I am designing vibration isolators, and I had some rubber compositions mixed and tested. I then used the test data to get an Ogden hyperelastic model for the material.
Before I attempt to design, I decided to replicate the tensile test using NX Nastran.
I set up a simple model, using the average dimensions given for the test specimens on the test report. I defined the Ogden material using MATHE, and I use a 3D mesh of CTETRA8 elements.
I have set up 1000 time steps over which the load of 166N is applied. The load is uniformly applied over the top face, while the bottom face is fixed in translation.
I set up the test using SOL601, since only SOL601 seems to support MATHE and Ogden materials.
But SOL 601 starts, then quits after (maybe) 1 time interval. The f06 file states a Jacobian problem.
" *** WARNING NO. A6 ***
Element distorted, Jacobian DET= -1.835167E-01 GROUP= 3 EL= 79
NUMBER OF ELEMENTS WITH NEGATIVE JACOBIAN DETERMINANT ...= 1
*** ERROR NO. A1101 ***
Mesh too distorted, Jacobian determinant not positive"
I tried to repeat the simulation using standard linear elastic materials (AISI4340 steel), but I still cannot get the simulation to run successfully.
What am I doing wrong?
If you have to simulate tensile test, you have to make sure Poisson effects are re ally small. The correct way to simulate a tensile test is to make the cross-section really small compared to the axial dimension. This will make sure you really simulate tensile tests.
I would recommend you make the cross-section square and small and keep the axial dimension you have.
The .f06 shows the max nodal displacement in the first increment is 1.29E+02. This is probably unintended, unless your block is several meters long
Are you sure the load is defined with a time dependency? If so, take smaller initial time increments or verify that the total magnitude is correct.
The first solution point is 1.0 seconds. Are you expecting that? You say you have it set up for 1000 time steps. Is that 1000 steps of 0.001 for an end time of 1.0 or 1000 steps of 1.0 for and end time of 1000?
You should be running with ATS so that the solver can cut back. You could also try running with TLA so the solver takes care of all the load incrementing, etc.
I have defined the force variation with time as follows:
And I have defined the number of time steps (TSTEP) as follows:
The unloaded length of the test specimen is 25mm, so I may have defined something wrong to stretch to 129mm (±516%) in one step. The intention was to apply the load over a time of 10 seconds.
I have reduced the force to 1N and even 0.1N, but the analysis still doesn't run any differently. I have experimented with available elements as well.
Here is the input file. I see all the parameters that I know to check for, and they seem complete and correct.
I had to change the extension from .dat to .txt to attach it here.
getting the time steps right in a 601,106 is tricky. Once I had defined the steps, but the I didn't "ADD" them to the list below. The way you select the time steps changed in the past with a new version.
You could try the following:
1. Choose a simple material and see if all the boundry conditions, steps and all that are set up correctly.
2. Do not go by force, go by "Enforced Displacements Constraints" , there you can choose a small displacement and if it works, check the reaction forces.
Hope this helps!