1) Click on File and go to Current Directory...
2) Browse to C:\Training. If folder is not there, create it. Then click Choose.
3) Click Fill.
1) Go to File - Import - General CAD with Repair.
2) Under Type select Parasolid.
3) Click on Import Parasolid File.
4) Select spring2a.xmt_text and click Open and OK.
5) Click Fill, if the model is not visible on your screen. Click View and go to Plot Control.
6) Uncheck Nodes, Points, Curves and Surfaces.
7) Under Elements, select Solids.
8) Click Redraw and OK.
1) Under Geometry & Mesh tab, in the Automesh group, click Surfaces.
2) Enter Element Size 1.0 in Patran Surface Mesher.
3) Click Tri Mesh!
4) Then click All Existing.
1) Under the Geometry & Mesh tab, in the Automesh group, click Volume.
2) Enter 1.5 for the Coarsening Factor.
3) Click Tet Mesh!
4) Click All Existing.
5) Click View and go to Plot Control.
6) Check Points.
7) Make sure Surfaces is checked.
8) Click Redrew and click OK.
1) Under Material Properties click on New, then click on Standard.
2) Under Name, enter aluminum and hit enter.
3) Click on Structural.
4) Enter 1e7 for the Young's Modulus and enter 0.3 for the Poisson's Ratio. Click OK.
5) Click Add under Elements.
6) Click on All Existing.
7) Click on End List.
1) Under the Geometry & Mesh tab and under Basic Manipulation, click on Geometry & Mesh.
2) Under Points, click Add.
3) Enter points from surfs_1.txt, -15 -2.55 -15 -15 -2.55 15 15 -2.55 15 15 -2.55 -15 -15 16 -15 -15 16 15 15 16 15 15 16 -15.
4) Under Surface, click on Add and select the the 4 points on top of the spring in clockwise or in counter-clockwise order as shown and then click on End List.
5) Under Surface, click on Add and select the the 4 points on bottom of the spring in clockwise or in counter-clockwise order as shown and then click on End List.
1) In the Tables & Coord. Syst. tab, click on New - Independent Variable.
2) Click Type.
3) Click Time.
4) Click Data Points - Add.
5) Enter 0 0 1 1 and hit Enter.
1) Under the Contact tab, go to New and then Deformable.
2) Enter the Name as spring.
3) Under Elements, click Add.
4) Click All Existing.
5) Click End List.
6) Click Copy.
1) Enter Name as bottom_plate.
2) Click Type.
3) Click Rigid.
4) Click Properties.
5) Enter Friction Coefficient as 0.3. Click OK.
6) Click 3-D Surface - Add.
7) Click the Lower Plate.
8) Click End List.
9) Click Copy.
1) Enter Name as top_plate.
2) Click Type - Rigid.
3) Click Properties.
4) Enter Friction Coefficient as 0.3.
5) In Body Control, select Position.
6) Click Parameters.
7) In Position (Center of Rotation) enter Y value -7.
8) Click Table.
9) Click table1.
10) Click OK, OK, and OK.
11) Click 3-D - Surfaces - Add.
12) Select Top Plate.
13) Click End List.
1) Under Contact tab, click Identify Backfaces in the Contact Bodies group.
2) Check inside of plate should be Gold color and outside of plates should be Magenta Color. If that wasn’t the case continue to:
3) Click Tools - Flip Surfaces in Contact Bodies group.
4) Click the surface which needs to be flipped (Example > top plate outside is magenta, which needs to flipped)
5) Click End List.
1) Under the Contact tab and under Contact Table, click New.
2) Click Properties.
3) In All Entities - Contact Type click Touching.
4) On the contact table, click the T at the intersection between spring and bottom_plate. (It is T when you change all contact types to Touching, but in the next step it will be changed to G)
5) Change Contact Type to Glue. Click OK and OK.
1) Under the Loadcases tab, go to New and click on Static.
2) Click Properties.
3) Click Multi-Criteria.
4) Click Parameters.
5) Enter Maximum Fraction of Loadcase Time = 0.01. Click OK and OK.
1) Under the Jobs tab, go to New and then Structural.
2) Click Properties.
3) Select lcase1.
4) Click Contact Control.
5) Change the Method to Segment to Segment.
6) Change Friction Type - Coulomb Bilinear. Click OK.
7) Click Initial Contact.
8) Click on Contact Table.
9) Click Ctable1. Click OK.
10) Click Job Results.
11) Under Available Element Tensors, click Stress and Total Strain. Click OK and OK.
1) Click Run.
2) Click Save Model.
3) Click Submit.
4) Click Monitor.
5) When Status shows Complete, click Open Post File (Results Menu).
1) Under Style, select Deformed & Original.
2) Under Scalar Plot, select Contour Bands.
3) Click Scalar.
4) Select Equivalent of Stress. Click OK.
5) Click Monitor Result File.
6) Under Results tab, click History Plot.
7) Click All Incs.
8) Click Add Curves.
9) Click Global.
10) In Contact Body Variables, for X-axis, click Pos Y top_plate and for Y-axis, click Force Y top_plate.
11) Click Fit.
Go back and change the element meshing from Tet4 to Tet10, Rerun the analysis and compare your results. Below are the differences you would find when you refine your model with Tet10 Meshing.
