Joint Analysis

  • 1.8K Views
  • Last Post 12 December 2019
  • Topic Is Solved
Mario123 posted this 11 December 2019

Hello,

I'm new in Ansys, I will like to simulate a  compression assembly in static structual analysis, but I don't know how to use joints and contacts correctly in the red circle. Can yo help me please?.

 

Joint Analysis

Best regards.

Order By: Standard | Newest | Votes
peteroznewman posted this 11 December 2019

If you have geometry for three solid bodies, let's call them Crank, Conrod and Piston, and are building this model in 3D, then you have a cylindrical face at the left end of the Crank.  Right mouse click on the Connections folder, Insert, Joint.  In the Details window for the Joint, change it from Body-Body to Body-Ground, and change the type to Revolute. With the Face filter active, click on the cylindrical face and click on the yellow field to fill out the Scope.

Repeat that for the two other joints, but leave it at Body-Body and there will be two yellow fields for Reference and Mobile sides of the Joint. Pick a cylindrical face on the Conrod for the Reference and pick the cylindrical face for the adjacent part for the Mobile side.  It's not important which face is Reference and which is Mobile.

There is a bit more work to do to apply the displacement as shown. If instead you wanted to insert a Joint Load, you could easily enter a rotation angle for any of the joints defined above. The easy way to insert a Joint load is to grab a Joint from the connections folder and drag and drop it on the Static Structural branch of the outline.

The last joint you need is between the Piston and Ground. Make the type Translation.  Pick the left face of the piston. Without any foam, that model will move the parts.

Now look in the Contacts folder. ANSYS may have automatically created some contacts for you. Delete them all.

Tell us more about the foam. If the foam is very soft compared with the three parts above, those bodies can be set to Rigid, greatly speeding up the solution time.

Mario123 posted this 11 December 2019

Thank you, but now have some warnings and I

-Not enough constraints appear to be applied to prevent rigid body motion.  This may lead to solution warnings or errors.  Check results carefully.

-One or more MPC contact regions or remote boundary conditions may have conflicts with other applied boundary conditions or other contact or symmetry regions. This may reduce solution accuracy. Tip: You may graphically display FE Connections from the Solution Information Object for non-cyclic analysis. Refer to Troubleshooting in the Help System for more details.

-Joints are being used in the current analysis with Large Deflection turned Off.  Thus, only linearized joint behavior will be considered.  If finite rotation and large deflection effects are to be considered, please turn on Large Deflection.

-Two or more remote boundary conditions are sharing a common face, edge, or vertex.   This behavior can cause solver overconstraint and is not recommended, please check results carefully.  You may select the offending object and/or geometry via RMB on this warning in the Messages window.

 

peteroznewman posted this 11 December 2019

If you want to squash the foam by more than a small amount, then you do need to turn on Large Deflection.
You find that under the Analysis settings.

Most of the other ones are warnings. Careful selection of faces can avoid all those warnings.

Did you put in a Joint Load? Does it solve?

If it solved, you have to insert a Total Deformation result under the Solution branch of the outline (and click Solve again).

  • Liked by
  • Mario123
Mario123 posted this 11 December 2019

I used Joint load and now I only have this warning:

-Not enough constraints appear to be applied to prevent rigid body motion.  This may lead to solution warnings or errors.  Check results carefully.

But is possible to use a displacement instead joint load?

 

peteroznewman posted this 11 December 2019

Yes, it's possible. I can easily tell you how after you do File, Archive to create a .wbpz file and upload your model.

After you post your reply where you say what version of ANSYS you are using, the Attach button will appear and you can upload the .wbpz file.

Mario123 posted this 11 December 2019

ANSYS 2019 R1

 

Attached Files

peteroznewman posted this 11 December 2019

 

Select the Edge filter, then Ctrl-click on the top edge of the conrod and the bottom edge of the conrod.

Under Static Structural, insert a Remote Displacement. Enter -14 for the Y coordinate, leave all others Free.

Suppress the Joint - Rotation load.  Solve.

By picking the top and bottom edge, the remote point is created at the center of the hole.

If your question has been answered, please click Is Solution to mark the discussion as Solved, or ask a followup question. 

peteroznewman posted this 11 December 2019

You already made them all rigid bodies.

peteroznewman posted this 11 December 2019

In Workbench, you could drag a Rigid Dyanamics analysis and drop it on the Model cell of Static Structural analysis.

In Mechanical, drag the load (joint rotation or displacement) from Static Structural and drop it on the Transient branch. Solve. 

See how much faster it solves?

peteroznewman posted this 12 December 2019

Duplicate the Static Structural model and change all the bodies from Rigid to Flexible and see how long the solution takes.  Much, much longer.

Close