Learning Forum

[zachary.brown]

I'm new to ansys and struggling to get my simulation to solve for an analysis on a Hirth joint. I am attempting to simulate a overhung impeller connected to a drive shaft via a Hirth. I would like to be able to utilize a frictional or frictonless connection at the Hirth joint. Even running a simplified case, I get errors regarding the internal solution magnitude limit being exceeded - except when running a bonded or "no separation" contact between the two bodies joined by the Hirth connection. Is there a support I should be using that could solve my problem? I would prefer to not have the body supported using a fixed support, as I plan on simulating thermal expansion as well. 

The problem persists when using both a fixed support on the end of the body and when using a combination of cylindrical and displacement supports. Any help would be greatly appreciated.

Here is an image of my setup:

The node accomanying the error seems unproblematic:

[peteroznewman]

Whenever you use a frictional or frictionless contact, it is important to insert a Contact Tool under the Connections folder.  Then Generate Initial Contact Status.  Look in the worksheet to see if the contact is Closed. If it is Near Open or Far Open, that can cause the problems you are seeing.  The corective action is to make sure the contact is closed. One method to do that is to insert a geometric treatment on the contact which is Adjust to Touch.  This moves the contact elements so that they become initially closed.

You may also need to change the Analysis Settings to turn on Automatic Time Stepping and to set the Initial and Minimum Substeps to 10 or higher and to turn on Large Deflection.

[zachary.brown]

Thank you sir. Conact was near open and the adjust to touch worked perfectly.