Help Isotonic Test
Altair EmployeeHi,
I need to implement non-linear analysis of a McKibben muscle. The tube is an hyperelastic rubber, that i have modelling as MATX42 and use an NLGEOM analysis.
In my model, I need to apply an initial force of 5N and after a time dt also apply an internal pressure. How do I define these two time intervals?
This is the condintion of my ISOTONIC TEST:
- FORCE F=5N applied from the time T=0 to T=2
- PRESSURE P=0.25Mpa applied from the time T=1 to T=2
Final objective is to obtain a graph that relates the pressure with the stretch of the tube. Thanks
Answers
-
Hi @jugerman
Is the intial load or force is a Preload on the muscle model?
You can define two curves one starting from T=0 to 2 and the other from 1 to 2.
0 -
The force is applied to the beginning when the internal pressure is zero and it is constant (F = 5N) while the pressure increases to the maximum value.
How i can define these curves?
Thanks for the answer.0 -
Hi Jugerman,
Provide two curves with loading as required. You can load the force from zero and load the pressure from one in the curve.
For your reference please refer tutorial OS-1360 in the Help Menu. Four curves are created in that model (loading and unloading curves) based on the required time of the user.
This will provide you a fair idea on creating the curves.
0 -
OK. I have 2 problems:
1) i have create 2 load collector, one for FORCE and one for the PRESSURES that are applicate on all faces of the 3D elements of internal tube. So how i can define the curve for my loads.2) when i create the LOADSTEPS, i can not select more than one item under the box LOAD, so how can define the parameter of my analysis?
Is possible that my mode is not correct.
Thanks you so much for the support, wanna resolve all problem if is possible.
0 -
I tried this way:
- created 2 collector without card image that include the FORCE and the PRESSURES (PLOAD4)
- than i created two curves using TABLED1 [xaxis/yaxis -> linear] with 3 point:
for the FORCE [(0,0) (1,5) (2,5)]
for the PRESSURE [(0,0) (1,0) (2,0.25)]
- than i used NLOAD1 to define the loads, in which i put as EXCITEID the first collectors without card image, as TYPE -> LOAD and as TID -> TABLED1
- at the end i created a collector with NLOAD in with include the two NLOAD1 [S1=1,L1=NLOAD1]
After that i created the load step:
ANALYSIS -> NLGEOMNLOAD -> the last collector
NLPARM
I hope I have shown as well have defined my load.
The analysis work, but the model have only a stretching. Why? Where i wrong? Thanks!0 -
0
-
0
-
Hi,
Somewhere the analysis is reset to static and I think this what causing the problem. Is it possible to share the model?
0 -
0
-
Hi @Prakash Pagadala ,
you need other information to help me?
I must resolve this problem. Thanks for all!
0 -
Hi @jugerman
So I modified the deck but I got same result and few errors.
Later when I was looking at the load and pressure magnitude, I increased the pressure magnitude by 10 times and the results are meaningful.
But I dont know why the action satrts from 1 and not from zero. this is what I am investigating now. Will update to you soon.
0 -
Hi,
So In NLPARMX you have given animation write time as 1. This will write the animation file starting at 1.
I will share the animation file with you. Please check the results and let me know.
0 -
Hi,
with the pressure of 0.25Mpa the muscle (by exsperimental test) should stretch of 38mm, in the simulation the max is only 7mm, this is not correct.
Curves have been well defined? The loads are fair? I do not know if there I made mistakes. Thanks @Prakash Pagadala0 -
Hi,
Can you check the units, material etc..?
If everything is fine then there should be some problem with modelling?
0 -
If i try a simple analys with this load step:
- same analysis: Geom non-linear (impl. static)
- same SPC- LOAD: only loadcollector with the pressures without curves
- same NLPARM
the model have a 'correct' deformation (-39mm) , obviously without considering the force of 5N , that i dont know how introduce in this type of analysis (this is my principal problem!).
So this analysis show that the model (component, property, material) is correct (i think), but the way in which the LOAD (Pressure + Force) are generated or combinated is not correct.
PS: by default, the pressure is expressed in Mpa when i use TABLED1?0 -
now the model work! The problem was in the parameters to be introduced in the table of TABLED1:
i change the parameters of Y, that i had set with the modulus of the force (5) and the pressure (0.25), but so i increase/decrease tha two LOADS (is correct my analysis?), while now i set up with the unit, and the model have the right stretch.
Now i have only a question: is possible create a plot with the PRESSURE on the X-axis and the DISPLACEMENT of a node on the Y-axis?
Thanks0 -
Hi,
Thank you for the update, Glad it is working now as you expected.
Yes, you can plot Pressure Vs displacement using Cross plots. Please refer to the below forum post:
Before that you need to output pressure and dispalcement or you can use create curve option in HyperView to plot curves.
0 -
I have just a problem: the pressure that i have as result of analysis is the pressure of singular element (Pressure 2D, 3D).
What is the output request to have the total pressure that deformed my muscolar model? Is possible?
I wanna plot Pressure vs Time, not the pressure of singular element, but the Pressure into total tube (the pressure of compressed air that enter into the tube model)Regards
0 -
Hi,
I dont see a way to output total pressure (as you said inlet and outlet) to h3d file.
Maybe you can calculate using result Math module in HyperView and plot the graph.
0