STRESS RELAXATION TEST IN ABAQUS BY sHAFI DADA.pdf

Tutorial Number 21: Compression and Stress Relaxation of a viscoelastic rubber seal Stefano Morlacchi August 2015

Strategic Simulation & Analysis Ltd Southill Barn, Southill Business Park, Cornbury Park, Charlbury, Charlbury, Oxfordshire, OX7 3EW T. 01608 811777 F. 016088117 01608811770 70 [email protected] W. www www.ssanalysis.co.uk .ssanalysis.co.uk

1.

Introduction

In this tutorial, you will investigate the time-dependent viscoelastic behaviour of a rubber seal after compression. You will use the Abaqus calibration tool to calibrate a linear viscoelastic material model of a generic rubber starting from stress-relaxation test-data. Quadrangular 2D plane strain elements will be used.

When you complete this tutorial, you will be able to: -

Calibrate a linear viscoelastic material model starting from experimental stress relaxation test data.

-

Create a model to compress a rubber seal with a *static procedure and then evaluate its stress relaxation using a *visco procedure.

Preliminaries - The model is based on the SI units based on millimetres.

Figure 1: Consistent sets of units available in Abaqus.

2.

Setting up the model

Open the Abaqus database file Tutorial 21.cae This file contains the geometry of the two parts, the 2D planar rubber seal and a rigid component used to simulate the compression. Geometry is in mm so material properties and loading conditions have to be defined accordingly to the table above.

Strategic Simulation & Analysis Ltd Southill Barn, Southill Business Park, Cornbury Park, Charlbury, Oxfordshire, OX7 3EW T. 01608 811777 F. 01608811770 [email protected] W. www.ssanalysis.co.uk

2

3.

Material and section properties

Enter the property module and define a new material model for rubber. You will define first the instantaneous elastic response of the material through the *Hyperelastic mechanical behaviour (Figure 2) and then the time-dependent mechanical properties through the *Viscoelastic keyword.

1. Go into the Property Module and click the Create Material icon. In the Edit Material dialog box, name the material Rubber . From the material editor’s menu bar, select Mechanical

→

Elasticity

→

Hyperelastic, select Neo-Hooke as

Strain Energy Potential, Coefficients as Input source and Instantaneous as Moduli time scale. Enter 200 and 0.0 as C10 and D1 coefficients, respectively.

Figure 2. Stress Strain curve of the instantaneous elastic response of the rubber defined by means of a Neo-Hooke strain energy potential.

2.

Figure 3 shows the time-dependent behaviour of the rubber evaluated

though a stress relaxation test at 5% strain. The material will be modelled with a linear viscoelastic model calibrated using Abaqus which is valid only if the timedependent properties are not dependent on the stress/strain levels. In this case, you can notice that mechanical properties degrade in 50s to reach the 30% of the initial values (Fig. 3). Strategic Simulation & Analysis Ltd Southill Barn, Southill Business Park, Cornbury Park, Charlbury, Oxfordshire, OX7 3EW T. 01608 811777 F. 01608811770 [email protected] W. www.ssanalysis.co.uk

3

3. In the Edit Material dialog box of the Rubber material model, select Mechanical

→ Elasticity →

Viscoelastic, select Time as Domain, Relaxation

test data as Time, enter 5 as Maximum number of Prony series and 0.01 as Allowable average root-mean-square error. Select Shear Test Data as Test data and enter the values in the middle and right columns as shown in Figure 4. Set 0.3 as long term shear modulus. Click Ok and click OK.

Stress Relaxation test at 5% strain Nominal Stress Normalized Stress

Time

200

1

0.01

180

0.9

0.4

164

0.82

1

144

0.72

2

112

0.56

5

88

0.44

10

76

0.38

20

60

0.3

50

Figure 3. Left, stress relaxation test data at 5% strain. The middle column represents the stress data normalized by the initial stress value and it is p lotted in the right plot.

Figure 4. Definition of the rubber v iscoelastic properties.


4

4. Right click the material called Rubber in the model tree and click on Evaluate. Unselect Perform Hyperelastic evaluation in the first tab. Move to the Viscoelastic tab, accept the default option in the Available Input Data area and select the Stress Relaxation Mode only in the Response plots area (Fig. 5). Click Ok and wait for the results.

5. Once the evaluation is completed, check the comparison between the experimental relaxation test data and the numerical model calibrated by Abaqus to match the test data. In the evaluation results, look at the Prony series terms that will automatically be used by Abaqus (Fig.7).

Figure 5. Evaluation of viscoelastic properties of the Rubber material model.


5

Figure 6. Comparison between, numerical model and experimental test data.

Figure 7. Terms of Prony series used to model the Rubber time-dependent behaviour.

6. Close the viewport of the material evaluation and create a

solid

homogeneous section referring to the material Rubber , by double-clicking Sections in the model tree. Assign the Rubber section to the part called Seal .


6

4.

Assembly and Step

1. Enter the assembly module and look at the instances already pre-assembled (Fig. 8).

Figure 8. Assembly of the numerical model.

2. Enter the step module and create a static general step called StepCompression with duration of 1E-6s to compress the seal. Turn on the nlgeom parameter and enter 1E-7s as initial increment size. The very small step size is required since the *visco procedure uses the total time (not the step time) to calculate the time-dependent properties of the material. Create then a *Visco step called Step-relaxation, enter a time period of 50 s, 0.1 as initial increment size and 0.1 as viscolelastic strain error tolerance. This step will calculate the stress relaxation of the seal in 50s. Viscoelastic properties are only taken into account in the Visco, Couple temp-disp and Dynamic procedures.

3. Create a new History Output request, choosing the set called Set-RP as region and RF2 as output variable. This output will monitor the time history of the reaction force necessary to compress the seal.


7

5.

Mesh

Enter the mesh module and mesh the part called Seal . Select 2 as global element size. Mesh the part and make sure that the element type chosen is a plane strain hybrid element for both quadrangular and triangular elements. Tick in both tabs.

6.

Interactions

Enter the Interaction module to create a mechanical interaction between the Seal and the two rigid bodies. 1. Interaction Property. Click on the Create an Interaction Property icon

in

the vertical toolbox and select Contact as Type in the opening dialog box. Select Mechanical  Normal Behaviour . Unselect the option ‘Allow separation after contact’ and Click OK.


8

2. Surface-to-Surface interaction. Create a new surface to surface interaction during the Step-Compression between the seal and the upper rigid surface. Select the previously defined surface called Master-1 as master surface and the surface Slave-1 as slave surface. Use the button Surfaces in the lower message bar to facilitate the surface selection. In the Edit Interaction dialog box, select IntProp-1 as interaction property. Click OK.

3. Surface-to-Surface interaction. Repeat the same steps to define the contact between the seal and lower rigid surface using Master-2 and Slave-2 as surfaces.

7.

Boundary conditions

1. Create an encastre boundary condition. In the initial step, create an encastre boundary condition using the set called SetENC already created at the assembly level which constrains the lower rigid surface.

2. Create a displacement boundary condition to t he rigid surface In the step called Step-Compression, create a displacement boundary condition using the set called Set-DISP already created at the assembly level. Enter -25 as displacement in direction-2 and 0 in the other fields.

3. Create a displacement boundary condition in the seal In the step called Step-Compression, create a displacement boundary condition using the set called Set-XDISP already created at the assembly level. Enter 0 as displacement in direction-1 to constrain the horizontal rigid body motions of the Seal. Click OK.

8.

Job module

Enter the Job module and create a new Job called

S t r e s s - R e l a x a t i o n .

Submit

the job and monitor the convergence.


9

9.

Results

1. In order to allow a better visualization of the stress field, extrude the 2D elements into a 3D visualization. Go on View

 ODB

Display Options. In the

Sweep/Extrude tab, enter a depth of 10 for both elements and the analytical surfaces.

2. Show the contour map of the Von Mises stress field in the seal by clicking on the Plot Contours icon. Animate the video.

3. Plot the time variation of the reaction force required to compress the seal component. In the main menu, select Result

History output. In the dialog box

select the entry that refers to the reaction force at the set called SET-RP and press the button Plot.


10


11

STRESS RELAXATION TEST IN ABAQUS BY sHAFI DADA.pdf

Recommend Documents