Create a part file with two solids as shown in the picture, note that both parts (A & B) are symmetric in two planes. This is done to save computational time without sacrificing result accuracy. Position them so the snapping tab is not inserted in the slot. Note that this case is defined as a non-linear problem.

Use a Non-linear Analysis if the model fails any of the following assumptions: (1) All the materials in the model comply with Hooke's law, that is stress is directly proportional to strain. For example, plastics & rubbers do not comply,(2) The induced displacements are small enough so that you can ignore the change in the stiffness caused by loading. For example, K in F = K dx remains constant, (3) Boundary conditions do not vary during the application of loads. For example, contact problems are naturally non-linear because the boundary conditions change when loading contact occurs.

• Simulation Tab > Study Advisor > New Study > Non-linear > Static > Enter study name and click OK
• R-click the top icon of the simulation tree > Properties... > Solution tab > Stepping Options: Time increment [Automatic], Geometry Non-linear options [Use Large displacement formulation], Solver [Direct Sparse] > Incompatible Bonding Option [Simplified] > Ok
• R-click Part A icon > select Apply/Edit Material... > For part A enter Material [ABS], Property tab -> Model Type [Linear Elastic Isotropic] > Apply > Close
• R-click Part B icon > select Apply/Edit Material... > For part B enter Material [Delrin 2700], Property tab -> Model Type [Plasticity - von Mises] > Apply > Close
• R-click the Fixtures icon > select the Fixed definition > select the back surface of the part B (1) > Ok
• R-click the Fixtures icon > Advance Fixtures... > Type: Advanced [Use Reference Geometry], select the direction vector (2), the Fixture face (3), Enter the distance (+ or -) the snapping tab is to travel (4), and Variation with time [linear] > Ok
• R-click the Connections icon > Contact Set > Contact [Manually select contact sets], Type [No Penetration] > select those surfaces that interact for no penetration (5) Set 1 & (5) Set 2 (green arrows) > Properties [Friction] is optional for this example > Ok
• R-click the Fixtures icon > Advance Fixtures... > Type: Advanced [Symmetry] > select (6) set 1 & set 2 faces > OK
• R-click the Fixtures icon > Advance Fixtures... > Type: Advanced [Symmetry] > select (7) set 1 & set 2 faces > OK
• R-click the Mesh icon > Apply Mesh Control > select surfaces and enter custom mesh size > Ok
• R-click the Mesh icon > Create Mesh > select an adequate position for the slider between Coarse and Fine > Ok
• Click the Simulation Tab > Run

Tips to improve simulation study

1. To visualize the full part symmetric results, R-click Results > Stress > Edit Definition > Definition Tab > Advance Options > Display symmetric results > Ok
2. To create a Stress-Time plot, first set-up a sensor: R-Click the Sensors icon in the model tree > Add Sensor > Sensor Type [Simulation Data], Data Quantity [Stress] > Ok. Second R-click Result Options icon in the simulation tree > Define/Edit... > Save Results [For all solution steps], Response Plots [All Tracked Data Sensors] > Ok. Third, R-click the Results icon > Define Time History Plot... > Select the Sensor > Ok.

Create an Assembly file composed of two Part models as shown. Make sure there is a split face in part A as shown (1). Note that part A, the impact target, is a hollowed 1/2 of a sphere and part B, the projectile, is a cube. Position parts A & B in as touching at a tangent point (2).

• Simulation Tab > Study Advisor > New Study > Non-linear > Dynamic > Name: nonlinear_dyna > OK
• R-click the top icon of the simulation tree > Properties... > Solution tab > Stepping Options: End Time [0.0001], Time increment [Automatic], Geometry Non-linear options [Use Large displacement formulation], Solver [Large Solver Direct Sparse] > Incompatible Bonding Option [Simplified] > Ok
• R-click Part icon > select Apply Material to All... > Enter Material [Alloy Steel] > Apply > Close
• R-click the Connections icon > Contact Set > Contact [Manually select contact sets], Type [No Penetration] > select surfaces indicated in (3) > Properties [Friction] is optional for this example > Ok
• R-click the Fixtures icon > select the Fixed definition > select the back surface of the part A (4) > Ok
• R-click External Loads icon > Initial Conditions... > Type [Velocity], For selection set 1 go to the part tree and select part B, for selection set 2 select the edge in part B for velocity direction (5) hover over part B to see which direction the velocity vector is pointing, correct this by entering +/- value in the velocity box > Ok.
• R-click Damping icon > Edit Definition... > Enter α = 0.02, β = 0.04 > Ok. (see Tip 2)
• R-click the Fixtures icon > Advance Fixtures... > Type Tab > Advance [Use Reference Geometry], select point (6) and surface (7), Translations [push buttons that restrain any translation perpendicular to velocity] > Ok
• Click the Simulation Tab > Run

Tips to improve simulation study

1. To display the impact force over time, R-click Results > List Resul Force... > Options [Contact/Friction Force], Selection [select Split face (1)] > Update button > click Response Graph button > The Force/Friction vs. time graph is displayed.
2. Note that α β numbers are only needed if the model damping changes with changing frequencies (see Rayleigh Damping).

Create a single Part file composed of four (4) solid models. Make sure there is a reference plane next to pipe 1 as shown. Simulation Tab > Study Advisor > New Study > Type: Static, Name: pipes_sim > OK

• R-click the Part icon > select Apply/Edit Material... > Enter changes to each solid > Ok.
• R-click the Connections icon > Contact Set > Contact [Manually select contact sets], Type [No Penetration] > select those bodies/faces (1 & 2) that interact for no penetration > Ok
• R-click the Connections icon > Contact Set > Contact [Manually select contact sets], Type [No Penetration] > select faces from parts 1 & 3 for no penetration > Ok
• R-click the Connections icon > Contact Set > Contact [Manually select contact sets], Type [No Penetration] > select faces from parts 2 & 3 for no penetration > Ok
• R-click the Connections icon > Contact Set > Contact [Manually select contact sets], Type [No Penetration] > select faces from parts 2 & 4 for no penetration > Ok
• R-click the Connections icon > Contact Set > Contact [Manually select contact sets], Type [Virtual Wall] > select reference plane & face of part 1> Ok
• R-click the Fixtures icon > select the Fixed definition > select the surface indicated on part 1 > Ok
• R-click External Loads > Pressure... > Type [Normal to selected face] > select all faces as shown in the picture > enter pressure value > Ok
• R-click the Mesh icon > Create Mesh > select an adequate position for the slider between Coarse and Fine > Ok
• Click the Simulation Tab > Run

Tips to improve simulation study

1. To visualize a cross section of the assembly, R-click Results > Stress > Section Clipping... > Planar > Ok
2. To change the units of the stress plot: R-Click the Stress icon > Edit definition > Display [Von Mises] change units from N/m^2 to psi > Ok.
3. Use the Probe tool to study specific nodes of the results, R-click the Stress icon > Probe > Section Clipping... > Options [On selected entities] > select Vertex or Node > Update > Ok

Creating a Bolt Connection: R-click the Global Contact (GC) icon located under the Connections icon > Edit definition > in the Component Contact menu select contact type: No penetration > OK. Next, R-click the Connections icon > Bolts > In the Connectors menu select the type of fastener you want to use (e.g. foundation, bolt-and-nut, etc.) > select the circular edge of the bolt side and the circular edge of the nut side > enter material properties or select one from the library. Next enter force Pre-load values and friction coefficient> OK. A bolt icon now appears under the Connectors icon.

You can copy the newly created bolt into another hole to speed-up the set-up process. R-click the bolt > copy > R-click the Connections icon > Paste > R-click the new bolt copy > Edit definition > select the new edges defining the bolt and nut sides > OK.

Bolt simulation with a virtual wall: This is a good method to use if you want to simulate only one part as opposed to two bolted parts. First create a reference place next to the face of the part. This will be our virtual wall. Next, R-click the Connections icon > Contact Set (CS) > in the CS menu select type: virtual wall > select the face and then the corresponding reference place > OK. Next, R-click the Connections icon > Bolts > In the Connectors menu select Foundation Bolt > select the bolt side edge and the plane (virtual wall) > Enter other information as described before and click OK.

To view bolt stress results: R-click the Results folder icon > List Pin/Bolt/Bearing Force... > Make a note of the Shear forces, Axial forces and Bending moments listed.

Virtual bolt connectors don't provide data about the stress distribution on the bolt/nut, but rather the effect of the bolt on the parts adjacent to it, or on the overall assembly. If the stress distribution on the bolt/nut is important, you can model bolt behavior by including the solid model of the bolt and nuts and then using contact conditions rather than the virtual bolt connector.

Find the stresses caused by a fall from a specific height or given a velocity at the time of impact:

• Place a Reference plane next to the area that hits the ground
• Simulation Tab > Study Advisor > New Study > Type: Drop Test, Name: drop_sim > OK
• Parts: Assign material to all parts
• Connections:R-click >
• Mesh: R-click > Create mesh
• Set-up:R-click > Drop test set-up > Drop Height or Velocity at impact > Pick gravity direction and Target plane (Flexible or Rigid)
• Result Options:R-click > Result Options > Enter Solution Time After Impact, etc. > Ok

Discovering the natural frequencies to avoid designs that resonate:

• Simulation > new study > frequency > OK.
• R-click the part and assign material to it. Remember that you can copy material assignment from one study to another by: select all the parts already setup > drag-and-drop the parts in the tab containing the new study.
• Enter appropriate fixtures.
• We are only looking for natural frequencies and modes of vibration so no loads need to be applied.
• R-click the top of the study tree > properties > Options: number of frequencies [5], use soft spring to stabilize model, ...no penetration contacting surfaces, simplified bonding contact. Solver: Automatic, Direct sparse, FFEPlus > OK.
• Create mesh > OK.
• Remember that you can copy and paste mesh settings from one study to another. Just R-click and select copy or paste.
• R-click the study name icon > Run.
• View the results: R-click the results icon > List resonant (natural) frequencies to view the potentially troublesome frequencies > OK.

The modes or shapes of the vibrations are also important. Most earthquake waves have a frequency of less than 20 Hz, so the waves themselves are usually not heard, this is according to earthquake. usgs.gov/learn/facts.php. The key is to optimize the structure design against the movement of the modes. That is, to make it stiff so its modes are 'moved' away from the frequencies it is likely to encounter.

Fatigue failure study (previous static study required):

• Simulation > Study advisor > New study > Fatigue > Ok.
• R-click the Loading icon > Add event > Enter: Number of cycles, Type of cycle (Fully reversed, zero based, loading ratio?, find cycle peak) and pick the static study previously conducted.
• R-click the part icon > Apply/edit fatigue data > this should be automatically loaded already but you can define it here if necessary > Ok.
• R-click the top of the study tree > run > Startup [check Solve], CPU and memory [], Results processing after finishing the calculations [load results] > Run.

The first set of results show the damage percentile showing where most of the damage occur. The second set shows the maximum and minimum cycles per part (e.g. red last longer, blue doesn't last very long).