

September 20, 2020 at 9:45 amAhmedDesokiSubscriberDear folksnI'm familiar with FemapNastran. I'm still new user of Ansys.nIf there is a static structural problem. If there are several loads scenarios (say 4) that all affect the same structure, in FemapNastran, I can define these using several (4) load cases. Internally, this reduces to solving a system of linear equations whose righthandside has 4 columns. In this way, if solving one load case lasts 1 hour, solving the 4 load cases usually completes in 1.1 hour. Thus, the solve time is greatly reduced.nI could not find similar feature in Ansys Mechanical UI. Someone told me to use load steps in Ansys Mechanical. I tried this, but I found that solving the 4 load cases lasts 4 times as the time of one step. This is not what I'm looking for.nSo my question is: if I have several different load cases, all affecting the same static structure, and the structure supports do not change for all the load cases, how can I efficientlysolve the problem for all the different load cases? Efficiently means that the total time to solve all the load cases should be comparable to the time to solve a single load case.nThanksn

September 20, 2020 at 3:02 pmpeteroznewmanSubscriberDear Ahmed,nI am familiar with Femap/Nastran and understand your question perfectly. I asked this same questions when I started using ANSYS. A linear model is a requirement to have what you want, which means: only linear materials, small deflections, only linear contact or no contact.nI have a small linear model that runs within the Student License limits, which is < 32,000 nodes. Under Analysis Settings, I set it for 3 load steps. I have a Force on a face and I put 1000 N in X for Step 1, 1000 N in Y for Step 2 and 1000 N in Z for Step 3.nANSYS uses a lot of program controlled logic to decide what to do, so you don't have to. Deciding whether to reuse the factorized stiffness matrix for the next load step is one of those automatic decisions. There is a way to override that automation and force the solver to reuse the factorized stiffness matrix by inserting a Command into the Static Structural branch of the model in Mechanical. If KUSE is set to 1, the program reuses the previous factorized matrix. KUSE,1 forces the factorized matrix to be reformulated at every equilibrium iteration or load step.nI set my Solve Process settings to use only 1 core to force the solution time to be as long as possible. nWith no Command object, the solution time is 13 seconds.nWith Command as KUSE, 1 the solution time is 13 seconds.nWith Command as KUSE,1 the solution time is 21 seconds.nSo you see, you don't have to do anything to get the benefit of reusing the factorized stiffness matrix to compute multiple load case results.nA few years ago, I had a nonlinear model that required a lot of equilibrium iterations in step 1 to pretension some bolts on a flange in nonlinear contact with another part. Step 1 took a few hours to compute. Then I wanted to apply a few different load cases for X, Y and Z. When I put them sequentially, as load steps 2, 3, 4, it took more iterations to finish since the starting point for load step 3 was at the end of load step 2 and the starting point for load step 4 was the end of load step 3. I figured out a way to have each load case start at the end of step 1 and that took fewer iterations. See this discussion. https://forum.ansys.com/discussion/20231/postprocessinginansysmechanicalworkbenchnRegards,nPetern

September 22, 2020 at 8:10 amAhmedDesokiSubscriberDear PeternThank you so much for your help.nAs I said, I tried 4 steps all on the same structure with the same supports, but Ansys didn't choose (KUSE, 1) automatically. In my case, solving 4 load cases lasts 4 times as long as solving one case!!nI tried your suggestion (KUSE, 1). Indeed it reduced the solution time. Please find below some screenshots I think relevant to you.nSo, can you explain why Ansys didn't automatically choose (KUSE, 1)?nIs the warning within the 1st red rectangle a problem?nThanks so much for your kind support.n

Viewing 2 reply threads
 You must be logged in to reply to this topic.
Ansys Innovation Space
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.
Trending discussions
 Saving & sharing of Working project files in .wbpz format
 An Unknown error occurred during solution. Check the Solver Output…..
 Understanding Force Convergence Solution Output
 Solver Pivot Warning in Beam Element Model
 Colors and Mesh Display
 How to calculate the residual stress on a coating by Vickers indentation?
 whether have the difference between using contact and target bodies
 What is the difference between bonded contact region and fixed joint
 The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
 User manual
Top Contributors

2524

2066

1279

1096

459
Top Rated Tags
© 2023 Copyright ANSYS, Inc. All rights reserved.
Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.