Transcript Workshop 1A Basics - Applied Mechanics Research Group

Workshop 7A
Diagnostics Tools for
Surface Body Contact
Workbench-Mechanical
Structural Nonlinearities
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-1
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
Workshop 7A: Diagnostics
Workshop Supplement
• Goal
Diagnose convergence trouble with surface body contact model
• Model Description
–
–
–
–
–
–
3D Spring plate –Surface Body
3D Rigid Target Body
Linear steel material
Meshed with 3D SHELL elements
Spring Fixed support at one end, A
Rigid Body displaced into Spring 19mm
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-2
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
Steps to Follow:
• Start an ANSYS Workbench session. Browse for and open
“W7a-contact-diagnostics.wbpj” project file.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-3
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
The project Schematic should look like the
picture to the right.
– From this Schematic, you can see that the
Engineering (material) Data and Geometry have
already been defined (green check marks).
– It remains to set up and run the FE model in
Mechanical
– Highlight the Engineering Data Cell and open by
clicking on the Right Mouse Button
(RMB)=>Edit to verify the linear material
properties.
– Verify that the units are in Metric(Tonne,mm,..)
system. If not, fix this by clicking on…
• Utility Menu=>Units=>Metric(Tonne, mm,..)
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-4
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
• Return to Project Schematic
– Utility Menu > Return to Project
• Double click on the Model Cell to open the FE Model (Mechanical
Session) (or RMB=>Edit…)
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-5
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
•
Workshop Supplement
Once inside the Mechanical application, verify the working unit system
– “Unit > Metric (mm,kg,N,s,mV,mA)”
•
•
The spring assembly is already set up with frictionless contact pairs, a fixed
boundary condition and a displacement load on the rigid component.
Highlight the entities beneath each folder to become familiar with the model
and to confirm that it is properly supported and loaded and ready to solve.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-6
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
• Confirm the Analysis Settings Specifications as
shown:
• Run the Solution…
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-7
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
• After solution run is complete, highlight the Solution Information
folder and scroll to near the bottom of the output.
– Even with the frictionless contact defined and with auto time stepping
and large deflection turned On, and plenty of substeps, this solves in
one iteration!
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-8
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
• Review the Total Deformation results.
– Something is wrong. The contact relationship between the two parts
has obviously failed.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-9
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
With 25 initial substeps and Auto Time Stepping turned On, the contact should
have engaged. In an effort to determine the problem, we will evaluate what the
initial condition of the contact pairs are.
• Highlight the Connections Folder: RMB> Insert> Contact Tool
• Highlight the Contact Tool: RMB>Initial Information>Generate Initial Contact
Results. This will run a partial solve to establish initial contact parameters
(i,e. Initial status, gap, penetration, etc…).
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-10
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
• Review the Initial Contact Information.
• Note the following:
– The two active pairs both have an initial status of “Far Open”
– Both pairs have a pinball radius of 4mm. Is 4mm enough?
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-11
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
• By studying a profile of the undeformed geometry we can see that the
initial gap is less then 1.50mm. Hence, the Pinball Radius of 4mm should
be sufficient for this contact pair to be in an initial status of ‘near-open’.
Rigid Target
Spring
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-12
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
• Highlight the contact region representing the contact between the
spring and target.
– In order for contact to work properly, the contact element normals must
be facing the target element normals.
– Recall that surface bodies are meshed with shell elements that have a
‘top’ and a ‘bottom’ face. The reason this contact pair is not working is
because the contact normals are on the wrong side of the surface body
with normals that face away from the target. This needs to be reversed.
Target element
normal direction
Contact element
normal direction
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-13
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
• From the details window of the contact region, switch the ‘contact shell face’
from Bottom to Top . The red color highlighting the contact side should
switch.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-14
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
• Highlight the Solution Information Branch
–
–
Set Newton-Raphson Residuals = 3
This will save force imbalance data for the
last ‘3’ Newton-Raphson iterations. This is
especially helpful information for
troubleshooting troubling contact
convergence problems.
• Rerun the solution
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-15
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
• From the Solution Information Branch, the contact is now
engaging, but the solution fails to converge after several iterations.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-16
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
These first two converged substeps likely represent the trivial solutions
that occur as the small gap between the two parts is being closed and no
contact has been made yet.
This first spike in the Newton-Raphson
residual (measure of imbalance) likely
occurs at the point when contact first
engages. From there on out, the solution
struggles and fails after two bisections
and many iterations to find a balance.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-17
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
A plot of Newton-Raphson Residual (measure of force imbalance in the model)
confirms that the point where contact is engaged is the source of the highest
imbalance .
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-18
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
• Highlight both Contact Regions and change the
contact specifications in the details window.
Augmented Lagrange is
recommended for general
contact
Reducing the contact
stiffness factor will reduce
the calculated force
generated at the contact
surface and thereby reduce
the imbalance
• Re-run the solution
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-19
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
The solution now converges very nicely with no bisections
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-20
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
• Review the Total Deformation results.
– Although this solution is now converged, notice the excessive
penetration. This is because, by default the shell contact detection
points are at the midplane of the shells.
– This can be remedied by adding a command object to the contact
elements with the following command: KEYOPT,cid,11,1 (refer to
Element manual documentation on CONTA174 and the KEYOPT
command)
– This command will include an adjustment for the shell thickness.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-21
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
EXTRA CREDIT !!
• Highlight each Contact Region
and RMB > Insert > Commands
– Inside the command object and
type the command as shown
*
to Element Reference documentation on
* Refer
CONTA174 along with Command Manual
documentation on ‘KEYOPT’
• Re-run the solution
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-22
April 30, 2009
Inventory #002660
Workbench Mechanical – Structural Nonlinearities
… Workshop 7A: Diagnostics
Workshop Supplement
• Review the Total Deformation results as before.
– Shell thickness is now properly accounted for.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS7A-23
April 30, 2009
Inventory #002660