COMSOL 6.4 - Transient Rolling Contact

This conceptual example shows how to handle a transient contact problem with stick–slip friction transition. A soft hollow pipe subjected to a gravity load is released at the top of a half-pipe. The motion varies between sliding and rolling, depending on the position in the half-pipe and the velocity of the pipe. The pipe deforms such that its cross-section becomes oval due to the contact and the inertial forces. An analysis of the energy balance validates the accuracy of the solution.

Model Definition

As illustrated in Figure 1, the geometry consists of a section cut from a hollow pipe and a half-pipe. The pipe radius is 15 cm and the thickness is 2 cm. The half-pipe radius is about 1 m and has a transition length of 50 cm.

Figure 1: Model geometry.

The half-pipe is rigid, so it is modeled only by a meshed edge without any physics defined. The hollow pipe is subjected to gravity and dropped in the half-pipe with its centroid at a height of 75 cm above the horizontal plane. The pipe is always in contact with the half-pipe.

The friction coefficient is defined as a function of the slip velocity through the exponential dynamic Coulomb friction model:

(1)

Here, μdyn = 0.3 is the dynamic friction coefficient, and μstat = 0.5 is the static friction coefficient. The friction decay coefficient α = 1, and v is the slip velocity.

The solution is computed for 4 s. The pipe displacement and the energy balance are the quantities of interest.

Results and Discussion

Figure 2 shows the von Mises stress distribution in the pipe at the final step together with the trajectory of a point located on the outer surface of the pipe. You can notice the deformation of the pipe due to gravity, and that the trajectory path clearly shows a transition between the stick and slip friction stages. In the former, the trajectory is smoothly following the rotation of the pipe, while in the latter stage the trajectory has a slightly more elongated path. Figure 3 below shows the position of the pipe at every 0.4 s.

Figure 2: Stress distribution and point trajectory of the pipe.

Figure 3: Position of the pipe at every 0.4 s.

In Figure 4, you can see the energy balance. As expected, the potential energy decreases as the kinetic energy increases. Because of frictional dissipation, the pipe never reaches its original height in the half-pipe. Most of the energy is lost due to friction when the pipe reaches the steeper slope region of the half-pipe. After 2 s, the pipe remains in the region with lower slope and will roll rather than slide. Note also that part of the total energy is stored as elastic strain energy, due to the deformation of the pipe. Lastly, Figure 5 shows the friction coefficient as function of time.

Figure 4: Energy balance versus time.

Figure 5: Friction coefficient versus time.

Notes About the COMSOL Implementation

To speed up the computation, manual time stepping is used to solve the model. Note, however, that for manual time stepping there is no error control, so it is good practice to inspect the total energy in a probe plot to verify the energy balance. In Figure 6 you can see that the conservation of the total energy is fulfilled for all time steps taken by the solver.

Figure 6: Total energy versus time probe plot. Note the scale on the y-axis.

Structural_Mechanics_Module/Contact_and_Friction/transient_rolling_contact

Modeling Instructions

From the menu, choose .

New

In the window, click

Model Wizard

In the window, click

In the tree, select > .

Click .

Click

In the tree, select > .

Click

Global Definitions

Parameters 1

In the window, under click .

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Value	Description
rp	15[cm]	0.15 m	Pipe radius
th	2[cm]	0.02 m	Pipe thickness
theta	10[deg]	0.17453 rad	Auxiliary geometric parameter

Geometry 1

Circular Arc 1 (ca1)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. In the text field, type -1.

Locate the section. In the text field, type 180.

Circular Arc 2 (ca2)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. In the text field, type 0.5.

In the text field, type -1.

Locate the section. In the text field, type 1.5.

In the text field, type 0.

Locate the section. In the text field, type 270.

Click

Line Segment 1 (ls1)

In the toolbar, click

and choose .

On the object , select Point 2 only.

In the window for , locate the section.

Click to select the

toggle button for .

On the object , select Point 1 only.

Convert to Curve 1 (ccur1)

In the toolbar, click

and choose .

Click in the window and then press Ctrl+A to select all objects.

In the window for , locate the section.

Find the subsection. Click .

In the dialog, type Contact Source in the text field.

Click .

In the window for , click

Circle 1 (c1)

In the toolbar, click

In the window for , locate the section.

In the text field, type rp.

Locate the section. In the text field, type -1+rp.

Click to expand the section. In the table, enter the following settings:


Layer name	Thickness (m)
Layer 1	th

Delete Entities 1 (del1)

In the window, right-click and choose .

In the window for , locate the section.

From the list, choose .

On the object , select Domain 5 only.

Rotate 1 (rot1)

In the toolbar, click

and choose .

Select the object only.

In the window for , locate the section.

In the text field, type theta.

Form Union (fin)

In the window, under > click .

In the window for , locate the section.

From the list, choose .

Clear the checkbox.

Click

Materials

Material 1 (mat1)

In the window, under right-click and choose .

In the window for , locate the section.

In the table, enter the following settings:


Property	Variable	Value	Unit	Property group
Young’s modulus	E	5[MPa]	Pa	Young’s modulus and Poisson’s ratio
Poisson’s ratio	nu	0.3	1	Young’s modulus and Poisson’s ratio
Density	rho	1e3[kg/m^3]	kg/m³	Basic

Solid Mechanics (solid)

Gravity 1

In the toolbar, click

and choose .

Definitions

Contact Destination

In the toolbar, click

In the window for , type Contact Destination in the text field.

Locate the section. From the list, choose .

Select the checkbox.

Select Boundaries 8, 9, 12, and 15 only.

Contact Pair 1 (p1)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. Click to select the

toggle button.

From the list, choose .

Solid Mechanics (solid)

Contact 1

The stick-slip friction is better resolved using the method.

In the window, under > click .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

From the list, choose .

Friction 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

In the μstat text field, type 0.5.

In the μdyn text field, type 0.3.

In the αdcf text field, type 1.

Click the

button in the toolbar.

In the dialog, in the tree, select the checkbox for the node > .

Click .

In the window for , click to expand the section.

Select the checkbox.

Definitions

Integration 1 (intop1)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Variables 1

In the window, right-click and choose .

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Unit	Description
V	intop1(g_constsolid.rho(y+0.85[m]))*1[m]	N·m	Potential energy

Maximum 1 (maxop1)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

Variables 1

In the window, click .

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Unit	Description
mu_max	maxop1(if(solid.dcnt1.isContact_p1,solid.dcnt1.mu_fric,0))		Maximum value of friction coefficient

Mesh 1

Edge 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Size 1

Right-click and choose .

In the window for , locate the section.

Click the button.

Locate the section.

Select the checkbox. In the associated text field, type 0.005.

Mapped 1

In the toolbar, click

Distribution 1

Right-click and choose .

Select Boundaries 4–7 only.

In the window for , locate the section.

In the text field, type 3.

Distribution 2

In the window, right-click and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. In the text field, type 20.

Study 1

Step 1: Time Dependent

In the window, under click .

In the window for , locate the section.

In the text field, type range(0,2e-2,4).

Solution 1 (sol1)

In the toolbar, click

In the window, expand the node.

In the window, expand the > > > node, then click .

In the window for , locate the section.

In the text field, type 5e4.

Continue with setting manual scaling for the following variables:


Variable name	Scale
comp1.solid.Tn_p1	5e4
comp1.solid.Tt_p1	5e4
comp1.solid.Wfric_p1	5e-3*5e4
comp1.u	5e-3

In the window, under > > click .

In the window for , click to expand the section.

From the list, choose .

In the text field, type 5e-3.

In the window, expand the > > > node, then click .

In the window for , locate the section.

In the text field, type 0.1.

In the window, expand the > > > > node, then click .

In the window for , click to expand the section.

From the list, choose .

Definitions

Variables 1

In the window, under > click .

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Unit	Description
W_tot	solid.Wk_tot+solid.Ws_tot+V+solid.Wfric_tot	N·m	Total energy

Global Variable Probe 1 (var1)

In the toolbar, click

and choose .

In the window for , locate the section.

In the text field, type W_tot.

Study 1

In the toolbar, click

Results

Stress (solid)

In the window for , click to expand the section.

From the list, choose .

In the text area, type von Mises stress (N/m<sup>2</sup>) and point trajectory.

Locate the section. From the list, choose .

Point Trajectories 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

In the text field, type u-cos(theta).

In the text field, type v-sin(theta).

Select Point 5 only.

Locate the section. Find the subsection. From the list, choose .

Find the subsection. From the list, choose .

Select the checkbox. In the associated text field, type 15.

In the toolbar, click

Click the

button in the toolbar.

Animation 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Surface 1

In the window, under > click .

In the window for , locate the section.

From the list, choose .

Animation 1

In the window, under > click .

In the window for , locate the section.

From the list, choose .

Locate the section. In the text field, type 1e-1.

Click the

button in the toolbar.

Energy

In the toolbar, click

In the window for , type Energy in the text field.

Click to expand the section. From the list, choose .

Locate the section.

Select the checkbox. In the associated text field, type Energy (J).

Global 1

Right-click and choose .

In the window for , locate the section.

In the table, enter the following settings:


Expression	Unit	Description
solid.Wk_tot	J	Total kinetic energy
solid.Ws_tot	J	Total elastic strain energy
V	N*m	Potential energy
solid.Wfric_tot	J	Total frictional dissipation energy
W_tot	J	Total energy

In the toolbar, click

Friction Coefficient

In the toolbar, click

In the window for , type Friction Coefficient in the text field.

Locate the section. From the list, choose .

Locate the section. Clear the checkbox.

Global 1

Right-click and choose .

In the window for , locate the section.

In the table, enter the following settings:


Expression	Unit	Description
mu_max	1	Maximum value of friction coefficient

In the toolbar, click