Solver pivot warning

  • Last Post 03 July 2018
  • Topic Is Solved
thanhttdt posted this 23 June 2018

Hi everyone, when I practiced as a tutorial 


there was an error (see picture).

Could you please give me some instruction to solve this problem?

I also attached project file here for more detail

Thanks in advance,

Order By: Standard | Newest | Votes
peteroznewman posted this 23 June 2018


The problem is the ribs are not connected to the plate. You can see this in Mechanical where the free edges are colored red.

There are several ways to correct this. One way is in SpaceClaim, to use Shared Topology. In SpaceClaim, here is the current setting:

Change Share Topology to Share.

Now the mesh shows that the nodes along the intersection of the plate and ribs have "triple" connections. This is what you want.

The solver will now solve.

ANSYS 18.2 archive attached.

Attached Files

  • Liked by
  • thanhttdt
thanhttdt posted this 25 June 2018

Hi peteroznewman 

Thanks for your kind support and very clear illustration. 

Best Regards,

kcao posted this 03 July 2018


Some general explanations on what "pivot error" means in FEM.

The pivot or pivot element is the element of a matrix, or an array, which is selected first by an algorithm (e.g. Gaussian elimination, simplex algorithm, etc.), to do certain calculations. In the case of matrix algorithms, a pivot entry is usually required to be at least distinct from zero, and often distant from it. (source: A negative or zero equation solver pivot value usually indicates the existence of a singular matrix with which an inderminate or non-unique solution is possible. In ANSYS when a negative or zero pivot value is encountered, the analysis may stop with an error message or may continue with a warning message, depending on the various criteria pertaining to the type of analysis being solved. You may also read ANSYS Help > Mechanical APDL > Basic Analysis Guide > Solution > Singular Matrices to access more details.