# Spring analysis of door locking mechanism

• 26 Views
• Last Post 26 April 2019
krRahul posted this 25 April 2019

There is an error occurring in my analysis of spring that "The solver engine was unable to converge on a solution for the nonlinear problem as constrained" .I want to know how to solve this error

contact is separated at some point and i am not able to find those problem at contacts.The maximum contact stiffness is too big. This may affect the accuracy of the results. You may need to scale the force unit in the model.
The unconverged solution (identified as Substep 999999) is output for analysis debug purposes. Results at this time should not be used for any other purpose.One or more bodies may be underconstrained and experiencing rigid body motion. Weak springs have been added to attain a solution.  Refer to Troubleshooting in the Help System for more details.

Attached Files

Order By: Standard | Newest | Votes
peteroznewman posted this 25 April 2019

I recommend you drastically reduce the amount of geometry in your model and focus just on the spring arm and the surfaces that press on the spring. By eliminating all the surrounding geometry, you will have a much smaller mesh and the model will run much faster.

Does the spring arm have a constant thickness? If so, while you are in the Geometry editor, take the spring arm and create a midsurface of that arm. The arm will then be meshed with shell elements instead of solid elements. The shell elements will have the correct thickness property. This will give you a very low node count, fast solving model of the spring arm with elements designed to compute bending stresses very efficiently.

The problem looks symmetric, so you could cut the model size in half again by using a symmetry plane. With the above steps you have reduced the model size by 100:1 to the original, so you could forgo this last factor of two, but symmetry does remove 3 of the 6 DOF of the spring to the base, which reduces the number of ways the nonlinear frictional contact can go wrong, so it is probably worth the effort. You would cut the model in half on a plane parallel to the XZ plane.

It looks like there is a square edge on the corner of the bridge that the spring is rubbing on. This is not a good situation for a contact pair to cope with. Add a blend to the geometry so that the spring will be rubbing on a small cylindrical surface instead of a sharp corner. You must have the solid model of the spring arm tangent to that blend in CAD before you transfer over the geometry. It's okay that there will be a 1/2 wall thickness gap to the midsurface in the geometry, see next paragraph.

Pick that blend face, and the underside of the bridge and put those on the Contact side of the contact pair, and put the spring face on the Target side of the contact pair. When you mesh the bridge part, make sure to put at least 6 elements around the blend.  You will also want to set Shell Thickness Effect to Yes. Add a Contact Tool under the Connections folder and make sure the Frictional Contacts are closed. If the contact is open by a tiny gap, set the Interface Treatment to Adjust to Touch.

Under Analysis Settings, you must set:

• Large Deflection On
• Auto Time Stepping On
• Initial Substeps 100

You can revise the Inital Substeps after you see some converged iterations.

Under the Solution Information folder, on the Newton-Raphson Residuals line, type the number 3.  You may need to look at these plots if it fails to converge.

You want this model to be a displacement driven model. I don't know what the force in your model is pushing on, but don't use force to move the slider, use displacement.

krRahul posted this 26 April 2019

Thank you for providing me with such details and i hope it works.