Non-Linear Viscoelatic Material in HM - Simulation
Altair EmployeeHello everyone,
i want to simulate a tensile testing with a non linear viscoelastic material (ABS). I have generate some stress-strain charts where i get the material values (E, ...).
So my questions:
- Which solver is for this case the right one? (Optistructe is for linear right? or maybe RADIOSS?)
- How can I define a non linear viscoelastic materialcard in HM? (Does it depends on the solver?)
The material and the geometry are non linear. This must be taken into account.
I am grateful of every answer.
Answers
-
0
-
ok ill check
thanks
0 -
so i checked LAW 33 and LAW 70. i think for my problem LAW 70 is possible. But where can i put the stress strain curve in this materialmodel?
Or do i need just some parameters to define my materialcard?
0 -
Hi Samorit
Check this forum post also. May be this can help you.
https://community.altair.com/community?id=community_question&sys_id=8776083a1b2bd0908017dc61ec4bcb6b0 -
Hi Pranav,
thanks you. It help for understanding however i can not transfer the problem from the post to mine.
My current problem is that i want to create a stress-strain curve in HM. So that the programm get the necessary parameter out of the curve. But it is a non linear viscouselastic material. So how can i connect the Materialcard LAW 70 with the stress strain curve?
Maybe it is simple but it is hard to get there.
(Sorry for bad english )
0 -
Hi,
you can find details about various viscoelastic material models in Radioss help (see files attached).
Tabulated Strain Rate Dependent Law for Viscoelastic Materials (LAW38) could be suitable for your application.
0 -
Hi Ivan,
i checked the RADIOSS Help before but there is no comment that explain how to import a stress-strain curve and how to combine it with the material law.
Now im so far, that i generate a curve with the relevant points. But now i need to connect this curve with my material /component.
Is there any way to do this ?
the curve looks like
real curve:
generated curve:
0 -
Tabulated means function can be referenced to describe material behavior. Material laws 38 and 70 provides this functionality.
About law 38 from Radioss help:
Engineering stress versus engineering strain can be input as functions for different strain rates. The stress and strain is positive in compression and negative in tension. By default (Itota=0), the tension behavior is linear elastic using Young’s modulus, E0. If Itota=1, the engineering stress strain behavior should be input using the functions, fct_IDiL, with the stress strain curve defined both in compression and tension.
So create the engineering stress versus engineering strain function in a tabulated format using XYplots>Curve Editor then reference this curve in the fct_IDiL field of material law and set the Itota=1. In compression, the nominal stress-strain curves for different strain rates are defined by you. Up to 5 curves may be input. The curves represent nominal stresses versus engineering strains.
You can find some examples of law 70 in the following topic:
https://community.altair.com/community?id=community_question&sys_id=5376083a1b2bd0908017dc61ec4bcbcd0 -
Hey,
thank you, ill check.
how can i open .rad ?
0 -
Ok i have combine the Material law with the curve. Thanks.
But after the Simulation it says in HV: 1 Error: Failed to attach results...
I share the model, maybe someone can check this.
0 -
Hi,
if you are new to FEA I recommend you go through the following free ebooks:
https://altairuniversity.com/free-ebooks-2/free-ebook-crash-analysis-with-radioss-a-study-guide/
Refer to the following Youtube channels for practical demonstrations:
Altair University
Altair India Student ContestHere is tensile test tutorial:
Refer to RD-T: 3500 Tensile Test Setup and RD-E: 1100 Tensile Test for Radioss tensile test. OS-E: 0110 Elastic-Plastic Large Displacement Analysis is Optistruct tensile test.
I have made some modifications to your model:
-define runtime, animation and plot output frequency, output requests. All can be created simultaneously in Radioss user profile by utility>engine file assistant
-remesh with hexahedral elements which are more computationally efficient and accurate than tetrahedral mesh
-simplified the model exploiting two plane symmetry in boundary condition, loads and geometry
The model does run, but there is a lot of hourglassing that results in huge energy error. Using fully integrated element formulation or under integrated with physical stabilization (Isolid=14,17,24) results in elements switching to small strain and run failure. Currently, I do not know how to solve this problem.
What unit system is used in this model? My guess is MPa, kg, but I am not sure about time units. The loading stress-strain curve is referencing the same as unloading but should be different due to hysteresis.
0 -
First of all, thank you a lot for your help. Ill check this and write back tomorrow.
My Units are: Kg, mm, MPa
Again, thank you @Ivan
0 -
Thanks for liking my help and subscribing to my content
/emoticons/default_smile.png' srcset='/emoticons/smile@2x.png 2x' title=':)' width='20' />
Success at last, the simulation is perfect in terms of energy (Check the T01 files in HG).
Material law 38 offers more parameters to characterize ABS.
Advanced Mass Scaling is used to speed up computation. For additional speedup when running type:
-nthread (number of cores) -sp (single precision)
Second and tonne units are assumed so interpret accordingly.
0 -
Hey @Ivan
I appreciate the help here in the forum very much. So i have to give something back.
I checked the modell and the most things have i understand. But i have some problems:
First i changed the Modell to fullsize (acutally the idea of symmetrie is nice but in my case i want to do it with the full model)
I have rebuild the model and defined the imp. velocity as follow:
<?xml version="1.0" encoding="UTF-8"?>
After the simulation i just get:
<?xml version="1.0" encoding="UTF-8"?>
Seems wrong to me
I noticed that the time is always 0s in the simulation. (Upper right in the second pictue).
Also you define grnodnode. What are these for? Do i need them or did you used these because of the symmetrie?
Here is the model with the mention changes.
I do not want to take advantage of your helpfulness. if you have the time I am very grateful to you.
[Units: Kg, MPa, sec, mm]
0 -
I need to check if it Is something to with the material curve?
0 -
-solid elements (hexa, penta, tetra, pyramid) do not have rotational DOF (only translational DOF)
-use law 38 which works- I do not know why material law 70 does not
-grnodnode can be used to reference a set of nodes in for example BC, loads, contacts, etc.
-check the unit consistency again- Units: Kg, MPa, sec, mm are not a set of consistent units. You can still use this unit system, but you have to set up analysis>control cards>HeaderCard according to the input and output units required and let the solver convert units appropriately
-you can define output requests to plot force vs. displacement in HG and do model calibration in Hyperstudy
You can give back and show appreciation by hitting the like button on comments you find helpful
0 -
Thank you guys, this is awesome.
After you advice i have checked the units and adapted them to [KG, m, S, N] (SI).
I noticed in the simulation that the component does not break. Then I increased the simulation time but I have no success here.
The Post-Processing looks like:
<?xml version="1.0" encoding="UTF-8"?>
does anyone have an idea?
Also i want to generate a force displacemnt plot. Is there is step by step guide to do that?
Thanks you !
0 -
Thanks for the likes
I am a little disappointed with your learning curve- units system consistency is fundamental and you still have not understood it.
When you adopted the SI system the header card should be revised and the model scaled accordingly.
For the component to break failure model should be defined. ENERGY, TENSSTRAIN and TBUTCHER failure models are compatible with material law 38 (check Failure models in Radioss help for more details). I have defined TENSSTRAIN with low failure strain so break happens during small displacement prescribed.
Force vs displacement plots can be generated by first defining cross-section and node output blocks and then cross-plotting in HG. More details can be found in the following threads:
https://community.altair.com/community?id=community_question&sys_id=cb76083a1b2bd0908017dc61ec4bcb69
https://community.altair.com/community?id=community_question&sys_id=3786007a1b2bd0908017dc61ec4bcb010 -
Hey Ivan,
im sorry for disappointing you. It is right that I still have to learn. Thats why im really grateful to someone like you. You take the time to explain it.
I will deal with the unit system. Like you said, it is very important.
I will do some research and continue my task. I will keep you informed.
Thank you, again!
0 -
Hello everybody,
So for i have updated the model:
- new model with other dimensions was imported
- the units have been adjusted (now: mm, Kg, s also defined in Header_card)
- Clamping lengths have been defined
- force range has been redefined (with grnodes)
- the number of elements has been reduced (because of a too high simulation time)
- the measuring path is 25 mm. At a test speed of 10 mm / min, the simulation time was increased to 150 sec.
So far so good.
When i press Simualte, it comes to following problem:
ERROR ID : 62
** ERROR IN MATERIAL/ELEMENT DEFINITION (LAW)
DESCRIPTION :
-- MATERIAL ID : 3
-- MATERIAL TITLE : ABS ML38
INVALID MATERIAL LAW 38
FOR SHELL3N ELEMENT ID=1
ERROR ID : 62
** ERROR IN MATERIAL/ELEMENT DEFINITION (LAW)
DESCRIPTION :
-- MATERIAL ID : 3
-- MATERIAL TITLE : ABS ML38
INVALID MATERIAL LAW 38
FOR SHELL3N ELEMENT ID=2
ERROR ID : 62
... for every note..It seems that the material is not coupled with the model, however, I can not find the mistake. Do someone have an idea?
Also another question:
From experience, I know that with a simulated time of 150 seconds, the simulation time itself is very high. Is there a methode to reduce it?
Data (Model):
0 -
0
-
thank you for reply. I dont used shell elements. I solved it by remeshing.
After i changed the model size and define the BC's and Material again i get follow Post-processing:
<?xml version="1.0" encoding="UTF-8"?>
i have had this problem before. It seems as if the elements themselves are not connected but that makes no sense. I'm surprised how hard it is to depict a non linear viscouselatic material in a tensile test.
Maybe someone have an idea?
0 -
like @Prakash Pagadala pointed out, law 38 is not compatible with 2D elements (check compatibility chart in Radioss help). Law 69 can be used with 2D elements and allows engineering stress-strain input to automatically calculate Ogden or Mooney-Rivlin coefficients. However, this curve input has to be modified since this law accepts only monotonically rising stress values.
The 2D meshing should be done on mid-surface, which is extracted from solid by geom>midsurface.
You can simulate a static loading more computationally efficient by time scaling, which means applying the load more quickly than in the quasi-static experiment in order to reduce the simulation time. However, the kinetic energy should be low (5-10%) compared to the internal energy for most of the simulation, to minimize the inertial effects. You can check the energy fraction in Hypergraph by plotting both energies and using Vehicle safety tools (File-Load-Preference File) to divide curves (Math-Two Curves-Divide w/Zero). Plot kinetic, internal, contact, hourglass and total energy in Hypergraph. Those variables are output by default and can be loaded in HG (file: runname_T01)>Global Variables>Y requests>MAG to plot.
0 -
I dont have MLAW69 as an option.
Do i have to activate a spezial option or maybe i have a older version of Hyperworks?
0 -
Looks like you have an older version that does not yet support law69.
You can use law 36, which is compatible with 2D elements and allows stress-strain input. Note that the work-hardening portion of the stress-strain curve is used (for example, plastic strain vs. stress). Given that your material stress-strain curve does not exactly have a linear slope you can try this workaround:
-approximate the stress-strain as linear until yield strain with elastic modulus and prescribe plastic stress-strain with a modified curve. See attached example where yield stress was defined @ 0.002.
You can also use the MATS1 and TABLED1 combination and run a non-linear analysis in OptiStruct (refer to OS-E: 0110 Elastic-Plastic Large Displacement Analysis).
0 -
Altair Forum User said:
Hi Ivan,
i checked the RADIOSS Help before but there is no comment that explain how to import a stress-strain curve and how to combine it with the material law.
Now im so far, that i generate a curve with the relevant points. But now i need to connect this curve with my material /component.
Is there any way to do this ?
the curve looks like
real curve:
<?xml version="1.0" encoding="UTF-8"?>
generated curve:
<?xml version="1.0" encoding="UTF-8"?>
0 -
OptiStruct 2019.1 supports viscoelastic material.
Viscoelastic material
Viscoelastic material through the MATVE Bulk Data Entry is supported for Small Displacement Nonlinear Analysis. Currently, CHEXA, CTETRA, CPENTA, and CPYRA elements are supported. Viscoelastic material can be activated by using the VISCO Subcase and Bulk Entries.
0
