Introduction
In this exercise, we will duplicate the three-point bending test required in ASTM D638 for plastic material flexural testing. Our analysis will feature a section of polymer (acrylonitrile butadiene styrene) subjected to a uniform stress (uniaxial tension test) in a test rig. We will setup a nonlinear material model, and will intentionally over-deform the beam into the apparent nonlinear and post-yield range of the material. Finally we will unload the test bar to look for permanent deformation.
It is important to note that some polymers behave differently in tension and compression. In such materials, the Flexural Modulus = Average Modulus. Nonlinearities cause stress redistribution during bending, meaning that linear calculations are no longer valid.
To reduce simulation time, we will use quarter symmetry of the model.
1. Open the Model and Start the
Autodesk Inventor Nastran Environment
Start Autodesk Inventor, and open
Flex Test.iam from the
Section 19 - Flex Test Fixture sub-folder of your training exercises folder. (Get Started > Launch > Open)
From the ribbon, click the
Environments tab, and click
Autodesk Inventor Nastran.
You should see this:
In the Model tree, expand
Idealizations. If any Idealizations are already defined, like Solids 1 and 2 below, right-click
, to ensure that no unwanted materials can participate in the analysis.
2. Change the Analysis Type
- From the Analysis tree, right-click
.
- On the Analysis dialog, set the
Type to
Nonlinear Static.
- On the Options tab, verify that
Large Displacements is
On.
- On the Output Controls tab, Output Sets group, make sure that
Stress and
Strain are checked.
- Click
OK.
Because stress-strain curves for plastic materials often have shallow slopes in the plastic region, it is preferable to view results in terms of strain.
3. Assign the Alloy Steel Property
- Click
Idealizations from the ribbon.
- Click the
New Material
icon.
- On the Material dialog, click
Select Material. Expand the Inventor Material Library, and select
Alloy Steel. Click
OK and
OK to close the two Material dialogs.
- In the Idealizations dialog, check the
Associated Geometry box.
- Select the load pin and the support parts.
- Click
OK.
4. Assign and Define the Nonlinear ABS Material
The typical ABS stress-strain curve (from Matweb Averages) looks like this:
- Click
Idealizations from the ribbon.
- Click the
New Material icon.
- On the Material dialog, click
Select Material. Expand the Inventor Material Library, and select
Acrylonitrile Butadiene Styrene. Click
OK.
- In the Material dialog, set the value of
E to
1265 MPa.
- Click
Nonlinear.
- On the Nonlinear Material Data dialog, set the
Type to
Plastic.
- Make sure the
Hardening Rule is set to
Isotropic.
- Set the
Initial Yield Stress to
43 MPa.
- In the table, double-click in the
Strain column in the first open row, and enter
0.5. (This is 50%.)
- Click in the adjacent
Stress cell, and enter
43.
- Click
Show XY Plot.
- Click
OK twice.
- Check the
Associated Geometry box.
- Select the test part.
- Click
OK.
5. Apply the Y Symmetry Constraint
- Click
Constraints from the ribbon.
- Click
Y Symmetry.
- Click the faces shown.
- Click
OK.
6. Apply the X Symmetry Constraint
- Click
Constraints from the ribbon.
- Click
X Symmetry.
- Click the faces shown.
- Click
OK.
7. Apply the Fix Constraint to the Support Pin
- Click
Constraints from the ribbon.
- Click
Fixed.
- Click the face shown.
- Click
OK.
8. Apply a Pushing Constraint
The pin loading will push the center of the beam through a defined displacement. This enforced displacement is defined as a combination of this constraint and a pushing load that we will define in the next step.
- Click
Constraints from the ribbon.
- Make sure all degrees of freedom are unchecked except for
Tz.
- Click the face shown.
- Click
OK.
9. Apply the Pushing Load
- Click
Loads from the ribbon.
- Set the
Type to
Enforced Motion.
- Set the
Sub Type to
Displacement.
- Set the
Tz value to
-3.
- Select the face shown.
- Click
OK.
10. Define Contacts
- Click
Automatic from the Contacts panel in the ribbon.
- From the Analysis tree, expand the Surface Contacts branch, right-click on the first contact, and click
Edit.
- Change the
Contact Type to
Separation.
- Specify
20 as the
Max Activation Distance.
- Click
OK.
- Repeat steps 2-5 for the second contact.
11. Mesh the Model
- Click
Mesh Settings from the Mesh panel in the ribbon.
- Set the
Element Order to
Linear.
- Uncheck
Continuous Meshing.
- Click
OK to close the dialog and generate the mesh.
-
- From the Analysis tree, right-click
.
- Enter
2 for the Face Data
Element Size.
- Click in the
Selected Faces box, and select the four contact surfaces.
- Click
OK.
- In the Analysis tree, right-click
.
12. Add a "Release" Subcase
- Right-click
.
- Name the subcase
Release.
- Select the four existing constraints.
- Click
OK.
13. Add a Release Load to the Release Subcase
- In the
Release subcase, right-click
.
- Set the
Type to
Enforced Motion.
- Set the
Sub Type to
Displacement.
- Set the
Tz value to
3.
- Select the face shown.
- Click
OK.
14. Define the Nonlinear Setup
In this step we will enable intermediate output. This provides output data for each load increment.
- In Subcase 1, right-click
.
- Set
Intermediate Output to
On.
- Click
OK.
- Repeat for the
Nonlinear Setup 2 subcase.
15. Run the Model
- Click
Run from the ribbon.
Subcase 1 will solve for 10 load steps.
Subcase 2 will use the results from Subcase 1 as its initial conditions.
16. View the Nonlinear Displacement Results
- From the Analysis tree, right-click
.
- Select
INCR 10, LOAD = 1.0 from the Subcases menu.
- Select
Displacement from the Result Data list, and set the Type to
Total.
- Click the
Visibility Options tab, and click
Hide All.
- Click
Display.
17. View the Nonlinear Strain and Plastic Strain Results
- Click the Contour Options tab, then select
Strain from the Result Data menu, and set Type to
SOLID VON MISES STRAIN. Click
Display if the results are not showing.
- Change Type to
SOLID EFFECTIVE STRAIN-PLASTIC/NONLINEAR ELASTIC.
Plastic strain is the strain accumulated beyond the yield strain. Because very little plastic strain is accumulated, permanent deformation to the beam is unlikely.
18. View the Final Deformation
- Change the
Subcase to
INCR10, LOAD=2.0
- Change the Result Data to
Displacement.
- Click
Probes from the ribbon, and hover over the end of the beam.
- Click
OK.
We can see that there is very small amount of permanent displacement in the beam.
19. Create a Multi-Set Animation
- Right-click on
Results, and click
Multiset Animation Settings.
- Set
Start Set to
INCR 1, LOAD = 0.1.
- Set the
End Set to
INCR 10, LOAD = 2.0.
- Click the
Deform Options tab. Set the
Deformation Scale to
Actual, and the
Value to
1.0.
- Click the
Visibility Options tab, and click
Hide All.
- Click
Animate.
To stop the animation, right-click
Results and uncheck
Multiset Animate.
20. Determine the Force Required to Bend the Beam
- Right-click on the push constraint from Subcase 1, and select
SPC Summation. (If you did not name your constraints, click on each until you identify the one assigned to the top of the pin.)
- Select
INCR 10, LOAD = 1.0 as the Subcase.
- Note the
Total Force reported.
- Click
Close.
Summary
In this exercise, we defined a nonlinear material. If we had run this analysis as linear, we would have seen severe nonlinearities that don't appear as severe with the full nonlinear analysis. It is important to understand that even though nonlinear analyses can take longer to solve, running nonlinear is often more physically realistic than running the analysis as linear.