TAGGED: anysmechanical


March 22, 2023 at 2:19 pmpiknockyouSubscriber
Hello.
I have computed a "similar" structural model in 2 different ways.
I would appreciate it, if you could explain the significant discrepancies in computational cost regarding memory and CPU time between the 2 "similar" models.
The geometry is identical.
The boundary conditions and analysis settings are identical (e.g., load steps: 1, solver: direct).
No nonlinearities available, thus, iterations/convergence are irrelevant.
No adaptive meshing.
The type of elements is identical (quadratic tetrahedras).
The number of nodes is the same.
The number of elements is the same.
The number of equations/DOFs are the same.
The computations were done incore & on a CPU with 4 cores.
The most significant difference between the 2 models is, in fact, the ELEMENT DENSITY:
Model 1: a homogeneous element density is distributed over all the volume (fine).
Model 2: a homogeneous element density is distributed over all the volume (coarse), except for one location where the mesh density is extremely high incl. a small growth rate.
In the solve.outs, one can see the computational cost of the matrix factorizations comparing Model 1 to 2: 4 vs 12 lines.
Comparing Model 1 to 2, there is over 6x the CPU time and over 3x the memory usage (incore) necessary.
With my limited knowledge of FEM theory, I would have intuitively estimated that similar computational effort would be required, if the same number of nodes, elements, equations/DOFs, and other identical boundary conditions are present.
However, my intuition appears to be entirely incorrect.
Therefore, I would be very grateful if you could explain to me:
Why do varying "arrangements" of element densities lead to such huge discrepancies in computational cost?
Thank you!

March 22, 2023 at 6:20 pmpeteroznewmanSubscriber
What type of analysis was performed?

March 23, 2023 at 8:03 ampiknockyouSubscriber
Static Structural

March 23, 2023 at 12:14 pmpeteroznewmanSubscriber
What is the acceleration load?

March 23, 2023 at 1:48 pmpiknockyouSubscriber
25000 mm/s²

March 23, 2023 at 6:03 pmpeteroznewmanSubscriber
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,,,,,,PERFORMANCEPut 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 nonzero 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 nonzero numbers near the diagonal and keeps the faroff diagonal values as zeroes. The more connections an element has to other elements increases the width of nonzero values near the diagonal. A model with beam elements arranged in a single line has the minimum width of nonzero values about the diagonal. 3D solid elements have a much wider set of nonzero 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 nonuniform 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 = 6.454NONUNIFORM 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 must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Ansys Blog
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
 Solver Pivot Warning in Beam Element Model
 Saving & sharing of Working project files in .wbpz format
 Understanding Force Convergence Solution Output
 An Unknown error occurred during solution. Check the Solver Output…..
 What is the difference between bonded contact region and fixed joint
 User manual
 The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
 whether have the difference between using contact and target bodies
 material damping and modal analysis
 Colors and Mesh Display

5290

3311

2471

1308

1016
© 2023 Copyright ANSYS, Inc. All rights reserved.