Sign-up for free online course on ANSYS simulations!Step 7: Solve!
As mentioned in step 1, the definition of initial contact is perhaps the most important aspect of building a contact analysis model. Before we start the solution, we'll verify the initial contact status. Issue the following command in the ANSYS Command Input window: *******cncheck
This feature lists the initial status of contact pairs and provides a summary of the contact problem we have set up. Note that an initial penetration of 1E-5 has been detected. This is consistent with the value of parameter inter=1e-5, which we set up at the beginning of the tutorial. Also, note that 1 contact pair is selected.
Define Solution Control Options
We'll specify the analysis option as a static analysis in which large deformation effects are to be included. To do this, we'll use the Solution Controls menu.
*Main Menu > Solution > Analysis Type > Sol'n Controls
This brings up the Solution Controls menu. Select Large Displacement Static for Analysis Options. Under Time Control, enter 100 for Time at end of loadstep and select from the off Automatic time stepping drop-down menu. Click OK.
Solve
We are now ready to solve:
Main Menu > Solution
Issue check in the ANSYS Command Input window. If the problem has been set up correctly, there will be no errors or warnings reported. If you look in the Output window, you should see the message: The analysis data was checked and no warnings or errors were found.
Main Menu > Solution > Solve > Current LS
Review the information in the /STATUS Command window. Close this window. Click OK in Solve Current Load Step menu.
ANSYS performs the solution and a yellow window should pop up saying "Solution is done!". Close the yellow window. You should get the following screen, which shows that the solution has converged.
Verify that ANSYS has created a file called diskscontact.rst in your working directory. This file contains the results of the (previous) solve.