March 23, 2023 at 6:03 pm

peteroznewman

Subscriber

I misunderstood at first, but now I am onto your question, which has nothing to do with material mass density, but element size!

A relevant question, are you using the recommended default of Distributed Ansys?

If so, insert the following Command into the Static Structural section of your model.

DSPOPTION,,,,,,PERFORMANCE

Put that command in each static structural model and solve. That will cause the Solution Output to contain all the performance data generated during the solution.

The Direct solver, also called a Sparse Solver, means that once the stiffness matrix is assembled, most of the values in the matrix are zeros and the number of non-zero values in the matrix is an important characteristic on how many floating point operations are required, see the output below. I didn’t make two models have an identical number of nodes, but I made them close enough as you can see in the number of equations.

When a stiffness matrix is created, the solver reorders the rows to optimize the matrix inversion. That reordering puts non-zero numbers near the diagonal and keeps the far-off diagonal values as zeroes. The more connections an element has to other elements increases the width of non-zero values near the diagonal. A model with beam elements arranged in a single line has the minimum width of non-zero values about the diagonal. 3D solid elements have a much wider set of non-zero values about the diagonal. This is called the bandwidth of a matrix. It seems that the sparse matrix is being strongly affected by the connections between the elements when the mesh is less uniform.

There are many methods to solve sparse linear systems. Section 10 of this paper describes Frontal Methods. Maybe that is relevant when you look in the solution output below and you can see the maximum size of a front matrix which is 6.5 million for the uniform mesh and 27.8 million for the non-uniform mesh.

Below are sections from the two Solution Output files, labelled with the two types of mesh.

UNIFORM MESH

===========================

= multifrontal statistics =

===========================

number of equations = 179178

no. of nonzeroes in lower triangle of a = 6694203

no. of nonzeroes in the factor l = 96111205

ratio of nonzeroes in factor (min/max) = 0.8874

number of super nodes = 6267

maximum order of a front matrix = 3597

maximum size of a front matrix = 6471003

maximum size of a front trapezoid = 4566471

no. of floating point ops for factor = 1.2764D+11

Solver Memory allocated on core 0 = 331.057 MB

Solver Memory allocated on core 1 = 304.230 MB

Solver Memory allocated on core 2 = 308.788 MB

Solver Memory allocated on core 3 = 293.040 MB

Total Solver Memory allocated by all cores = 1237.114 MB

DSP Matrix Solver CPU Time (sec) = 5.078

DSP Matrix Solver ELAPSED Time (sec) = 5.101

DSP Matrix Solver Memory Used ( MB) = 331.057

EQUIL ITER 1 CPU TIME = 6.797 ELAPSED TIME = 6.454

NON-UNIFORM MESH

===========================

= multifrontal statistics =

===========================

number of equations = 181173

no. of nonzeroes in lower triangle of a = 7717884

no. of nonzeroes in the factor l = 231164534

ratio of nonzeroes in factor (min/max) = 0.8010

number of super nodes = 5671

maximum order of a front matrix = 7458

maximum size of a front matrix = 27814611

maximum size of a front trapezoid = 15050733

no. of floating point ops for factor = 8.0454D+11

Solver Memory allocated on core 0 = 769.905 MB

Solver Memory allocated on core 1 = 763.813 MB

Solver Memory allocated on core 2 = 672.730 MB

Solver Memory allocated on core 3 = 638.205 MB

Total Solver Memory allocated by all cores = 2844.652 MB

DSP Matrix Solver CPU Time (sec) = 21.734

DSP Matrix Solver ELAPSED Time (sec) = 21.757

DSP Matrix Solver Memory Used ( MB) = 769.905

EQUIL ITER 1 CPU TIME = 23.75 ELAPSED TIME = 23.44