John: I highly suspect that the finite element formulations (of the type used in this specific software) are not quite appropriate to model some nonlinearities very well - I've come to the conclusing using this software with plasticity modeling (i.e., a near 'flowing' material). I don't believe it's the software developers at fault here - just the appropriate math used in the finite elements. The elements get too stretched or compressed and they tend to 'lock' or not provide realistic results, or the program 'exits' (i.e., crashes). I know there is other software called: Adina and MARC and Abaqus that have element formulations specifically designed to handle these types of nonlinearities.
To suggest a solution other than that, this type question should go to the developers - the software should handle it: it should only be a matter of twiddling the knobs on their math models, which I'm not good at.
I hope that helps (a little). I'm trying to prevent you from going down a rabbit hole (which I've done many times with this software).
Anthony -- Thanks very much for the caution. I had heard that some (older?) FEM software did not handle elestomers well. An interesting article I found seemed to be saying that it was Poisson's ratio very close to 1/2 that caused the problems. (I don't know how to add an attachment to a post here, but the difficult-to-find article that I'm thinking of is "Springy Finite Elements Model Elastomers" by Robert H. Finney, in MACHINE DESIGN, May 22,1986, pp.87-92.) It's not that the media are "nonlinear" -- they don't have to be -- they just flow elastically, as you say, rather than compressing in bulk because the bulk modulus is very large compared to the others.
Just a couple more follow-ups if I may:
1) In your experimentation, have you tried deliberately lowering Poisson's ratio, say to 0.49 or even 0.45? This would have relatively little effect on the relationship between Young's and shear moduli, just make the bulk modulus smaller, and it might still give reasonably realistic results for "shape factors" that aren't too extreme.
2) Where do you find these "knobs on their math models" in the settings menus? I'd be happier going after the developers if I had a better idea what I'm talking about.
3) Do you (or does anybody else in this forum) know anything about how SolidWorks handles the input material properties? (See the P.S. on the end of my OP.)
Thanks again! -- John Willett
Hi John: Yes, you found the element 'locking' phenomenon. I have tried some models in SW tutorials and training manuals where they recommend to set the Poisson's ratio to 0.49 or even 0.4999, but never 0.5. The models worked (i.e., solved), but I do not know if the answers matched any test data. Anyway, I have seen code in ANSYS that handles the large deformation issue- as you say the material does not have to be nonlinear. It's the model that needs to allow the extreme stretch, compression, bending, etc., of the elements. The ANSYS code handles that by stopping the solver when the elements get "too deformed"; saving the data to that point, then re-meshing the model with nicely-shaped elements; then continue from there with the loading until the elements get too deformed again, at which point it will stop again, remesh, and so-on. I believe you need some deep pockets to buy that functionality - it is an option purchase similar to the vehicle proximity alert monitors on the side mirrors of some new automobiles.
1) I have tried deliberately lowering Poisson's ratio and it appears to give reasonable results that (as you mention) may not be too different from results at 0.4999. However, I have not assessed accuracy.
2) knobs are in the "Properties" panel of the nonlinear study. There are stepping options, time increment options, and geometric nonlinearity math model options. Then, there is a button at the bottom labeled "Advanced Options". Click that, and there's a set of more knobs to twiddle, including the nonlinear control agorithm selection, step/tolerance options, singularity handling, and so-on. You can greatly affect your analysis outcome (and whether or not it will finish) with these knobs.
3) I was told by technical support that (for the linear-elastic, isotropic material model), if you do not put in a shear modulus, the software will calculate one based on the Poisson's ratio. Likewise if you do not put Poisson's ratio, it will calculate one if you have a shear modulus. If you do not put in one or the other, it will stop and say so.
I hope that helps!
Anthony -- I've read a bit now about nonlinear FEM, but I'm still puzzled by why it is needed in my problem. I'm looking at very small strains in these rubber bushings where the material should remain in the linear range and all the linear stress-strain relations should be valid. Linear analysis, as in SolidWorks, really ought to be applicable...
I should probably clarify that I'm working with SolidWorks Premium (which has linear static simulation capabilities), not SolidWorks Simulation with its broader capabilities.
Based on what you have said, I think it makes sense to do some test runs with my bushing and Poisson's ratio artificially lowered (that is, specify Young's modulus and an altered Poisson's ratio and let SolidWorks come up with its own shear modulus, which I can also calculate for myself). I can then compare the results with my semi-empirical formulae for the same bushing (which assume perfect incompressibility but still linear behavior) and see if they become more reasonable. If so, I can just "tweak" the rubber properties in my model to a point where SolidWorks can swallow them. Sound reasonable?
I will also try contacting the SolidWorks developers through my re-seller and see what they can tell me. Thanks again! -- John Willett
what kind of strains are we talking here? would you consider the deformed shape to have small displacements relative to the size/shape or will they be very visible in the model?
to note, all the controls that tony has talked about are only in simulation premium. at the linear static stress level, you don't have any controls other than playing with the material properties. you can enable large displacement mode but that is a subset of what can be done in simulation premium's nonlinear analysis capabilities.
Jared -- Thanks again for the useful input.
>>what kind of strains are we talking here?<<
My bushing is 3/4" diameter and 0.136" thick (material properties stated in my OP) and is bonded on both faces to relatively very rigid plane surfaces. The displacements that I calculate from my semi-empirical formulae are 0.0044" in pure shear or 0.00035" in compression with 1 lb force (a typical load in the application) applied in each case. So the displacements seem very small in comparison to the bushing dimensions.
The oddest result, from my point of view, is that SolidWorks Premium matches these displacements fairly well with very low resolution, also as described in the OP, but its solution gets much worse at reasonable resolution. (I still haven't tried tweeking Poisson's ratio...) Was Anthony trying to tell me that the "locking" phenomenon occurs when the local strains get too large within individual elements or as Poisson's ratio approaches 1/2?
>>...all the controls that tony has talked about are only in simulation premium. at the linear static stress level, you don't have any controls other than playing with the material properties. you can enable large displacement mode...<<
What does the "large displacement mode" do, and might that help in my application? -- John Willett
John, if you want to really dig into the software, go into the solidworks KB and search for geostar. It has all the equations, element formulations..etc that are used on the background. Much of it is not exposed in the software other than what anthony has described. Here at Hawk Ridge, we carry both SolidWorks Simulation and ABAQUS because we know there are classifications of problems that can't be solved in SolidWorks Simulation in the nonlinear realm. Yours may be one of those but before you start looking for another tool, I would definitely double check with your reseller who can confirm things with SolidWorks. Without going over your problem I can't say for certain, but it sounds like you're either at or nearing some of those limits as Tony has described.
You may want to post a sample up here for others to try out and check setup..etc to get a few more opinions.
Unless you are doing a really simple sort of analysis, you really should be using a hyper-elastic material model for the particular Silicone or Silicones that you are using. You need to spend something like $1K to get a material lab to establish the material properties. We have used Axel < http://axelproducts.com/ > and been happy with the results.
>>Unless you are doing a really simple sort of analysis, you really should be using a hyper-elastic material model...<<
Thanks for the useful reference. At this point I think I'm still at the "really simple" level, since I'm using these bushings at very small strains where they should exhibit linear elastic behavior. -- John Willett
Yes, I see from the numbers in your second reply to Jared that you can probably get away with linera analysis. One reason I can think of for your results is that the rubber is actually much stiffer at the very small deflections than you are expecting. Rubbers often have an S shaped stress-strain curve, where they start out stiff, soften up through the middle, and then stiffen up again at high strains. Since the published values for Young's modulus are usually given at fairly substantial strains, the stiffness at very small strains is probably going to be much higher.
>>One reason I can think of for your results is that the rubber is actually much stiffer at the very small deflections than you are expecting. Rubbers often have an S shaped stress-strain curve, where they start out stiff, soften up through the middle, and then stiffen up again at high strains.<<
Jerry -- Thanks for calling attention to this nonlinear behavior. Actually I don't expect my material properties to be very accurate in any case since I derived them (through the use of some tables I found in a rubber-design book) from the manufacturer's published value of Shore A hardness = 35. (Direct measurements of the shear and compression behavior of my bushing at the expected loads are in the plans.) From what you say, I'm guessing that the quoted hardness spec. would apply to intermediate strains and might therefore give lower stiffness values than I will experience at the near-infinitessimal strains in my application. Is that a correct interpretation?
But I don't understand the first part of your quoted comment. Since I have yet to measure any real parts, SolidWorks Premium should be giving me results for the linear material properties that I plug into it (as in the OP). It can't know the actual dependence of stiffness on strain level for the real material. What am I missing here? -- John Willett
i think we're at a point where posting an example would be good
>>i think we're at a point where posting an example would be good<<
Jared -- Can somebody please explain how to attach files to a post? I have a .ZIP file containing the part and assembly information for these studies (the relevant .SLDASM and .SLDPRT files), but I can't immediately see a way to post it..
I do see an "insert image" button and have used it to attach images here of the two study results -- pure compression:
and pure shear (with the aid of some constraints to prevent the forced plate from tilting):
Here also is the material-property screen for the bushing:
I apologize that this may get a bit involved: I'm not the SolidWorks licensee in this case; I'm evaluating the software for a potential purchase. The runs I'm describing are being done for me by a friend who already has a license and subscription for SolidWorks Premium. I specify the bushing dimensions, material properties, and desired tests; he sends me the resulting images and files -- in particular the node location and displacment listings for the face(s) of interest. I then analyze the displacements (in this case just averaging displacements across a face) and compare them with the predictions of my semi-empirical formulae for the same material properties.
For these tests, 1 lb force was applied either to the compression block or the shear plate, and the corresponding displacments were computed. The bushing was a right-circular cylender 3/4" diameter and 0.136" thick, with the two faces bonded to rigid blocks or plates. I believe that SolidWorks was allowed to choose its own node densities in the parts. In any case there was plenty of resolution to model the bushing displacements. The comparison results are as follows:
Displacements for 1 lb Total Force Compression Shear Compression/Shear Ratio
----------------------------------- -------------- ------------- ----------
SolidWorks Displacement (mm) -3.2762E-05 -1.5510E-04 0.21123
Semi-Empirical Displacement (mm) -8.7997E-03 -1.1154E-01 0.078891
SolidWorks/Semi-Empirical Ratio 0.0037231 0.0013905 2.6775
As you can see, the disagreement is dramatic. (As mentioned in my OP, however, there reasonable agreement in a much more complicated study that had a much lower density of nodes in the bushing.) My friend tells me that the "study" files are way to large to send by e-mail. Please let us know what else you need in order to duplicate our results. Thanks! -- John Willett
hit reply to start a new post in the thread
at the top right click "use advanced editor" and then you can attach the files
i'm still soaking things in but why did you include those 2 components for compressing the bushing?
what is the long term application for software with respect to the bushing?
Can you elaborate on what you mean by semi-empirical?
>>hit reply to start a new post in the thread
at the top right click "use advanced editor" and then you can attach the files<<
>>i'm still soaking things in but why did you include those 2 components for compressing the bushing?<<
If you mean why the metal/rubber/metal sandwich, I guess that's just the first way my friend thought of applying forces to a bonded bushing.
>>what is the long term application for software with respect to the bushing?<<
Bit of a long story. I'm designing a mirror cell for an astronomical telescope. The surface of such a mirror must be accurate to within a few tens of nanometers. My novel approach to "floating" the mirror without the suspension system's either (1) directly distorting its surface or (2) passing along significant distortions from the metal cell (which must be suspended by three points for collimation and will consequently flex) is to cement the mirror into a ring-shaped cell with nine silicone-rubber "bushings." These bushings will be made by supporting the mirror inside the ring, injecting RTV paste through holes in the metal ring, and then allowing them to cure before removing the supports. The three requirements for success with this design are (1) that there be enough support points (bushings) around the mirror's edge to support it sufficiently uniformly, (2) that the bushings be very soft (relative to both the glass and the metal) so that distortions in the metal ring are "buffered" and not fully transferred to the mirror, and (3) that the metal ring itself be sufficiently stiff not to flex too much.
As you can see, this design requires all three elements (mirror, bushings, and ring) be modeled together to make sure they will actually work as planned. We started modeling the entire assembly with SolidWorks, allowing it to chose the node positions in each part. We found anomalies apparently due to the fact that there weren't enough nodes in the bushings, so we increased their resolution. This step turned out to make the bushings a couple of orders of magnitude stiffer, passing too much of the cell distortion to the mirror. Now we're trying to figure out what's wrong with the model bushings by examining them separately.
>>Can you elaborate on what you mean by semi-empirical?<<
The easiest way for me to do that is to send you far more informaiton than you want, although you might find it interesting. Attached is an MS-Word file that summarizes, starting on p.3, the shear, compression, and thermal behavior of doubly bonded, cylindrical rubber bushings and gives the formulae that I use with references to my original sources. I believe these formulae to be pretty good (although we are obviously having trouble getting agreement with SolidWorks), but they clearly aren't enough on their own to design the cell because they don't give a mechanism of integrating the flex of the mirror and of the metal cell as a system.
I hope I've answered your questions. -- John Willett
still haven't looked at things in depth but i just wanted to go back to the original problem definition
1. compression is completely off vs expected
2. shear is good until the mesh is improved
expectation is based on the provided equations that are specific to this type of material and application and no physical tests are available.
do we have any "known good" results, experimental + calcs + fea ideally.
have you checked standard equations for compression of a part and/or shear of a part based on linear static assumptions?
>>1. compression is completely off vs expected
2. shear is good until the mesh is improved<<
BOTH compression AND pure shear behave essentially the same vs. resolution. Both agree reasonalby well (shear is near perfect, as might be expected since there is little or no "flow" of the elastomer) at low resolution (in a much more complicated assembly). Both are terrible at SolidWorks's default resolution in the simple assembly posted.
>>expectation is based on the provided equations that are specific to this type of material and application and no physical tests are available.<<
Correct. The equations are specifically developed for rubber (assuming Poisson's ratio = 1/2). I presume that the authors of the source book have tested them against real materials, but I have not.
>>do we have any "known good" results, experimental + calcs + fea ideally.<<
>>have you checked standard equations for compression of a part and/or shear of a part based on linear static assumptions?<<
I'm not sure what you mean here. I have not searched for equations for any particular shape made of, say, steel, nor have tried to validate SolidWorks output for such a material. (We did verify that cubes of both "glass" -- Poisson's ratio = 0.24 -- and "rubber" -- Poisson's ratio = 0.40 -- exhibit volumetric compression when exposed to gravity with the bottom face rigidly bonded. That is, subtracting the subsidence of the top face from the bulging of the four sides gives a negative volume change that is larger for the glass than for the rubber, as one would expect from the differing Poisson's ratios. We have not tried this for the silicone rubber specified in this thread. I hope this may anwer your question.) -- John Willett
so a couple of things
first i pulled down your model and the materials don't match what you posted and the shear modulus wasn't included in the material definition. there are some assumptions that are made when they aren't entered.
i didn't spend a tonne of time looking through your document but what i was looking for is where your values for displacement came from. what was the force input what were the material properties used..etc. the reason is that i wanted to setup your problem in reverse (input the displacement and output the force necessary) to see what happens but stopped when i noticed that the setup didn't match what you had described so before going too much further i wanted to make sure the setups are equivalent. if we don't know that we're comparing apples to apples and that the assumptions are the same, its going to be difficult to get the same numbers. not knowing whether the method has been validated physically is also an issue but until we have exhausted everything, we shouldn't go down that path.
regarding assumptions, in my setup i took the 2 plates out of the equation. they are there but the boundary conditions are applied to their inside faces. in the compression example the top plate was bending around the bushing more than it was actually compressing the bushing. does this match the case for the equations you're using to get an estimate of what the reactions should be? ie in the shear case for example that there is no play in the Y direction or the X direction and that the bushing is in pure shear?
>>first i pulled down your model and the materials don't match what you posted and the shear modulus wasn't included in the material definition.<<
I can't answer the questions about the input files -- have to wait for my friend who did the runs to respond.
>>i didn't spend a tonne of time looking through your document but what i was looking for is where your values for displacement came from. what was the force input what were the material properties used..etc.<<
About the semi-empirical model, the equations are stated for force as a function of displacment, whereas I put in a 1 lb force and solved them for displacement. As written:
For shear force use Equation 1. For displacement = 0.00439" (0.112 mm), shear modulus = 70.1 psi (the value in the document is an older estimate), r = 0.375", and t = 0.136" I get F = 1.00 lb. (Poisson's ratio doesn't figure into this directly, except in terms of the relationship between Young's and shear moduli, because the formulae effectively assume perfect incompressibility.)
For compression use Equation 5. (The shape factor has a big effect -- factor of 4.23 increase in force per displacement over simple Equation 2.) For displacement = 0.000346" (0.00880 mm), Young's modulus = 210 psi, Phi = 0.85 (semi-empirical factor out of the book), and r and t as above, I get F = 1.00 lb.
These assumed displacements here agree with those given in the table in my post #14.
>>in the compression example the top plate was bending around the bushing more than it was actually compressing the bushing. does this match the case for the equations you're using to get an estimate of what the reactions should be? ie in the shear case for example that there is no play in the Y direction or the X direction and that the bushing is in pure shear?<<
I don't know what the plate was made of, but if it is bending around the bushing in the compression case, Young's modulus for the bushing must be way too large (or that for the plate way too small). .The equations represent pure shear (no change in thickness) and pure compression (faces remain parallel and only thickness changes -- of course in the compression case there will be bulging of the edge of the bushing).
-- John Willett
lets find out the materials and go from there
>>lets find out the materials and go from there<<
Dear Jared -- I must apologize for leaving you hanging so long on this issue.
The reason for the delay is that I have learned from my friend that separate material properties can be entered both in the original part definition and in the simulation section of SolidWorks Premium. Apparently the latter supersede the former in the resulting simulation, so we're not certain what material properties were actually used during the bushing simulations in question. Until my friend can find time to run these simulations again with silicone-rubber properties that we know correspond to those stated in my OP, we will not be certain that we have any contradiction between SolidWorks output and my semi-empirical formulae.
The only question that I can reasonably ask at this point is, can SolidWorks Premium correctly simulate linear shear and compression strains in essentially incompressible elastomers (e.g., Poisson's ration = 0.499) as long as the strains remain small enough? If 0.499 is a too close to 1/2, is there an upper limit on the magnitude of Poisson's ratio that will work?
Thanks again for your help with this issue. I hope to be back with a more conclusive test before too long. -- John Willett
Question:Can I have a Poisson's ratio of 0.5 or greater in Simulation for isotropic materials?
Visible to Customer:
Answer:No, Poisson's ratio must be less than 0.5 for the isotropic material model. For hyper-elastic material models the values can get extremely close to 0.5, such as 0.4999. However, in general, values of Poisson's ratio very close to 0.5 can result in negative diagonal terms in the stiffness matrix which would result in solver termination.
>>Poisson's ratio must be less than 0.5 for the isotropic material model. ...in general, values of Poisson's ratio very close to 0.5 can result in negative diagonal terms in the stiffness matrix which would result in solver termination.<<
Jared -- I understand the theoretical limits. Would you say that 0.4990 was too close to 1/2 for SolidWorks Premium? If so, how close to 1/2 can we expect to get results? 0.495? 0.490? -- John Willett
according to the KB it should be fine. i think the issue here is we don't have tests that are equivalent. before we worry about the validity of the software, let's make sure the cases are consistent.
Yes, your interpretation is correct.
I assumed that you were incorporating your assumed material properties in the FEA and that the semi-emperical results were based on something real, like scaling from similar parts. If they were based on the same assumed material properties, then I am also confused by the results.