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
You are navigating away from the AIS Discovery experience