The rubber has hardness of 45 A shore. It gets heavily deformed.
I have used the following mooney-rivlin constants. I will attach the research paper from where I got this, as data is old one I have to look in to my collection of literature review
Did you calculate them yourself (if yes then in what way ?) or took them from literature ?
if I calculate it myself then the coefficients are 0.2426, 0.0612 and 0.1635. but I am not sure about the correctness that is why I stick with the research paper data
I have used the curve fitting tool that calculates mooney rivlin co-efficients from stress strain curves
Different values could help. I guess you canāt share the stress-strain curves (I could calibrate several different hyperelasticity models based on them and see which model has the best fit in this case).
Do you have some photos of the real-life deformation to compare with simulations ?
Here is the data sheet of this component
I have the component but unfortunately it is in undeformed shape. The main problem is there is no way to separate the rubber material from this assembly except cutting it in half.
I have very limited data and what i am 100 % sure is only that it is natural rubber with hardness 45 shore. The rest of data I gathered from research papers.
The real life deformations show that the rubber is around 4.5 mm pressed but I canāt see what it looks life from the inside. I wish to perform further fatigue analysis and for that I wish to obtain the deformed shape of my rubber after loading.
Mechanical properties of rubber may vary a lot depending on the supplier even for the same kind of rubber. If you donāt have reliable test data then it might be worth playing with different constants of the Mooney-Rivlin model you are using now and maybe even with different hyperelastic models (but the rule is that one should use the simplest models when thereās no sufficient data available). On the other hand, the Mooney-Rivlin model should be used for moderate strains (not significantly larger than 100%).
1 Like
I agree. Do you have any dummy data to start with ?
Can you check if upper/lower metal are bonded? Maybe you can scratch with a pencil or stick from bellow for checking the upper metal. If that the case, the void in the upper side could not be realistic due to mold undercut.
In the table there is a max load of 1275 N for a max displacement of 4.5mm, and the rubber hardness shore A 45 , so if we asume that this is for vertical loading, you can use your one element thickness model (similar to an axissimetric) to create a load/deflection curve and see if the geometry is accurate.
Also exist the possibility that the part is preloaded during the assembly (riveting), this could modify your stress state for durability predictions.
Only from research papers like you. For example, I got those constants derived from some article:
C_10=0.137880667, C_01=0.216797082, D_1=0. But I would suggest changing the values a bit in different ways and checking if thereās any visible effect on the results.
This is what I doubt. At the time of assembly the riveting happens. I also calculated that because of the tilt and unsymmetric assembly one of the damper is going to be loaded at 1900 N (far above the maximum limit) because of the load the rubber will be compressed initially (this is what I simulate currently). After this the vibrations will be induced on deformed geomtery (the fatigue case)
Thank you I will try them
Just as a quik reference.
Unless my mesh has scaled incorrectly your model dimensions do not fit the catalogue.
Where does your mount end up.?
Remove contacts and apply the 4.5mm BC to see where it end up.
Maximum run of 4.5mm is most probably vertical displacement.
Take a look at TRELLEBORG NovibraĀ® type RAEM as example.
Complete catalog is full of data.
Just by how the Rubber is shaped and fits at final position I would say your device was mostly intended to work under vertical load.
Iām using (ccx) , your same material parameters , full C3D8R and 4mm vertical run.
Low tangential stifness and 0.1 friction coeficient in the contact.
Just one master and one slave.
When solving the extruded problem itās better to provide a wider master surface to assure the rubber doesnāt loose contact when expanding. Use rigid body on the mount until you find suitable contact parameters. If you manage to compute the Jacobian (@Matej _Could be a nice improvement) you will be able to anticipate where the mesh will most probably will fail first.
I will try to move the analisys to Prepomax.
By the way this is not the solution of the problem. As Sergio said you need to revolute the problem not extrud it. Now itās missing all the hoop stresses.
Whitout that gap ā¦troubles.
Is your model related with this other question/user.? If thatās the case it would be better to include the mount as you are doing to apply the Moment properly.
This is how it looks like without contact. The deformation of rubber will be drastic
You are right, the dampers should be used only in vertical direction and they are only designed for it. But in my case they are assembled at an angle, this is risky and I doubt that the dampers will not survive this unsymmetric loading.
Unfortunately the transfer link has expired and I can not access the files. The photo you have attached is from different damper model. There are 100s of different models with varying load carrying capacity.
In my model there is no gap as you can see from the data sheet
This seems a nice idea
why do you use 0.1 friction coefficient, I read that sometimes the friction coefficient between metal and rubber can go high up to 0.9
To increase the problem complexity slowly until some parameters are adjusted.
Because that critical area is confined, there is no possible load redistribution. You could perform a simplified compression test with that thickness and run to see if itās worth to keep going with the full model. If the rubber exceeds allowable stresses, there is no reason to continue and maybe report the client to replace with some other device.
Large friction can cause convergence issues. Abaqus activates unsymmetric solver from 0.2 but it should be used also for lower friction coefficients. Itās even better to avoid modeling friction at all when not necessary (itās really nasty for convergence) but sometimes thereās no choice and reducing it initially may help before proceeding to the actual values.
1 Like