WS2-3 Steps to Follow: Start an ANSYS interactive session and open (or read in) the input file named “spotweld.inp”. You might need to set your “Files of type: = (*.*) Use the GUI menu method: Select the Open ANSYS File ICON… Select the file “ spotweld.inp ” Click OK Or Command Input Method /INPUT, spotweld.inp Note: This file consists of APDL input which will automatically erase any currently active database and change the jobname to “spotweld”. It will then generate the geometry, define the materials and apply boundary conditions and loads to begin the current exercise. … Spot weld

4. 9.0 New Features Workshop ANSYS v9.0 © 2004 ANSYS, Inc. October 1, 2004 Inventory #002157 WS2-4 Review the Model: Before proceeding, become familiar with the geometry, mesh, element type, material, BCs and load specifications for this model. It remains to join the three parts together at areas 7, 2 and 12, with a 0.50 inch diameter spot weld using the prescribed hard point location illustrated in figure to the right as the starting point. Note: One hard point (keypoint #33) has already been created at the location defining the centerline of the spot weld. This hard point is associated with the top plate (area# 7). The node (#393 in 9.0) associated with this hard point has been parameterized with the name “SW_NODE” for convenience. Confirm this by listing parameters with *STAT. Hard point for starting location of spot weld … Spot weld

5. 9.0 New Features Workshop ANSYS v9.0 © 2004 ANSYS, Inc. October 1, 2004 Inventory #002157 WS2-5 Create Spot Weld Enter the Preprocessor and create the spot weld between first two plates. Main Menu > Preprocessor > Modeling > Create > Elements >SpotWeld > Create New Set > By Area… Pick or enter area “7” and then area“2” as the first two areas to be welded. Pick or Enter node to spot weld “SW_NODE:” Note: The order in which the area numbers are entered will effect the way the spot weld is created. Recall area #7 already has a node (SW_NODE) defined at the desired start location of the spot weld. For this reason, area #7 needs to be entered first. If the areas are entered in reverse order (2, 7), then the student will receive the following warning: With the area entry (2,7), ANSYS will associate node #393 with area #2 and create a second node on area #7 which is coincident with node 393. Hence, the warning message. … Spot weld

6. 9.0 New Features Workshop ANSYS v9.0 © 2004 ANSYS, Inc. October 1, 2004 Inventory #002157 WS2-6 … Spot weld Create Spot Weld (cont’d) Enter Element Component Name “sweld1” Enter SpotWeld radius “0.50” [OK] Note: ANSYS has now created a contact pair for the two surfaces. (areas 7 and 2). Each contact pair contains one node-to-surf contact element (CONTA175) defined at the spot weld node associated with area 7 (#393) and a newly created node associated with area #2. This new node was located by a normal projection at node 393 from area 7 onto area 2. Target elements were overlaid fully or partially on each surface. Only the surface nodes that fall within a sphere of radius, called a search radius, with its center at the original position of the corresponding spot weld node are used to form target elements. The search radius can be user defined but must be larger then the spot weld radius. The default search radius is four times the spot weld radius. For each spot weld surface, ANSYS will build 6 force distributed constraint equations through a contact pair. The spot weld radius determines the influence range of the constraint equations. Each spot weld node couples with a group of nodes on the corresponding surface within the radius. The spot weld nodes associated with each surface are tied together with rigid MPC184 elements. Refer to ANSYS output for a summary of elements created

7. 9.0 New Features Workshop ANSYS v9.0 © 2004 ANSYS, Inc. October 1, 2004 Inventory #002157 WS2-7 … Spot weld Add third surface to spot weld Main Menu > Preprocessor > Modeling > Create > Elements >SpotWeld > Add more Surfaces > By Areas… Pick or enter area “12”. [OK] Note: A maximum of 11 surfaces can be included in one spot weld assembly

8. 9.0 New Features Workshop ANSYS v9.0 © 2004 ANSYS, Inc. October 1, 2004 Inventory #002157 WS2-8 … Spot weld Review the newly created spot weld specifications Main Menu > Preprocessor > Modeling > Create > Elements >SpotWeld > List … You can also enter the contact manager to review the contact pairs created for each surface and/or to plot the pairs altogether or individually.

9. 9.0 New Features Workshop ANSYS v9.0 © 2004 ANSYS, Inc. October 1, 2004 Inventory #002157 WS2-9 Review “Basic” solution control options These specifications are not defaults, but were set via APDL commands when input file was read into ANSYS Session. Main Menu > Solution > Analysis Type > Sol’n Control Select tab: “Basic” Analysis Options = Large Displacement Static Time at end of loadstep = 4 (Total displacement) Number of substeps = 10 Max no. of substeps = 25 Min no. of substeps = 5 All solution items Write every substep [OK] Run the Solution Main Menu > Solution > Solve > Current LS [OK] OR enter the following commands: /SOLU SOLVE … Spot weld

10. 9.0 New Features Workshop ANSYS v9.0 © 2004 ANSYS, Inc. October 1, 2004 Inventory #002157 WS2-10 After the run is finished, post process results… … Spot weld

11. 9.0 New Features Workshop ANSYS v9.0 © 2004 ANSYS, Inc. October 1, 2004 Inventory #002157 WS2-11 Additional Features: The Spot weld assembly can also be created, listed and deleted with the following commands: SWGEN,sweld1,0.50,7,2,sw_node,, !Generates spot weld between first two surfaces (7 and 2) SWADD,sweld1,,12!Adds surface 12 SWLIST!Lists spot weld specifications and reactions (after solution is complete) SWDEL,sweld1 By default, ANSYS connects each surface together by creating MPC184 rigid link elements between the spot weld nodes. A flexible weld can be created if the active element is a BEAM188 with a circular cross section prior to weld creation. You must define the material properties for the BEAM188 and define the geometry of the beam section using section definition tools (SECTYPE and SECDATA commends) in advance of weld creation. Below is an example APDL script for creating the same spot weld in this workshop model using flexible BEAM188 elements. After the solution run, corresponding results in the flexible spot weld are conveniently summarized in the SWLIST and are also available in the traditional ETABLE for BEAM188. /PREP7 MP,EX,2,28e6 MP,PRXY,2,0.3 SECTYPE,2,beam,csolid SECDATA,0.25 ET,2,188 TYPE,2 MAT,2 SECNUM,2 SWGEN,sweld1,0.50,7,2,sw_node,, SWADD,sweld1,,12 … Spot weld Stress calculations in spot weld are added when BEAM188 is active prior to spot weld creation