March 16, 2021 at 12:24 pmWasifSubscriber
I am doing a three point bending test. In the results below, you will see that when I use mid-plane surface in the shell, the contact stiffness is lower. However, when I use NLOC, the stiffness is higher but there seem to vibrations in results. I tried to set VDC to 100% percent but the vibrations still exist. Is there a workaround to this problem where we can increase the stiffness without going to material properties?
PS. I tried changing penalty factors in the contact but that does not work.March 21, 2021 at 7:50 pmAndreas KoutrasAnsys EmployeeHello Wasif,nYou may tune the contact penalty stiffness through the parameters SLSFAC (in CONTROL_CONTACT), SFS and SFM (in *CONTACT), SOFSCL (in *CONTACT optional card A) depending on what contact you are using. See Sections 29.7.1, 29.7.2, and 29.7.3 of the Theory Manual for how the penalty stiffness is determined in SOFT=0, SOFT=1, and SOFT=2 contacts. For a general purpose contact in explicit analysis we recommend *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE with SOFT=1. The penalty contact stiffness of SOFT=1 is determined from:nk = max(SLSFAC*SFi*k0, SOFSCL*k1)nwheren k is the penalty stiffnessn SLSFAC is user input in *CONTROL_CONTACTn SFi is either SFS or SFM in *CONTACT card 3n SOFSCL is user input in *CONTACT optional card An k0 is the stiffness calculated from the bulk modulus of the material and the element dimensions, as described in Section 29.7.1.n k1 is the stiffness calculated from nodal masses and the solution time step, as described in Section 29.7.2.nIf you increase the contact penalty stiffness to a value higher than the default one, you may need to specify a lower time step through TSSFAC in *CONTROL_TIMESTEP to ensure stability of the explicit analysis. nFor implicit analysis, the recommended contact is *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_MORTAR. The contact pressure -versus- penetration constitutive relation can be tuned through the parameters SLSFAC, SFS, IGAP, and PENMAX as described in Section 29.21.2 of the Theory Manual.nIf you want to tie the shells to the solids, you will need to look at the CONTACT_..._TIED and CONTACT_..._TIEBREAK options.nI hope this helps.nRegards,nAKViewing 1 reply thread
Ansys Innovation Space
- You must be logged in to reply to this topic.
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.
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
- explicit dynamics
- Explicit dynamics ERRORS
- turning simulation
- getting zero maximum and minimum stress value in explicit analysis
- How do get Full values instead of just minimum and maximum ?
- How to figure out impact force in Explicit Dynamic Analysis
- Monte Carlo Simulation
- Running an explicit dynamics simulation on a composite plate
- Which analysis to use for dynamic and quasi-static compression of auxetic structures?
- Euler Domain Restricting Simulation
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.