Abaqus Tutorial 26 Three point bending

Prévia do material em texto

Simuleon B.V. 
Sint Antoniestraat 7 5314 LG Bruchem 
T. +31418644-699 E. info@simuleon.nl W. www.simuleon.nl 
 
Three point bending: general 
contact and contact pairs. 
 
 
 
 
 
 
 
 
 
 
Simuleon B.V. 
Sint Antoniestraat 7 5314 LG Bruchem 
T. +31418644-699 E. info@simuleon.nl W. www.simuleon.nl 
1. Introduction 
 
The first exercise of this contact event will show you the two main approaches 
available in Abaqus to include interactions within your model: the general 
contact and the contact pairs approaches. 
Main difference among the two approaches is the way the contact is defined. 
Furthermore, there are other minor differences related to the numerical solution 
of the contact and some specific restrictions for each of the approaches. 
 
- General contact allows you to define contact in your entire model with only 
one-click and it is generally a very fast process. 
 
- Contact pairs approach requires you to define a new interaction for each 
surface pair you want to include in the model. This could become really 
complicated and time-consuming if you have a large assembly. However, 
sometimes, it is the only option if you have for instance analytical surfaces in the 
model. 
 
In this example, a metallic beam modelled with plastic material properties will 
undergo a three point bending loading condition enforced through contact with 
three rigid tools. 
 
The model will be already pre-defined in terms of geometry, meshing and 
boundary conditions. Your only task will be to define the interactions with the 
two approaches provided by Abaqus, run the analyses and post-process the 
data. 
 
 
2. Preliminaries 
 
- Double click on the file Contact1.cae, this will open an Abaqus database where 
you will already find a model called Model-GC including the geometric parts, the 
instance positioning in the assembly and the discretization of the parts. 
 
- The model (Figure 1) is actually a quarter of the model shown in the title page 
to exploit the symmetry occurring in the X-Y and Y-Z planes and reduce the cost 
of the analysis. 
 
Figure 1. Assembly of the three point bending moment. 
 
Simuleon B.V. 
Sint Antoniestraat 7 5314 LG Bruchem 
T. +31418644-699 E. info@simuleon.nl W. www.simuleon.nl 
3. Material and section properties 
 
- Start to define the material properties by clicking on Materials in the model tree. 
In the Edit material dialog box, type Steel as material name and select 
Mechanical Elasticity  Elastic as material behaviour in the material menu. 
Enter 210e3 MPa as Young’s modulus and 0.3 as Poisson coefficient. Select 
Mechanical PlasticityPlastic and enter the values shown in the following 
picture to define the plastic behaviour of the material. 
 
 
 
- Now create a new solid homogeneous section called Section_Steel by 
clicking on Sections in the model tree. Choose Steel as material and click OK. 
 
 
 
Simuleon B.V. 
Sint Antoniestraat 7 5314 LG Bruchem 
T. +31418644-699 E. info@simuleon.nl W. www.simuleon.nl 
- Assign the section to the beam. In the model tree, explode the Parts container, 
explode the part called Beam and double-click on Section Assignment. Select 
the whole geometry of the beam and select the Section called Section-Steel. The 
part should turn from grey to green. Rigid tools do not need to have any material 
assigned. 
 
 
 
 
- Double click Assembly in the model tree, and click on the View Mesh Icon and 
check the assembly and its already predefined mesh. 
 
 
 
 
Simuleon B.V. 
Sint Antoniestraat 7 5314 LG Bruchem 
T. +31418644-699 E. info@simuleon.nl W. www.simuleon.nl 
4. Define the analysis steps 
 
- Double-click on Steps in the model tree and create a new Static, General step 
called Load. Set Nlgeom parameter as on and include automatic stabilisation as 
shown in the following picture. 
 
 
 
 
 
- Move to the incrementation tab and set an initial time increment of 0.01 and a 
maximum of 0.05. 
 
 
 
 
 
- Create a second step called Elastic Return using the same procedure and the 
same parameters as the first step. 
 
 
 
 
 
Simuleon B.V. 
Sint Antoniestraat 7 5314 LG Bruchem 
T. +31418644-699 E. info@simuleon.nl W. www.simuleon.nl 
5. Define boundary and loading conditions 
 
Four boundary conditions are applied to this model. 
 
- Define a Symmetric displacement condition to the beam in the x direction. 
Double click on BCs in the model tree, call the boundary condition as BC-SYMM-
X, select Initial as step and Symmetry/Antisymmetry/Encastre as type. Select the 
face highlighted in the following Figure as region and then X-SYMM as type. 
 
 
- Repeat the same to create a BC-SYMM-Z boundary condition (Z-SYMM) in the 
face of the beam shown below. 
 
 
 
 
 
Simuleon B.V. 
Sint Antoniestraat 7 5314 LG Bruchem 
T. +31418644-699 E. info@simuleon.nl W. www.simuleon.nl 
- Create now a new Boundary condition called BC-Encastre to encastre the 
lower rigid tool. Select Initial as step and Symmetry/Antisymmetry/Encastre as 
type. Select the reference point of the lower rigid body as region and then 
ENCASTRE as type. All the nodes of this part will follow the movement of this 
node, thus the whole part will be fixed to its initial position. 
 
 
 
 
- Lastly, create a Displacement/Rotation boundary condition called BC-DISP. 
Select Load as step, Displacement/Rotation as type, select the reference point of 
the upper rigid body and enter the parameters as shown in the following picture. 
 
 
 
Simuleon B.V. 
Sint Antoniestraat 7 5314 LG Bruchem 
T. +31418644-699 E. info@simuleon.nl W. www.simuleon.nl 
- Enter now the Boundary Conditions manager (in the model tree, right click on 
BCs and select Manager). Select the cell belonging to the Elastic return step 
column and the BC-DISP row. Click on Edit and replace -35 with 0 in the U2 
field. This will return the rigid tool to its original position. 
 
 
 
- Save the model. File  Save. 
 
6. Define Interactions using General Contact approach 
 
- Create new Interaction Property by double-clicking Interaction Properties in 
the model tree, call it IntProp-1 and select Contact as Type. Select Hard contact 
for Mechanical Normal Behaviour. Select MechanicalTangential 
Behaviour, select Penalty as Friction formulation and enter 0.1 as friction 
coefficient. 
 
 
 
Simuleon B.V. 
Sint Antoniestraat 7 5314 LG Bruchem 
T. +31418644-699 E. info@simuleon.nl W. www.simuleon.nl 
- Create now a new General Contact interaction. Double click on Interactions, 
select Initial as Step, call the new interaction as INT-GC and choose General 
Contact as type. Keep All with self as contact domain to say that you want all 
the parts of your system in contact with everything. Select IntProp-1 as global 
interaction property. 
 
 
 
 
Interactions defined with general contact are very fast to be implemented (only 
two clicks also for complex models). It is still possible, if needed, to improve the 
definition by including/excluding specific surface pairs or by assigning 
individual interaction properties to particular surface pairs. 
 
7. Create and Submit a Job 
 
- Double-click Jobs in the model tree and create a new Job called Contact1-GC. 
Select the Model-GC and click Continue and then ok. Now, right-click on Jobs 
and open the Job-Manager. Highlight the job Contact1-GC previously created 
and click on Submit to start your analysis and on Monitor to monitor the 
advancement of the analysis. Once it is terminated click on Results in the Job-
Manager. 
 
Simuleon B.V. 
Sint Antoniestraat 7 5314 LG Bruchem 
T. +31418644-699 E. info@simuleon.nl W. www.simuleon.nl 
 
 
 
8. View the Results 
 
- Visualize the complete model. In the main menu bar, click on View  Odb 
Display options and enter the Mirror/Pattern tab. Tick the XY and YZ mirror 
planes to mirror the model and exploit the symmetry of the system. Click OK. 
 
 
 
 
 
 
 
 
 
 
 
 
Simuleon B.V.Sint Antoniestraat 7 5314 LG Bruchem 
T. +31418644-699 E. info@simuleon.nl W. www.simuleon.nl 
- Visualize the displacement and the stress contour plots. Animate the analysis 
using the tools highlighted in the following picture. Then return on the model tree 
bu clicking on the Model tab on top on the left. 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
Simuleon B.V. 
Sint Antoniestraat 7 5314 LG Bruchem 
T. +31418644-699 E. info@simuleon.nl W. www.simuleon.nl 
9. Define Interactions using the Contact-Pair approach 
 
It is possible to define interactions in a different way. The Contact Pairs 
approach is more time-consuming but it allows sometimes a wider range of 
interaction properties (rough friction), contact domains (include analytical rigid 
surfaces, spheres, cylinders) and contact formulations (node-to-surface). General 
contact is more limited. 
 
- Copy the Model-GC by right-clicking on Model-GC in the model tree and 
selecting Copy Model. Rename the new model as Model-CP. 
 
- Explode the new model and collapse the Model-GC. Go in the Interactions 
container and delete Int-GC from Model-CP (Right-click and Delete). 
 
- Now define two new interactions between the beam and the two rigid tools. 
Double-click on Interactions, name the interaction Int-Upper, select Inital as step 
Surface-to-Surface contact as type. Select the upper rigid tool as master 
surface, choose the colour (brown or purple) that faces the beam to define the 
shell surface. Select Surface as slave region and select the upper face of the 
beam as shown in the following picture. 
 
- Once the Edit Interaction dialog box appears, choose IntProp-1 as interaction 
property and click OK. 
 
- Repeat the same for the second rigid tool and create the Int-Lower contact pair. 
 
 
 
 
 
 
Simuleon B.V. 
Sint Antoniestraat 7 5314 LG Bruchem 
T. +31418644-699 E. info@simuleon.nl W. www.simuleon.nl 
- Double-click Jobs in the model tree and create a new Job called Contact1-CP. 
Select the Model-CP and click Continue and then ok. If not already open, right-
click on Jobs and open the Job-Manager. Highlight the job Contact1-CP 
previously created and click on Submit to start your analysis and on Monitor to 
monitor the advancement of the analysis. Once it is terminated click on Results 
and check them as done in the previous section. Results should be the same. 
 
10. Use the automatic Find contact pair tool 
 
As highlighted earlier, the contact pair approach could be very time-consuming in 
case of large models and analyses. A new interaction is define for each contact 
pair. Sometimes it is not even possible to know which surface will undergo 
contact. Abaqus offers a tool to overcome this issue to automatically find 
contact pairs and define new interactions. 
 
- Copy the Model-Cp as Model-CP-AUTOM as did before. Delete the two 
interactions previously created. 
 
- Click the Find Contact pairs icon as highlighted in the following picture and 
then click the Find Contact Pairs button. Notice that two contact pairs are found, 
the Intprop-1 has already been selected as default. All the options in the cells 
can be modified specifically. Click ok and notice that in the model tree, two new 
Surface-to-Surface interactions have been selected. 
 
 
 
 
 
 
 
Simuleon B.V. 
Sint Antoniestraat 7 5314 LG Bruchem 
T. +31418644-699 E. info@simuleon.nl W. www.simuleon.nl 
- Double-click Jobs in the model tree and create a new Job called Contact1-CP-
AUTOM. Select the Model-CP-AUTOM and click Continue and then ok. Without 
opening the Job Manager, you can also right-click the Job Contact1-CP_AUTOM 
and select Submit to start your analysis and Monitor to monitor the advancement 
of the analysis. Results can be accessed with this method as well.