Hello, This is my first FEA using PrePoMax, so forgive my ignorance in advance. I am trying to run a static simulation on a rubber seal. An analysis is run, but no results are shown. Essentially I am looking for the following:
a. force on the top rim of the part in the radial direction when the displacement of 1mm is applied radially.
b. Force on bottom inner surface that has a displacement of 0.3mm
c. Deformed shape.
I would be grateful if someone could give me guidance on this!
Thanks
I can’t upload the PMX file due to being a new user, so a Google Link is attached.
Unfortunately, I can’t access it (to check, you could try opening the link from incognito mode so that you’re not logged in to Google Drive). Maybe try WeTransfer if it’s too large for the forum.
For such kind of models I would sugest you using hexa elements, and as you want to have a radial loading, you can use only half of the part and apply simmetry. That´s an advantage, as with half part is very easy to get an hexa meshing with Prepomax tools.
This analysis runs (for quite some time), but struggles to converge due to hyperelasticity (you don’t have any other nonlinearities). I would refine the mesh (this is important if you want it to fold in various ways), but what attracts my attention the most is the number of BCs (including prescribed displacements in addition to pressure load) that you have in different locations. Especially the ones on the edges might be problematic. It would be good to reduce the complexity of this model. Maybe try with linear elasticity first. Then, if the results look good, proceed to add more features. Also, try with individual loads at once.
What is the source of your Mooney-Rivlin parameters ?
If you are unsure about your BCs, run a frequency analysis (just add density to the material properties) and check the initial mode shapes. If there are some around 0 Hz, you have rigid body motions. Either way, you will see how your model can deform with the BCs you applied:
Of course, BCs should represent the real-life conditions as closely as possible (you can even use compression-only supports in PrePoMax if needed), but also prevent RBMs in a static analysis.
You could include the rim, modeled in an artifitially increased diameter (enough to unload the rubber lip), and the lower plate also must be modeled 0.3 mm lower. Then in your simulation:
Mesh your part with hexa elements, pay attentio to put about 5-6 elements in the thickness of the rubber part that is being compressed, axial and radial sides. Rim and plate you don´t need much elements.
First step to reduce the diameter of the rim to the finished/real diámeter (radial displacement applied to all the nodes of the rim), with contact with the rubber. You can move also the lower plate to the final position with contact also
Second step with the load, you can apply first the axial load in the rim as a displacement with contacts
Third step with the radial load, again applied in the rim, with contacts
I see that the frequency analysis shows the part rotating around its Z axis. Is this using the constraints that I had? The forces are radial only on the lip, there should be no moment around the Z (local coord.) Should I be constraining the lip from rotating too? Thanks
I think those were your original BCs (even though I played with different combinations too - particularly for the bottom edge). Check the frequency values too - if you have any mode shapes at around 0 Hz, you should indeed adjust the BCs (replace/add some DOFs).
I found the Mooney-Rivlin parameters through this slide show. I cannot find the original table, but I did find some white papers referencing this table using and this source. (see pages 17-20). I’m looking to test 50A and 60A shore diameters.
To preface this, I want to thank you all for your help!
I just wanted to provide an update on this. I tried a different approach in using only a segment of the part to help me refine the mesh as recommended. This allowed a revolved mesh.
I noticed I had set the solver to “pardiso” and I changed that to “default”. I changed the pressure at “1” above to a small displacement (0.2mm) instead. Kept the Mooney-Rivlin material and constrained the segment as shown at “2” and similarly at 90 degrees.
You could also try different meshing algorithms to get more hexes than wedges. The mesh could beore refined too.
Pardiso is actually the fastest and the most reliable solver.
You are showing the total displacement. What’s the magnitude of the tangential displacement there ? Is it significant ? It looks like a slight overconstraint. What type of elements are you using ? It’s quite important if it’s first/second order and full/reduced integration. Especially when using incompressible or nearly incompresible materials and modeling bending.
