HB 002 - Backbone curve of a clamped-clamped beam

Model definition

In this example, the vibration of a thin metal beam clamped from both ends (a clamped-clamped beam) is considered. When plotted, the displacement of the vibrating beam forms a so called “backbone curve”. The setup is detailed in the paper Parallel harmonic balance method for analysis of nonlinear dynamical systems¹. Below is an image of the model in Quanscient Allsolve model view.

Simulation setup guide

Step 1 - Create the geometry

In the Model section, create boxes to form the beam geometry:

Name	Element type	Center point (m)	Size (m)	Rotation (deg)
beam	Box	X: 0	X: 1	X: 0
		Y: 0	Y: 0.03	Y: 0
		Z: 0	Z: 0.03	Z: 0

Name	Element type	Center point (m)	Size (m)	Rotation (deg)
beam half x	Box	X: 0.25	X: 0.5	X: 0
		Y: 0	Y: 0.03	Y: 0
		Z: 0	Z: 0.03	Z: 0

Name	Element type	Center point (m)	Size (m)	Rotation (deg)
beam half y	Box	X: 0	X: 1	X: 0
		Y: 0.25	Y: 0.015	Y: 0
		Z: 0	Z: 0.03	Z: 0

Name	Element type	Center point (m)	Size (m)	Rotation (deg)
beam half z	Box	X: 0	X: 1	X: 0
		Y: 0	Y: 0.03	Y: 0
		Z: 0.25	Z: 0.015	Z: 0

Click Confirm model changes after creating all the boxes.

Step 2 - Define shared expressions and materials

Proceed to the Properties section.

First, define a shared expression:

Name	Description	Expression
freq	Fundamental frequenzy for multiharmonic simulation	100

Then, define the material of the beam, as detailed in the paper¹:

Create a new material:

• Name
  • Material from paper
• Target
  • All volumes.
  • Save the target as a shared region.

Caution: material name

Make sure to name the material as Material from paper It is referred to in an output definition as reg.material_from_paper. The reference will not work with other names.

• Properties
  • Add Density (kg / m^3).
    • Set value to 7800.
  • Add Elasticity matrix (Pa).
    • Set Poisson’s ratio to 0.3.
    • Set Young’s modulus to 210e9.

Now, your shared expressions and model materials are defined.

Step 3 - Define the physics

Proceed to the Physics section to define the physics.

For this example, only Solid mechanics are required.

Solid mechanics

• As solid mechanics target, select all volumes (or let the application default it to all volumes).
• Add Clamp.
  • As target, select the end surfaces of the beam (surfaces 1, 7, 12, 19, 22, 27, 33 and 36).
• Add Load.
  • Name it as Center point load.

  Caution: Load physics name

  Make sure to name the load physics as Center point load so that it can later be used in scripting. The load target is referred to in scripting as reg.center_point_load_target.

  • As target, select the middle-most point of the beam inside the volume (point 7).
    • Add the target as a shared region.
  • Set Parameters as in the image below.

Now, your simulation physics are defined.

Step 4 - Set up the mesh

Proceed to the Simulations section to set up the mesh.

In this example, Structured meshing is utilized. Create a new mesh:

• Set Mesh quality to Expert settings.
• Set Used mesher to Basic.

Create a structured entity for each of the 8 volumes in the model:

• Click Add structured entity.
  • Select Volume.
  • Add a volume 1 - 8 as target.
  • Repeat this 8 times, each time targetting a different volume.

Click Apply at this point to save your work so far.

• For each structured entity, choose segment counts so that the long sides are divided into 5 segments, and the short sides into 2 segments. See the image below for clarification (long side curve A of volume 2 is highlighted in red).

  Caution: Segment identifiers

  The curve identifiers A/B/C may differ between volumes, so be careful to pick the correct segment counts for each volume.

• Click Apply & mesh.

Now your mesh is complete, and should look like in the image below.

Step 5 - Simulate

In the Simulations section, create a new simulation:

• Analysis type
  • Multiharmonic
• Fundamental frequency
  • freq (100 Hz, this was set as a shared expression in Step 2)
• Harmonics
  • 1, 2, 3, 4, 5, 6, 7
• Solver mode
  • Direct solver
• Mesh
  • Select the mesh you created in Step 4.
• Input
  • Add freq sweep with override expression linspace(161, 164, 41).
• Output
  • Add Max u2 custom output with output expression maxvalue(reg.material_from_paper, norm(getharmonic(2, u)), 5).

Run the simulation by clicking Not Run.

Step 6 - Plot results

In the Simulations section, plot the results.

For the autogenerated script and simulation setup in this example, the results will look like in the image below.

To see the backbone curve and get all it’s branches, some scripting is required. Some branches can be hard to obtain, and expertise with continuation methods is required. Below is an image of the backbone curve with one missing branch drawn in red.

 

---

References

Footnotes

1. https://asmedigitalcollection.asme.org/GT/proceedings/GT2020/84232/V011T30A028/1095387 ↩ ↩²