The Presentation inside:

Slide 0


Slide 1

Slide 2

Problem Description Instead of meshing with solid elements the parasolid solid that represents a junction box, this workshop involves creating surfaces at mid-plane throughout the solid. Then, these mid-surfaces are meshed with 2D quadrilateral elements. From the 2D mesh, a complete analysis model is created, an analysis is performed, and results viewed.

Slide 3

Suggested Exercise Steps Create a database midsurface.db, and import a parasolid solid file, j_box.xmt Create a group that the midsurfaces will be placed in, midsurfaces. Use Group/Create. Create midsurfaces for the junction box. They will be in group midsurfaces. Post only the group with midsurfaces. Edit the gussets created by the midsurface operation. This involves eliminating the long thin tops of the gussets. Associate the edges of the gussets with the midsurfaces that represent the junction box. Paver mesh the midsurfaces. Equivalence the nodes to connect the 2D quad4 elements. Apply distributed loads to midsurface surfaces. Constrain select points of midsurface surfaces. Create material and element properties. Check the load case. Submit the finite element model to MSC.Nastran for analysis. Post process the results from MSC.Nastran

Slide 4

Step 1. Create new database and import parasolid file Create a new database called midsurface.db and set the model preferences. a. File / New. b. Enter midsurface as the file name. c. Click OK. d. Set the Tolerance to Based on Model. e. Set Analysis Code and Analysis Type to MSC.Nastran and Structural, respectively. f. Click on OK.

Slide 5

Step 1. Create new database and import parasolid file (Cont.) Import the parasolid. a. File / Import. b. Select j_box.xmt and click on Apply. c. Click OK when import summary appears. d. Click on the Iso 3 View icon.

Slide 6

Step 1. Create new database and import parasolid file(Cont.) This is what the Junction Box should look like when observing it from the ISO3 view. To better visualize the object, click the smooth shaded icon. Then, go back to the wireframe view. It is easier to work with this display.

Slide 7

Step 2. Create group for midsurfaces Create a new group called midsurface a. Group / Create. b. Enter midsurface for New Group Name. c. Make sure Make Current box is checked. d. Click on Apply. e. Click on Cancel.

Slide 8

Step 3. Create Midsurfaces from Parasolid Solid Create the midsurfaces a. Geometry: Create / Surface / Midsurface. b. Select Automatic icon. c. Enter 0.1251 for Max. Thickness. d. Click on Solid List, then on the solid. e. Click Apply (If Auto-Execute is checked do not click on Apply).

Slide 9

Step 4. Post Midsurfaces Group only Post the midsurface group only a. Group / Post. b. Select midsurface from Select Groups to Post. c. Click on Apply. d. Click on Cancel.

Slide 10

Step 5. Edit Gussets Edit the Gussets a. Geometry: Edit / Surface / Trim. b. Check Delete Sliver Surface. c. To select a surface to trim, click on any of the gussets. d. To select the trimming edge, click on the sloped edge of gusset e. Repeat procedure for the seven remaining gussets

Slide 11

Step 6. Associate Gusset Edges to Midsurface Surfaces Associate gusset edges to the junction box midsurfaces. (Need to associate the gussets to the junction box to make the quad meshes congruent during the Paver mesh.) a. Geometry: Associate / Curve / Surface. b. Associate vertical edge of gusset to adjacent surface. Click Apply. c. Associate bottom edge of gusset to bottom of junction box. Click Apply. d. Repeat for all remaining gussets. if Auto Execute is checked, it is not necessary to click Apply.

Slide 12

Step 6. Associate Gusset Edges to Midsurface Surfaces(Cont.) Here is the model after all of the gusset edges have been associated to the junction box midsurfaces. The associated edges are indicated by the triangles.

Slide 13

Step 7. Paver Mesh All Midsurface Surfaces Paver mesh all the midsurfaces of the solid. a. Elements : Create / Mesh / Surface. b. Make sure Quad, Paver, and Quad4 are selected. c. Remove check for Automatic Calculation and enter 0.1875 for the Global Edge Length. d. Click on Surface List. Select all the surfaces by dragging a box around the entire object. e. Click Apply *Surface List should be: Surface 1:13

Slide 14

Step 8. Equivalence Nodes to Connect 2D Quad Elements Observe that none of the elements at geometric boundaries are connected, they have free edges. This problem will be remedied with the Equivalence command. a. Elements: Verify / Element / Boundaries. b. Check Free Edges c. Click Apply. Yellow lines indicate free element edges.

Slide 15

Step 8. Equivalence Nodes to Connect 2D Quad Elements(Cont.) Equivalence the object and show that elements at the internal edges of the junction box are connected. a. Elements : Equivalence / All / Tolerance Cube. b. Click Apply. c. Elements : Verify / Element / Boundaries d. Check Free Edges. e. Click Apply. Now all free edges shown are desired free edges

Slide 16

Step 9. Create Distributed Loads Create the CID Distributed Load for the model. a. Loads/BCs : Create / CID Distributed Load / Element Uniform b. Enter CID_Distributed_Load in New Set Name. c. Make sure to select 2D under Target Element Type. d. Click Input Data… e. Enter <0 100 0> in Surf Distr Force. f. Click OK.

Slide 17

Step 9. Create Distributed Loads (Cont.) Continue to add Loads and Constraints a. Click Select Application Region… b. Click on Edge icon. c. Click the edge of any small hole on the end of the junction box at the greatest Y-coordinate. d. Click Add. e. Repeat c and d for remaining three holes. f. Click OK. g. Click Apply. Application Region should include edges Surface 4.5 4.6 4.7 4.8

Slide 18

Step 9. Create Distributed Loads (Cont.) This is an illustration of the junction box midsurface with the CID distributed loads.

Slide 19

Step 10. Constrain the Base of the Junction Box Bolt down the base of the junction box, i.e. constrain the four holes on the bottom so that they are fixed. a. Loads/BCs : Create / Displacement / Nodal. b. Enter Fixed for New Set Name. c. Click Input Data… d. Enter <0 0 0> for Translations. e. Enter <0 0 0> for Rotations. f. Click OK. g. Click Select Application Region. h. Select Select Geometry Entities and click on Curve or edge icon. i. Select the edge of any hole of the base and click Add. j. Repeat procedure for remaining three holes and Click OK. k. Click Apply. Application region should include Surface 2.21 2.22 2.23 2.24

Slide 20

Step 10. Constrain the Base of the Junction Box (Cont.) This is what the object should look like when constraints are applied. You can observe that the constraints on the bottom four holes of the junction box are all six degrees of freedom.

Slide 21

Step 11. Add Material and Element Properties Add the Material Properties for the model. a. Materials : Create / Isotropic / Manual Input. b. Enter Aluminum under Material Name. c. Click Input Properties. d. Enter 10E6 for Elastic Modulus and 0.3 for Poisson Ratio. e. Click OK. f. Click Apply.

Slide 22

Step 11. Add Material and Element Properties (Cont.) Add the Element Properties. a. Properties : Create / 2D / Shell. b. Enter 2D_shell in Property Set Name. c. Make sure Homogenous and Standard Formulation are selected. d. Click Input Properties… e. Click on Mat Prop Name icon and Select Aluminum from Select Material. f. Enter 0.125 for Thickness. g. Click OK. h. Under Select Members select the entire object by dragging a box around the junction box. I. Click Add and then click Apply. Application region is surface 1:13

Slide 23

Step 12. Check Load Case Check the load case a. Action: Modify. b. Select load case Default from Select Load Case to Modify. c. Check to see that the CID distributed load and the constraint are assigned to the default load case. d. Click Cancel.

Slide 24

Step 13. Run the analysis Run the analysis of the model. a. Analysis : Analyze / Entire Model / Full Run. b. Click on Translation Parameters. c. Select XDB and Print. d. Click OK. e. Click Subcases. f. Make sure the default subcase is selected. g. Click Apply and Cancel. h. Click Subcase Select… i. Make sure subcase Default is selected and click OK. j. Click Apply. It may be helpful to check each window, in order to become familiarized with each of the the various forms.

Slide 25

Step 14. Look at the Results Observe the results generated by MSC.Nastran. a. Analysis : Access Results / Attach XDB / Result Entities. b. Click Select Results File… c. Select the midsurfaces.xdb file. d. Click OK. e. Click Apply.

Slide 26

Step 14. Look at the Results (Cont.) Look at the Deformation created by the load. a. Results : Create / Deformation. b. Select Default, Static Subcase under Select Result Case(s). c. Select Displacements, Transitional. d. Click Apply. Here the deformation due to the CID Distributed loads is illustrated.

Slide 27

Step 14. Look at the Results (Cont.) Remove the undeformed plot and erase the geometry to get a better illustration of the load effects. a. Click on the Display Attributes icon. b. Remove the check from the Show Undeformed box and from the Show Title box as well. c. Click on the Plot/Erase icon. d. Click on Erase under Geometry. e. Click OK.

Slide 28

Step 14. Look at the Results (Cont.)

Slide 29

Step 14. Look at the Results (Cont.) Look at the von Mises stress for the junction box surface model. a. Results : Create / Fringe b. Select result case. c. Select Stress Tensor, and Quantity : von Mises. d. Click Apply. This illustration shows a combined representation of the deformation and von Mises stress of the junction box mid surface model.

Slide 30

Step 14. Look at the Results (Cont.) Modify the attributes to get a better fringe plot. a. Click on the Display Attributes icon. b. Change the Display to Element Edges. c. Uncheck the Show Title box. d. Click Apply.

Slide 31

Step 14. Look at the Results (Cont.) This final illustration shows the fringe plot along with the deformation plot.