The reason is given in the WARNING
What can you do to avoid switching from Iterative to Sparse solver? Don't use u-P formulation. Don't use MPC184 elements using Lagrangian multiplier. Don't use constraint equations.
Every contact pair is given a number before it is sent to the solver. These numbers are called real constants. The numbering is arbitrary. When a stiffness matrix is assembled, the dimensions are large. If the number of DOF in the model is N, then there are NxN entries in the stiffness matrix, but most of them are zero, which is why it is called a sparse matrix. There are special direct methods to invert a spare matrix. If you had a cantilever beam and meshed it with 100 beam elements, that would be a 600x600 stiffness matrix because each node has 6 DOF. The nonzero entries in the stiffness matrix are organized to be as close to the diagonal as possible. The width of the nonzero entries is called the wavefront. In the case of a beam element, where each node only touches 2 elements, that has the smallest wavefront. The larger the wavefront, the more memory is required while inverting the matrix. When you add a Remote Displacement and scope it to many nodes, that increases the wavefront.
This warning says that the element connects one node to node 0, which is a grounded node. If this is not what you wanted, then you could take action to change the model to make it the way you intended. Having unintentional connections to ground can ruin a model's results since a ground connection adds a boundary condition that can greatly affect the result.
The memory resident database can be ignored. It is a small amount of memory that is automatically managed by the solver, so pay it no further attention.
Remote points are internal nodes, which are also called pilot nodes. They are needed to apply remote forces or remote displacements.
You have about 4 million elements total, but you and 2 million nodes. If the nodes are on solid elements, each node has 3 DOF so there would be about 2x3 = 6 million DOF in the model.
Look for a table like this in your model:
That is where it tells you how many contact elements were added to the solid elements that you created.
What is the difference between Workspace and Database? ANSYS automatically manages memory so you don't need to interfere with it. If you run out of RAM, reduce the model size or install more RAM. Trying to override the ANSYS settings can, in rare circumstances, get a model to run without doing either of those things, but more frequently leads to failure.