Pipe Crush Analysis
Step 1 - Create a New Database.
1) Click MD Explicit.
2) Select File /Save.
3) Enter pipe_crush.
4) Click Save.
Step 2 - Set the Units.
1) Check in the lower right-hand corner for the current system of units.
2) If the current system of units is not English units (in, lb, s), click on the box to bring up the User Options window.
3) Click on Standard Units.
4) Scroll down and select the line with units in, lb, s,…
5) Click OK and OK.
Step 3 - Import Mesh.
1) Select File / Import / Nastran….
2) Select pipe_crush_model.bdf.
3) Click Open.
Step 4- Rename the Parts.
1) In the Model Browser, double-click on part, SHELL_1…
2) Rename the part as pipe.
3) Click OK.
4) In the Model Browser, double-click on part, SHELL_2…
5) Rename the part as rigid.
6) Click OK.
Step 5 - Create Steel Material for Pipe.
1) Under the Materials and Properties tab, click MAT [1 to 20] in the Materials group, and then [003] MAT_PLASTIC_KINEMATIC.
2) Enter steel for Name.
3) Enter 7.85e-4 for Density.
4) Enter 30e6 for Young’s Modulus.
5) Enter 0.3 for Poisson’s Ratio.
6) Enter 36e3 for Yield Stress. 7) Click OK.
Step 6 - Create Rigid Material.
1) Under the Materials and Properties tab, select MAT [1 to 20] in the Materials group, and then [20]MAT_RIGID.
2) Enter rigid_mat for Name.
3) Enter 7.85e-4 for Density.
4) Enter 30e6 for Young’s Modulus.
5) Enter 0.3 for Poisson’s Ratio.
6) Click OK.
Step 7 - Modify the Property for the pipe.
1) From the Model Browser, double-click on the property, SHELL_1...
2) Enter pipe for property Name.
3) Click in the Entities text box, and select the part, pipe, from the Model Browser.
4) Click in the Material text box, and select the material steel from the Model Browser.
5) Click OK.
Step 8 - Modify the Rigid Surface Property.
1) In the Model Browser, double-click on the property, SHELL_2…=.
2) Enter rigid for Name.
3) Click in the Entities text box, and select the part, rigid, from the Model Browser.
4) Click in the Material text box, and select the material rigid_mat from the Model Browser.
5) Enter 0.125 for Part thickness.
6) Click OK.
Step 9 - Create LBCs at the Ends of the Pipe.
1) Click Fixed in the LBCs group.
2) Enter end_disp for Name.
3) Click in the Entities text box and select the nodes on the left and right edges of the pipe.
4) Click OK.
Step 10 - Define Initial Velocity.
1) Click Transient Condition in the Global group.
2) Enter initial_velocity_upper for Name.
3) Select Initial Condition (TIC) for Type.
4) Check Ty and enter -6000.
5) Click in the Entities text box and select all the nodes on the upper rigid surface.
6) Click OK.
7) Click Transient Condition in the Global group.
8) Enter initial_velocity_lower for Name.
9) Select Initial Condition (TIC) for Type.
10) Check Ty and enter 6000.
11) Click in the Entities text box, and select all the nodes on the lower rigid surface.
12) Click OK.
Step 11 - Create Deformable Surface Contact.
1) Click the Deformable Contact Body icon in the Contact group.
2) Enter pipe as Name.
3) Select Deformable Surface for Type.
4) Click in the Pick Entities text box, and select the part pipe from the Model Browser.
5) Click Apply.
6) Enter rigid as Name.
7) Select Deformable Surface for Type.
8) Click in the Pick Entities text box, and select the part rigid from the Model Browser.
9) Click OK.
Step 12 - Create Nastran Job.
1) In the Model Browser, right-click Pipe_crush_model.bdf and select Create new Nastran Job.
2) Enter pipe_crush as Job Name.
3) Click OK.
Step 13 - Create Loadcase Control Parameters.
1) In the Model Browser, double-click Load Case Control.
2) Enter 0.007 for Ending Time.
3) Enter 0.0001 for Time Increment for Outputs.
4) Click Apply.
5) Click Close.
Step 14 - Solve MD Explicit Contact Analysis and Attach Results.
1) In the Model Browser, right-click pipe_crush, and select Run.
2) Select File / Attach Results….
3) Click the File path icon.
4) Select pipe_crush_dytr.d3plot.
5) Click Open.
6) Click OK.
Step15 - Plot Stress Fringe.
1) Under the Results tab, click Fringe in the Results group.
2) Select Time 0.007…
3) Select Stress, Components under Result type.
4) Select von Mises under Derivation.
5) Select At Shell Outer Surface under Layers.
6) Click Update.
Step 16 - Animate the Stresses.
1) Click Deformation in the Results group.
2) Select all Result Cases by clicking on pipe_crush.dytr.
3) Click the Deformation tab.
4) Select True under Deformation scaling.
5) Click the Plot Data tab.
6) Select Displacement, Components under Result type.
7) Click Update.
8) Pull down Fringe for Plot type.
9) Select all the Result Cases by clicking on pipe_crush.dytr.
10) Select Stress, Components under Result type.
11) Select von Mises under Derivation.
12) Check Animate.
13) Click Update.
Step 17 - Save and Exit SimXpert Database.
1) Pull down File / Save.
2) Pull down File / Save.
