Simon Križnik

Content Count
1079 
Joined

Last visited

Days Won
99
Posts posted by Simon Križnik


To select elements within a circle, Shift + Single click and release of the mouse displays the entity selection popup menu:
Inside of circle selects the entities that are inside of a circle window.
In Hyperworks X,
Right Click anywhere in the window:
PrasannaK likes this 
Hi,
simulating maching process can be done in Radioss, but there are some issues:
due to timestep considerations, these simulations are computationally intensive
proper definition of failure (damage)models is essential
There are no milling examples in Radioss yet, but the screwing process is analogus:
https://altairuniversity.com/learninglibrary/radiosssampleofascrewingprocess/
Try to implement this approach in Radioss:

Hi @KBE,
in Radioss user profile rotations can be applied with imposed displacement or velocity boundary condition (XX, YY or ZZ direction of global or local coordinate system skew) with prescribed displacement/rotation versus time curve.
Create rigid bodies on each of the upper and lower tool and apply the boundary conditions only on the master nodes of rigid bodies. Make sure to constrain all unwanted degrees of freedom.

Hi,
First you need to extract the midsurface
Then you can use any of the following option
1)Create Different properties
You can organize the elements of different thickness in different components. then respectively create properties for them with the correct thickness and then assign them.
2)Utility menu>Geometry mesh>midsurface thickness
This option will consider the existing elements for assigning the thickness. Here you are allowed to do the surface editing. But the surface which you are meshing should be extracted mid surface of the required Geometry.
3) Menu>>Assign>>Midmesh Thickness
This is the best option as you can select the elements and apply the thickness.

Hi,
The crushing behavior of the foam cells is represented by a stress plateau with irreversible strains. An elasto plastic behavior is introduced in the deviatoric part of the stress tensor in order to represent this phenomenon.
σ dev plas = A + B (1 + C * γvol) with γvol = (V / V0) − 1
where σ dev plas is the plastic stress applied to the principal stress of the deviatoric tensor, γvol is the volume strain and A, B and C are modeling parameters.
The densification phenomenon is modeled by a pressure term in the spherical stress tensor.
σ spher ij = −P * δij with P = (− P0 * γvol) / (1 + γvol − Φ)
where δij is the Kronecker symbol, Φ is the foam porosity and P0 the initial air pressure.
sebmeca likes this 
Hi,
There has been some changes in the way boundary conditions are applied and organized in Hyperworks X.
The BC manager isn't available; instead BCs are applied under Analyze (on the menu bar).
Also boundary conditions are now organized under load collectors (similar to Optistruct).
I too was not happy at first with the change, but it just takes some time to get used to it.

This material law initially follows the MaxwellKelvinVoight viscoelastic model until it intersects the defined yield curve, which limits the viscoelastic stress in tension and compression.
For more details refer to the attached documentation (from Radioss help):
Viscoelasto Materials for Foams (LAW33).pdf _MAT_LAW33 (FOAM_PLAS).pdf

Hi,
this modelchecker error indicates badly shaped 3D element (meshing issue). The solid is decomposed into subvolumes associated to each integration point. If the element is badly warped, one subvolume could be negative.
Check your element quality.
Tool > check elems > 3D > aspect, jacobian, warpage, tet collapse

Hi,
the issue is because the interface "impacteur vs foam" had dtmin=0.6 If the time step of a slave node in this contact becomes less than dtmin, the slave node is deleted from the contact and a warning message is printed in the output file. This dtmin value takes precedence over any model interface minimum time step entered in /DT/INTER/DEL. Because dtmin is quite high, a lot of nodes are deativated from the interface, therefore penetrating the plate.
The recommended solid property parameters for material law 70:
If there is hourglassing, use Isolid=17, however your model runs fine with the above.
sebmeca likes this 
Hi,
There are initial penetrations; check and resolve using:
in Hypercrash: Quality>Check all Solver Contact Interfaces
in Hypermesh: Tool>penetration checkThe issue is due to the yield stress vs. volumetric strain curve. Because the curve has a negative last slope Radioss extrapolates negative stress, which is not valid (The input stress should be positive for both tension and compression). As a workaround, define an additional curve segment with a zero or positive slope.
Yield stress vs. volumetric strain curve should look like:

Hi,
the minimum timestep warning in the interface is due to the kinematic time step of the interface. It is because the node is penetrating too far into the gap. You can try increasing the Gapmin in your TYPE7 interface which will allow the contact to work sooner and prevent node from penetrating so far. Or you could try making the interface stiffer, Istf=3 which uses the maximum stiffness of the slave and master.
First check for initial penetrations and intersections:
in Hypercrash: Quality>Check all Solver Contact Interfaces
in Hypermesh: Tool>penetration checkCheck the gap that is used for this interface.The value must be physically realistic and based on shell thicknesses in case of contact between shells. In case of constant gap (Igap =0) with no input gap (Gapmin=0), RADIOSS determines a default value for Gapmin and you can check this value in the starter out file. Gapmin=1mm usually works in most simulations.
If some elements fail on the master side or on the slave side of the interface, it is important to set Idel =2 (or Idel =1) for this interface. This will prevent nodes connected to deleted elements whose stresses are released to impact with a possible high velocity.

Hi,
Ishell/Isolid=QEPH/HEPH=24 is not recommended for orthotropic materials because the physical hourglass stabilization forces are computed based on isotropic assumptions.
Instead, use fully integrated elements Isolid=14 or 17.


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,nonzero requirement (the yield stress can not be zero). So your curve should start with 0,360 instead of 0,0. 
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/globallocalmodelingfea/

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 nonzero displacements.
Crashphys likes this 
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 complianceCrashphys likes this 
Glad to help.
Hypermesh is unitless and it is the user's responsibility to follow a consistent set of units.
https://www.altairuniversity.com/wpcontent/uploads/2012/04/Student_Guide_5557.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)
Moawez Zamir Awan likes this 
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 (1e2 to 1e3)3.export the deformed shaped.
4. import the deformed shape into Hypermesh Radioss user profile and set up nonlinear 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 ArcLength methods to solve postbuckling 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:
 RDT: 3030 Buckling of a Tube Using Half Tube Mesh (Hypercrash)
 RDT: 3530 Buckling of a Tube Using Half Tube Mesh (Hypermesh)
 RDE: 0300 SBeam Crash
RDT_ 3030 Buckling of a Tube Using Half Tube Mesh.pdfUnavailable RDT_ 3530 Buckling of a Tube Using Half Tube Mesh.pdfUnavailable RDE_ 0300 SBeam Crash.pdfUnavailable
Brian DO likes this 
Hi,
perhaps mesh imprint functionality can be utilized.
https://altairuniversity.com/wpcontent/uploads/2017/10/Mesh_Imprint.pdf
https://connect.altair.com/CP/SA/training/self_paced/aero_v13/PDF/chapter5_demonstration.pdf
Roshan Shiveshwar likes this 
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.

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 worstcase scenario is when the excitation frequency (rampup 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.
Crashphys likes this 
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.Crashphys likes this 
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 01. 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.
Moawez Zamir Awan likes this
Area and perimetr
in Altair OptiStruct
Posted · Report reply
Hi,
Area is the measurement of the surface of the object (square units)
Perimeter refers to the outline that surrounds a closed shape (linear units).