Jump to content

Simon Križnik

  • Content Count

  • Joined

  • Last visited

  • Days Won


Everything posted by Simon Križnik

  1. Hi, the error is because the first two X coordinate entries are the same (not ascending). The initial coordinates in the plasticity curve (TYPSTRN=1) should satisfy zero,non-zero requirement (the yield stress can not be zero). So your curve should start with 0,360 instead of 0,0. https://altairuniversity.com/wp-content/uploads/2016/10/1189_MATS1-definition-with-TYPSTRN-in-Optistruct1.pdf tensile_lg_str.fem
  2. I haven't done breakout model optimization yet so take this with a grain of salt: One way coupling is a limitation of breakout modeling: the boundary conditions transferred from the global model may not be valid in a local model, if the local model's stiffness is changed significantly (in a way that alters global behavior). Check how the global response changes at upper when compared to lower bound stiffness (thickness). Afterward, perform optimization with a narrower stiffness range for which boundary conditions are still valid. Also try including a more extended transition region. You may find the following article useful: https://www.digitalengineering247.com/article/global-local-modeling-fea/
  3. While there are forces and moments in the FSI_LOADS load collector, there are also imposed displacements on the model boundary as a result of breakout modeling. Running without any loads results in non-zero displacements. ThickComp.rar
  4. Hi, These counterintuitive results can be explained if the displacements are imposed: the thicker structure is stiffer and develops more stress under the same imposed displacements. For similar reasons when optimizing for stiffness: -imposed loads= minimize compliance -imposed displacements= maximize compliance
  5. Glad to help. Hypermesh is unitless and it is the user's responsibility to follow a consistent set of units. https://www.altairuniversity.com/wp-content/uploads/2012/04/Student_Guide_55-57.pdf Since the material properties are consistent with the tonne, MPA, mm unit system, the model dimensions and loads should follow the same units. So yes, the moment should be Nmm. You are getting a compliance error because of the unrealistically high pressure load of 24000 MPa. Applying only the moment load in the model you shared, the displacement is actually minimal (0.0068 mm). The pressure load should be calculated according to unit system (1 MPa = 1 N/mm2 = 1000000 Pa)
  6. Hi, While nonlinear buckling could be done in Optistruct, it is very is likely the implicit solver will experience convergence difficulties resulting in long run times or even fail due to nonconvergence. Alternatively use Radioss integration to solve your model with the explicit method in Optistruct. 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. Nonlinear buckling analysis is recommended to be performed within Radioss. Post buckling can be solved using nonlinear geometry (Implicit) loadcase. Use any of the Arc-Length methods to solve post-buckling analysis. Buckling.pdf1.46 MB · 130 downloads 2_2_snap_roof___implicit.pdf663.71 kB · 105 downloads 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.pdfUnavailable RD-T_ 3530 Buckling of a Tube Using Half Tube Mesh.pdfUnavailable RD-E_ 0300 S-Beam Crash.pdfUnavailable
  7. Hi, perhaps mesh imprint functionality can be utilized. https://altairuniversity.com/wp-content/uploads/2017/10/Mesh_Imprint.pdf https://connect.altair.com/CP/SA/training/self_paced/aero_v13/PDF/chapter5_demonstration.pdf Mesh Edit Panel.pdf
  8. The most convenient way to get the average size of elements is with TCL: Note: in case mindim specified is smaller than the actual average element size, it will be set as the average size. Yes, setting 0.2 as the upper limit volfrac means 20% volume should be retained. Setting volfrac as 1 is a trivial case wherein all of the available design space is utilized and the optimized configuration is the same as the initial.
  9. The amplitude of vibration is high because there is no damping in the second step. The damping effect is more pronounced at frequencies near the resonance peaks. The worst-case scenario is when the excitation frequency (ramp-up period) is near the resonant frequency and there is no damping. When you are unsure about the damping, perform a sensitivity analysis by varying structural damping in the realistic range and observe how much the responses of interest are affected. The proper amount of damping should also reduce interface force fluctuation. Unfortunately, I do not have the documentation on how the total interface force is calculated, but it is probably the sum of all contact forces. Your explanation is plausible, but it does not account for the period of vibration. p.s. I would appreciate being acknowledged in your thesis. Actually, your challenging queries also sparked my interest in the subject therefore I would like to have a look at your thesis.
  10. Since the AMS run matches other runs without time scaling, the conjugate gradient is below 30 and energy error stays low throughout we can conclude the observed behavior is not an artifact of AMS and the run can be considered verified. Because I haven't researched sloshing I am not able to comment on the validity (matching physical behavior), but I can provide my explanation of the simulation results. There is not a single peak, because the lateral acceleration is ramped up, is held for .8 s then ramped down. The cargo "sticks" to the wall as long as there is lateral loading- instead of bouncing right off. A single peak would be expected if the impulse was a lot shorter (without hold period) or there was an initial velocity imposed on the model. However, I think the acceleration pulse used is consistent with the railcar cornering. The lateral load is ramped up over a period of .3s which excites the bending eigenmode in the sidewall. In the graph below, the X displacement in the region of the highest amplitude of vibration is plotted. The period of vibration of the sidewall coincides with the period of vibration of the contact force; the hypothesis is as the sidewall vibrates against the cargo the contact forces exhibit pulsating forces in phase with sidewall vibration. Therefore the T01 seems consistent with the expected behavior (given the boundary conditions). But I have no idea why T02 does not overlap the T01 trend.
  11. hi 1. mindim is a minimum member size manufacturing constraint. It penalizes the formation of small members and reduces checkerboarding effect. It is recommended that MINDIM be at least 3 times the average element size for all elements referenced by that DSIZE (or all designable elements when defined on DOPTPRM). The average element size for 2D elements is calculated as the average of the square root of the area of the elements, and for 3D elements, as the average of the cubic root of the volume of the elements. 2. Volfrac is a fraction of design space, expressed in the range between 0-1. Volfrac as the optimization constraint with an upper limit as 0.2 means the optimizer will utilize only 20% volume of the design space. 3. Use LOADADD and SPCADD load collectors to combine multiple loads and spc load collectors, respectively then reference them properly in the loadstep. Free-size Optimization Manufacturability.pdf
  12. The animation file is not available for some reason. Can you share it through Google Drive? Compare the interface forces between AMS and CST runs on the same plot. It is strange that T01 and T02 plots not matching in trend nor the magnitude.
  13. Hi, it would be useful to have the animation (my workstation is too weak for this model)- use the HVtrans tool to reduce the file size to upload limits (only stress, contact forces and displacements; reduce frames if necessary). Verify the AMS run against a CST (or without mass scaling) run with a reasonable energy error (ERROR < +2%) and acceptable added mass (MAS.ER < 0.02) along its simulation time.
  14. Hi, This error occurs when a model is under constrained or incorrect material property definition or contact definitions are incorrect or missing. In your case (the units are tonne, MPA, mm) the pressure loading of 24000 MPA is causing excessive deformations. You should review the unit consistency and/or pressure load magnitude.
  15. Following these tutorials, you should be able to resolve this basic issue. Without having access to your model I can only guess.
  16. There are differences in available options as you are using version 13.0 and I'm using version 2019.1- upgrading to a newer version is suggested. I see the split component by body/part option is available at your end, but they are grayed out. This can be expected when importing a part (sldpart file), but not assembly (sldasm file).
  17. Hi, import geometry>solidworks>split components by>part (default is body) Try other formats and/or import options if the issue is not resolved.
  18. Welcome, node-to-node connectivity is preferred (edges panel (F3)>equivalence). Tie or freeze contact can be used to connect nonmatching mesh. Use auto-contact in the tools>contact browser to automatically create contacts. i beam DND_2_edit.hm One element through the thickness is not recommended for bending problems. Remeshing the flanges with many elements through-thickness might lead to bad element quality (aspect ratio) or an excessive number of elements (bad computational efficiency). Given the web and flanges are relatively thin they could be meshed with shell elements instead, which should also enable node-to-node connectivity. https://knowledge.autodesk.com/support/inventor-nastran/troubleshooting/caas/sfdcarticles/sfdcarticles/Thin-parts-can-have-inaccurate-results-when-using-solid-elements.html
  19. There is a tool for material system review: Tools>orientation review>material system Orientation Review - Altair University
  20. Stresses are calculated in the material coordinate system. The material coordinate system may be defined as the basic coordinate system (CORDM=0), a user defined system (CORDM = Integer > 0), or the element coordinate system (CORDM=-1). Edit the PSOLID property and change the CORDM to USER and select the coordinate system which will be the material orientation. Alternatively, material orientation can be assigned to elements directly with analysis>systems>material orientation. In the model you shared the CHEXA elements are oriented with THETA option. The element angle option for Hexa solid (Theta) is very useful if the material system is changing from element to element. Make sure to define only one of these options to avoid confusion. Perform a simple 1 element tensile test to verify material orientation. The like button is a nice way of showing appreciation for the help
  21. Hi, as far as I know, there is no simple way to get the percentage of added mass per each part (part mass output using /TH/PART does not include the mass added, due to mass scaling). Using the animation output option /ANIM/NODA/DMASS or /H3D/NODA/DMASS, the relative mass increase per node can be visualized in a post-processor as a contour plot.
  22. For shell elements, the contact and tie search considers the shell thicknesses. This implies that the defined search distance is expected to be the true distance between the shell surfaces facing each other. For example, in the case of shells without offset, if the geometric distance between the two shell surfaces facing each other is 5.0, and the shell thicknesses are 2.0 each, then the actual distance between the shell surfaces facing each other is 3.0. If the Search distance field is now set to 3.0, then the contact is generated as expected (in this scenario, if SRCHDIS is set lower than 3.0, then there is no contact generated). For more details, please refer to the attached document. To constrain the plate from sliding: -use symmetry (refer to 10.3) -constrain some nodes in the Z DOF Contact.pdf
  23. The initial velocity should be a negative number along the global Z direction. There is a crashbox tutorial in the Radioss ebook, and here are a few videos:
  24. Glad to help. RBE2 transmits the displacements and RBE3 transmits the loads (MPC Forces). Dependent and independent nodes are reversed in RBE2 and RBE3, therefore it is invalid to constrain the RBE3 master node, which is dependant on the deformation of the independent nodes. For more details refer to: http://www.endurasim.com.au/wp-content/uploads/2015/02/EnDuraSim-Rigid-Elements.pdf https://www.predictiveengineering.com/sites/default/files/predictive_engineering_white_paper_on_small_connection_elements-mpc_and_cbush_rev-1.pdf
  • Create New...