hi tony, what's the problem in the background? are you getting results you don't trust?
if you have small displacements, you're in the lower part of the linear range of the material and there are no inertial effects in your loading, a linear analysis should be fine.
Thanks Jared.. but no, no real problem.. just trying to firm up my understanding.
Say I wanted to analyze a plastic part.. very non linear material.. but I did not want to run
a full non linear analysis -- or I couldn't.
I believe that if I do a displacement based linear analysis (obviously static, no large displacements, etc)
that I should still get real strain results.
For example: Plastic cantilever beam. I use a linear material model despite the fact that the plastic is
very non linear. I deflect the end 0.1" -- lets say this is very small compared to its length, etc.
In this case, I think I could trust the strain results, but not the stress (because I'm not accounting for
the real S-S character of the material).
On the other hand, if instead of a 0.1" deflection, I use a, say, 1/4# load on the end. In this case,
strain is nonsensical, but I could trust my stress results.
I hope that made sense.
hi tony, why do you think that the deflection input method has an effect on the results? force vs displacement?
let's use this example, you create a 0.1" deflection, displacement is very small relative to length such that you know there is no change in the stiffness of the part (stiffness matrix) and you know that part of the stress strain curve is very linear.
one of the outputs of that analysis is the force required to create the 0.1" deflection. you remove the input deflection and replace with a force. the deflection remains the same.
does your theory still hold true?
Jared Conway wrote:
...and you know that part of the stress strain curve is very linear.
Thats the catch. In my hypothetical situation, you know the s-s curve is not linear.
But you're running a linear analysis (that assumes the s-s is linear).
As a result, strain is reported correctly (input is a prescribed displacement, not a load), however stress is not correct.. because
of the discrepancy between the linear s-s assumption (of the FEA) and the real life s-s behavoir (of the material).
to continue to beat the horse, the displacement based strain equation for a simple beam is
strain = (3*deflection*dist to neut axis)/(lenght^2)
note in the equation there is no material property (E).
'by the book', it does not matter (for strain) if the material is metal or rubber.
In a nutshell, I'm wondering if this is also true for FEA.
Given that no material properties are in the bending or axial stess formula you could argue that the stess is right but the deflection will be wrong if you apply a load. If you run a bunch of analysis you will find this is more or less true. However, since the deflection is incorrect that strain will also have to be wrong as the right stiffness is not used. FEA is a stiffness based method which is why it can solve indeterminant problems which are not solvable via statics. The elastics enables solution. The stiffest path takes the most load. Strain is strictly a function of curvature, regardless of regime - linear or non-linear.
If I understand you correct, you state that strain is correct due to the fact that you know the original size (from mesh) and you set the change in length by adding a displacement and that strain = change in lengt / original length.
It sounds reasonable, but the stress and the reaction forces should be wrong.
i don't think you can use terms "right and wrong" in such an absolute way. the stresses and strains and displacements will be based on what you input and they will be correct to that. will they match the physical behavior? maybe not because you've made assumptions. just document them or go with the right type of analysis with all of the appropriate components.
What I am saying is this: In my experience, the stresses will be about right (provided the small displacement assumption is valid) but the displacements will be worng because the stiffness is wrong. As far as I am concerned that is it and it doesn't matter how you load it and even this is a bit iffy and is really only applicable to non-linear elastic models. With plasticity all bets are off as the elements tend to turn to mush post yield. I am unclear as to the point of trying to logic ones way into some sort of confidence in this sort of estimate. It is what it is - a linear approximation. If you pick the right slope you can be right somewhere.....
Bill and Jared.
I really appreciate your posts in the simulation forum. Your knowledge and experience in this very complex area is important for "newbie’s" like myself.
My response was only based on the little knowledge that I have on linear simulation.
In linear simulation (small displacement and linear elastic material):
If I put a force on a part, the stress will be the same regardless of material. Stress = Force / Area.
So if I have a part made of rubber or steel and load it with a force (N or lbs), the stress will be similar. The deflection and the displacement will be different due to the different stiffness of the materials. But if your only interested in stress, not displacement nor strain, it doesn't matter what material you select for you simulation in this case.
In the same manner, as I understood Tonys example, if you in a linear simulation add a displacement to a part, instead of a force, the strain will be the same regardless of material. Strain = change of length/original length and the original "length" is given by your mesh and the "change in length" is given by your displacement/advance fixture. In this case, the reaction force and the stress will be different depending on the material you select.
Non-linear is above my "paygrade" so far :-)
Have a nice weekend.
If you have strain failure critria, you method ought to be valid for a constant strain situation (like a tab). If have a constant stress situation (like a window under water), though, you should probably be more worried about creep. You can use the creep modulus in place of the Young's modulus in a linear simulation. You'll have to calculate the creep modulus for the working life.
The more I think about this method, the less I like it. I think it might only work in uniform strain. I think that if you have a significant strain gradient, the strain will not be distributed correctly, since the increase in stress should work to limit strain in high strain areas. In other words, I'm not sure the lowest energy state for a given load is the same in linear s-s as it is in non-linear s-s unless the strain is uniform--such as a rod in tension.
Maybe somebody with a more sophisticated grasp of solid mechanics could weigh in.
Thanks all, this is exactly the sort of discussion I was hoping to prompt, and Mike's latest post are exactly the
kind of questions I'm asking myself.
Typically in analysis of plastic parts the only clear failure data one might have is strain to yield.. and plastic has
a nasty way of being non-linear / rate dependent / etc.
By and large in plastic design its usually the desplacements we know most clearly.. ie a snap needs to get past
and over a retention features.. an annular ring is force to snap into an annular groove. The amount of displacement
is very well understood.
Hand calculations here are usually much faster -- and as we said, in a displacement/strain situation, material
properties are irrelevant (in the theoretical formulation).
But as Mike mentions this may only be valid for a limited set of cases (low strain gradient) -- jury is still out.
Would love it if someone with the mechanics background could weigh in on whats really happening behind
the FEA curtain in terms of the numerical formulation of the theoretical problem.
Bill: yes, only applicable to non-linear elastic.
To give a very very poor analogy: hand calculations for cantilever in bending make no mention of poisson's ratio..
however, if you try to simulate, one has to be very careful to either set the ratio to zero, carefully define the
restraints, or go to, say, a beam element.. to get agreement between theoretical and FEA.
If you choose the right material model, your ability to predict the physical behavior should be pretty good. That's why the software has multiple material models. But if you want to do everything with a linear material, don't expect the results to be correct. That is why we have different analysis types.
The equations and methods are thoroughly documented in the help and also the old geostar manuals that are in the swx kb.
But in the end, it sounds like for you, you need to prove this to yourself by analyzing some samples and comparing them to simulation and your hand calcs. I had a customer just do that with the hyper elastic material model for their masters thesis. Everything in simulation was dead on once they had the right material model and material curve.
Thanks Jared, all very valid points. Sometimes we don't have access to different material models (not all of us here run
the premium license).. or more often than not we don't have the true material properties (s-s curve).
It'd be mighty handy to speed up a full blown NL analysis (and be confident in whats happening).. by running a linear
static analysis and comparing the strains to failure strain.. completely disregarding the stress values.
I suppose benchmarking against the lab tests is the way to go, as you suggest.
I'll certainly have a look at the geostar manuals (didn't know they were out there).. if I could find out exactly what the
FEA engine is doing, might save myself some lab tests.
I think i'm missing something here. You're saying the stresses are no good because the incorrect E is being used to calculate them because the user is using a linear material curve rather than nonlinear?
Stress is not correct because E is not correct. (rather it is likely that its not correct).
Strain is correct because it is independent of E.
& I have/know/can find strain failure data more easily than stress failure data.
(Again, this is only in the cases where my boundary condition is a prescribed deflection.
If i'm using a force instead of deflection, then the argument is inverted: Stress
is correct but strain is not).
I think the most important point in this discussion was made by Mike. Your approximations only make sense when the strains are close to uniform. When the strains are very non-uniform, the approximations lose their value.
I have more faith in your displacement based analysis, as I have used it successfully in the past to design plastic snaps. The strains are not at all uniform, but the results seem to work out pretty well, in terms of whether or not the plastic fails. I think it is probably because the highly non-linear reactions are confined to only a small fraction of the volume. As you noted, the analysis does not give a very good answer for the forces required.
The bottom line is, if you really want to know what it happening when operating in the non-linear regime, you will have to run a non-linear analysis. Any linear analysis is highly suspect, although it may help you get a handle on the qualitiative aspects of how the system will respond.
Thanks all.. some good thoughts here.
I'd like to summarize where some of my soul searching has taken me, thanks in large part to the responses here.
SW simulation is a displacement-based analysis package. IE all loads, b/c's, etc will be reformulated in terms of
displacements.. ie a force(load) will be reformulated effectively as a displacement as the software converts that load
to displacement via the material properties to develop a stiffness matrix, and searches for equilibrium.
In a linear analysis, that stiffness matrix never changes / is updated.
So in my hypothetical "displacement-loaded" linear model approximation of a non linear material, assuming the
strains are uniform, the answer should be in the ballpark.
A force analysis, however, would be reformualted using the material properties so stress results would be rubbish.
Does that sound like a fair summary?