Jump to content


  • Content Count

  • Joined

  • Last visited

  • Days Won


Everything posted by Hyperman

  1. Hi, non-linear penalty-based contact interfaces require a non-zero initial gap. Type 24 linear contact interface can be used with a zero gap. Type 19 is computationally inefficient and since there is no edge to edge issue in your model a type 7 will be more efficient. A rigid body was put on plates so they will not affect the timestep. The model and boundary conditions are symmetric so a quarter symmetry could be used for efficiency (this will also properly constrain the cylinder in the symmetry planes- currently it is held in place only by friction). plate_cylinder_edit_0000.rad
  2. The model you shared had several issues: no card image and material parameters were assigned to the "rubber" material rigid elements should be placed in a separate component the pressure load collector did not have pressure versus time function referenced (The cause of error id 120) only one linear (first order) tetrahedral element through thickness is not recommended (too stiff in bending). In order to calculate the bending stresses accurately in thin-walled structures, a minimum of 3 solid elements through the thickness should be used. You can take advantage of geometry and boundary condition symmetry by modeling only a quarter of the model. Use Quality> ModelChecker in HyperCrash or Tools>model checker>radiossblock in Hypermesh https://insider.altairhyperworks.com/wp-content/uploads/2017/09/T-T-1248-HyperMesh-Model-Checker.pdf In order to get different buckling modes and Buckling load factor a geometric imperfection should be introduced. Either use a /RANDOM nodal noise or the procedure described in thread:
  3. You need to define simulation controls. Use Tools>engine file assistant to set up the simulation controls. Define animation output frequency ANIM/DT to get the animation output.
  4. Supported Ls-Dyna result types: HyperView LS-DYNA Results Reader.pdf
  5. In the run folder open: 3PBBend.h3d file with Hyperview to review animation output 3PBBendT01 file with Hypergraph to review time history output
  6. Hi, results can be investigated in Hyperview, not in Radioss solver window.
  7. Hi, to asses if the component will break you need to define failure parameters on law 25 or add failure model. The yield stress parameters only relate to the start of plasticity, not rupture. See the attached document and links for more details: Elastic-plastic Orthotropic Composite Shells.pdf https://insider.altairhyperworks.com/accuracy-matters/ https://insider.altairhyperworks.com/composites-rupture/ With Composite stress, you look for stress in each ply (ANIM_SHELL_TENS_RESTYPE). The other stress is homogenized one over the entire laminate (ANIM_ELTYPE_RESTYPE). In composites, it's important to understand stress in each ply. With /ANIM/SHELL/TENS/STRESS/ALL and /ANIM/SHELL/TENS/STRAIN/ALL keywords we can output the stress and strain for all plies in the composite material. In case failure cards for the composite are provided (like /FAIL/LAD_DAMA, which describes the Ladeveze failure model for delamination (interlaminar fracture) you can input /ANIM/SHELL/IPLY/MAXDA, /ANIM/SHELL/IPLY/DAM keywords in the engine file for extracting damage parameters.
  8. Actually, Radioss also supports Yeoh material (law 94). Check the attached tutorial RD-E: 5600 Hyperelastic Material with Curve Input. RD-E_ 5600 Hyperelastic Material with Curve Input.pdf Postbuckling behavior is difficult to converge for implicit solvers like Optistruct. There are two tutorials and one example on NL buckling: RD-T: 3030 Buckling of a Tube Using Half Tube Mesh (Hypercrash) RD-T: 3530 Buckling of a Tube Using Half Tube Mesh (Hypermesh) RD-E: 0300 S-Beam Crash RD-T_ 3030 Buckling of a Tube Using Half Tube Mesh.pdf RD-T_ 3530 Buckling of a Tube Using Half Tube Mesh.pdf RD-E_ 0300 S-Beam Crash.pdf
  9. Hi, check if you can run Transient heat transfer analysis for composites with this model: CARBON LAMINATES- Thermal.hm
  10. Hi, my suggestion is to use Radioss solver due to nonlinear geometry (buckling) and material (hyperelasticity) and possibly contact. Radioss also supports implicit method which can be used for preloading and quasistatic analysis.
  11. Hi, you need to import either the solver deck (*.fem file) or model file (*.hm). Note the former contains only FE entities while the latter also includes geometry with the possible mesh-geometry association.
  12. Hi, buckling instability causes convergence difficulties for implicit methods. Therefore I suggest using Radioss explicit solver instead following this procedure: 1.perform modal analysis in Optistruct 2.in postprocessing create a derived load case>linear superposition>use small scale factor (1e-2 to 1e-3) 3.export the deformed shaped. 4. import the deformed shape into Hypermesh Radioss user profile and set up non-linear buckling analysis. By using the deformed shape obtained from the modal analysis the structure will have geometry imperfection triggering a buckling pattern consistent with modal and linear buckling analysis. Note:1D element idealization will not capture the true buckling behavior of the thin-walled structure. Therefore 2D shell elements should be used instead.
  13. Hi, the mass scaling technique will not reduce the kinetic energy- to the contrary, it will increase by adding mass. The timestep imposed is too high, increasing the mass of the model by 380% (normally only 1-2% mass increase is feasible)- probably the run fails due to this. Check INITIAL ADDED MASS ESTIMATION in the starter out file: at scale factor 0.9 for a 1% increase in mass the imposed timestep should be 1.174E-06 instead of 1E-4. Although I haven't found this in the Radioss manual, it looks like MAT 37 is not supported for mass scaling (mass scaling in your model applies to other components and interfaces). Fluid-Structure Interaction Analysis with Radioss and AcuSolve is possible (check the attached document from Radioss manual). There are initial penetrations in your model and should be cleared before running. Fluid-Structure Interaction Analysis with Radioss and AcuSolve.pdf
  14. Hi, in explicit method the timestep is affected by characteristic element length, stiffness and density. Please go through the timestep chapter in Free eBook: Crash Analysis With RADIOSS – A Study Guide. Also recommended is 2017 Radioss user guide starting from page 30. Timestep_Crash_Analysis_with_RADIOSS.pdf940.97 kB · 13 downloads Review what is causing very low time step in the engine out file: •For an element, check the related material (especially its Young modulus and density in case of an elastic-plastic material; and its viscosity in case of a visco-elastic material). There must not be an error in the units system that this data is given in.  Check the size of the element, since elemental length is proportional to time step. If some elements are distorting badly during simulation it will lead to very low time step and the run will terminate. In this case use small strain formulation (in the property card). •For a node, check the characteristics of connected elements. If the node is on the master side or the slave side of an interface, this interface must be verified. •For an interface, the gap of the interface must be verified if some failure happens on the master or the slave side of the interface. Check the interfaces defined in the model for any penetrations. https://altair-2.wistia.com/medias/osd349gz4k To reduce solving time use mass scaling (DT/NODA) or advanced mass scaling (AMS). Any targeted model for AMS application should run first in /DT/NODA/CST with a reasonable energy error (ERROR < +2%) and acceptable added mass (MAS.ER < 0.02) along its simulation time. A model unable to run with /DT/NODA/CST will not run with AMS either. Output the number of AMS iterations per cycle via /DT/AMS/Iflag - Iflag =2 may help to monitor convergence quality at no extra CPU cost. Maximum allowed iterations before the divergence stops is 1000. 75 to 100 iteration per cycle is a sign of a poor convergence 50 still may provide some speedup 30 iterations or less is considered a good convergence.There should be only a few cycles where INTER is controlling the timestep. Use Multi-Domain Technique if your model has different subdomains characterized by different mesh sizes and consequently very different minimal time step. Additionally, you can use single precision (Radioss panel options: -sp) to speed up computation. Run time remaining can increase during the run even if the timestep does not drop. This happens when available CPU power is used during the run for other tasks (use Windows task manager to check how much CPU is utilized). Negative Energy Error represents energy dissipated from the system and this can be from many sources including plastic deformation and Hourglass energy. If you have included coefficient of friction then the energy error is due to coefficient of friction which is justified. If this amount of energy error is there when no coefficient of friction is defined, then it may be a case of penetration which is problematic. The combined energy error (contact + hourglass) should be less than 15% of the total energy. Energy error.pdf The following contact settings are recommended for type 7: Istf=4 Igap=2 Fscale_Gap=0.8 INACTI=6 Gap_min=1 Fric = 0.1 Iform=2 You can try increasing the Gapmin in your TYPE7 interface which will allow the contact to work sooner and prevent deep penetration. It is also possible to use /DT/INTER/DEL in the engine file to release slave nodes from the interface when time step drops below the value given in this option /DT/INTER/DEL- however, if there are many nodes released during the run the results can be questionable.
  15. Hi, while not exactly foam material calibration, these tutorials might be helpful: HS-1506_ Material Calibration with a Curve Difference Integral.pdf HS-4200_ Material Calibration Using System Identification.pdf Side note: Radioss material law 69 supports Test Data Input to automatically fit hyperelastic coefficients. RD-E_ 5600 Hyperelastic Material with Curve Input.pdf
  16. The files are attached. incremental_output.h3d incremental_output.out incremental_output.pch incremental_output_nl.out incremental_output.fem
  17. As mentioned before, I get the results much lower than required. The probable cause of difference is inappropriate material properties. sonny_25.pch sonny_25.op2 sonny_25.h3d sonny_25.fem sonny_25.out
  18. The shared model works on my end as SPCF and GPFORCE are output at every increment:
  19. Sorry, I overlooked the shared pdf had multiple pages. The signed von mises stress basically displays the tensile (+) and compressive (-) von mises stress. There are two issues: -If I understood the mechanism correctly there should be loads acting on the other end of the pin (as you sketched in the latest post, also see image below). Extract these counterbalancing forces and moments from MBD. -applying loads on the same nodes as constraints is not recommended. In cases like this, inertia relief (Analysis>control cards>PARAM>INREL>-2) should be used to constrain the model. You should not give up so easily- I think you are actually doing great. You can find support on this forum, but you will also have to study on your own. I suggest you go through free Altair e-books, start with Practical Aspects of Finite Element Simulation and for optimization refer to: Practical Aspects of Structural Optimization with Altair OptiStruct You can learn from learning and Certification program. Please follow below link. https://certification.altairuniversity.com/ > (Learn Modeling and Visualisation) Check the following youtube channels: AltairUniversity Altair India Student Contest ELEATION By Apoorv Bapat
  20. You're welcome. Yes, you should fully define the gravity loading. Make sure to select all the nodes in your model (master as well as slave nodes of a rigid body). Here is the procedure:
  21. Glad to help. Looks like the material orientation step is missing in the tutorial. Sharing issues on the forum is a great way to catch problems that could happen even to experienced users. That is why feeback (even if negative) is important.
  22. Hi, You can directly add mass to the rigid body. Select rigid body with Rbody Manager or Card Edit in the graphics area and input added mass in MASS field.
  23. Glad to help. You can show appreciation by liking the content. Yes, the issue is with the G13 , G23 parameters. Are you sure you are not confusing the material property matrix parameters (Gij) with the shear modulus? If material data is specified with the Engineering Constants E1, E2, E3, NU12, NU13, NU23, G12, G23, and G13, then use the MAT9OR data. Analysis>control cards>PARAM>CHECKMAT>NO, but it is possible CHECKMAT is not supported in HM 9.0. It will not solve your problem as mentioned before.
  • Create New...