Back when SolidWorks was new, and FEA simulation was the purview of dedicated specialists, I could assume that anyone who is using the SolidWorks Simulation must already have an engineering degree. That’s not so anymore. The widespread adoption of SolidWorks by Industrial Designers, Artists, Machinists, and other creative trades, has democratized the 3D CAD user base. The Simulation tools are now available to a much wider audience.
I get two or three hotline calls a month from people who are trying to research, or interpret, material properties for doing an FEA simulation. Not that I mind that! I’d much rather have someone call in-person with a question, rather than to just take their chances with some Internet searches. There is a particular hazard to Wiki-Engineering. You can seem to get exactly the right answer, quickly, and only later find out that it was the right answer to a slightly different question. The more technical trades are fraught with such small but meaningful variations on terms, scope of applicability, etc.
And the frequency of such inquiries is rising, so it’s time to consolidate a lot of our replies into a blog post. So I’m going to do a couple of extended tech tips, each one on a critical Material Property you have to input into a simulation. Then I’ll do a follow-on series on how you interpret the stress and strain results.
In the SolidWorks Simulation dialog for Material Properties, the fields colored RED are the ones that are absolute must-have to perform the analysis.
Must-Have: Elastic Modulus
The Elastic Modulus is the single most important property you have to get right when setting up a Simulation.
Each Finite Element in your mesh is essentially a spring. It is not a simple, one-directional spring, but in fact is a six-dimensional spring, but it is a spring nonetheless. And the most important property for determining how that spring will flex under a load, is to know the stiffness, or Spring Rate. When you buy a simple coil spring, you specify the Spring Rate as some number of pounds per inch:
The spring rate depicted above is not solely a function of the spring material, but also the spring geometry – especially the wire diameter, coil diameter, and the number of turns. But for FEA we need a more generic property, one of the materials only, independent of the shape. That generic stiffness property is called the Elastic Modulus. It is also frequently called Young’s Modulus, and also Tensile Modulus – all are exactly the same thing. It is arrived at by putting a dog-bone shaped strip of the material into a tensile-tester, and pulling on it in the long-wise direction, (oriented vertically in the figure below).
Getting test data
Test set-up for measuring Elastic Modulus of a thin strip of material. The machine gradually applies an increasing force, and graphs the ratio of force for each increase in length.
The raw data from the testing machine is in the exact same form as in the catalog listing we saw earlier – the Spring Rate is a force per unit change in length. But – we can generalize this result, first by computing what the Stress must be in the controlled, constant-thickness area of the dogbone. If the original thickness of the dogbone was, say ½” both ways before the test, then the cross-sectional area of the specimen would be 1/4 sq. in. At a point where the machine recorded a force of 100 lbs, we would report this instead as a stress of 400 psi.
s = Engineering Stress = Force / original cross-sectional area
s = F / A
If we did the test pictured above, on a specimen with a length of 10 inches, and then repepeated the test a day later on a specimen that was machined to be 20” long, you would expect different results – the longer specimen would be less stiff, so would stretch more than the 10” specimen, for the same input stresses. So the second way we must generalize the test result is to make it independent of the length of the particular dog-bone we used. We don’t actually report the growth of the specimen, as a deflection in inches. We instead report the Strain – the percentage that the specimen grows, compared to its original length.
e = Engineering Strain = change in specimen length / original specimen length
e = dL / L
So the Young’s Modulus (aka Tensile Modulus, aka Elastic Modulus) you must input to Solidworks Simulation, to represent the generalized stiffness of our Finite-Element springs, is the Engineering Stress divided by the Engineering Strain. Strain is a change in length, divided by length, so it actually has no units. Stress has units of psi, (or in SI, Pascals, which is Newtons per sq. meter). So the units of the Elastic Modulus will also be in PSI (or Pascals);
E = Elastic Modulus = s / e (lbsf/in2 or N/m2 )
OK, on a good day, your Simulation system should help confirm good design intuition, so here’s some hard numbers to help ground you. Let’s look at a plot of Engineering Stress, vs. Engineering Strain, for a typical metal.
An average Steel can withstand a Stress of about 60,000 psi before starting to take permanent damage. The Strain at the point of yielding is usually about 0.2 % of the test-specimen length, or about .002
The Elastic Modulus, then, is the SLOPE of the graph above. You can see that across the useful, working stress levels of this material, the slope is pretty near constant. Wonderful!!! Engineers just love things that are linear! So what exactly IS the Elastic Modulus of the steel plotted above? As long as we keep the stresses within the useful, working limit at the left side of the graph, then Young’s Modulus is:
E = 60,000 psi / .002 = 30,000,000 psi.
That’s not wrong; 30 million. I get calls about this. Young’s Modulus is big. Expect big numbers. Since the Strain at which most metals start to tear is a relatively small number, (and even plastics will have working-strain limits of about 1% or 2%), you are looking at a pretty big number that is always divided by a really small number.
Typical values of Elastic Modulus:
Steel 30,000,000 psi
Nylon 6/6 400,000
Second common source of errors when inputting Elastic Modulus; Beware of the European Comma!!!
If you are researching a material, (especially a plastic) from Bayer or Sabic or some other non-USA locale, remember that they frequently use the comma as a decimal separator, instead of the period. Since a Pascal is a much smaller unit of stress than PSI is, you get even bigger numbers in SI, and so E is reported sometimes in Pa, and sometimes in MegaPascals, Mpa - Pascals x106
If you’re looking at a data sheet expecting unusually large numbers, anyway, and some European university or material provider or design agency lists a value of 12,600 Mpa, understand that it is not 12.6 thousands of MegaPascals, it is in fact 12.6 MegaPascals, the comma is a decimal. Tricky!!!
Finally, if you are researching a plastic material, you sometimes get no information on Elastic Modulus, you instead get a Flexural Modulus. What’s up with that? The short answer: If you are given only a Flexural Modulus for a plastic, you can usually assume this is the same thing as the Elastic Modulus, they are near enough to the same thing but arrived at by way of a different test.
More nuanced answer: Many plastics have a lot lower stiffness than metals do, and most annoyingly, the useful working portion of their Stress-Strain curve is very often not terribly straight – (see below).
Another thing that goes on with plastics is that they can exhibit a great deal more stiffness when loaded in Compression, then when loaded in tension. For many metals, we don’t worry about this distinction. But just imagine for a moment that you have a design for a living hinge, or a spring clamp, or some other thin-walled plastic thingy that expects to see a whole lot of bending forces.
The upper side of the beam above will be loaded in compression, the lower surfaces, in tension. For a material that was equally strong in tension as in compression, you would expect the neutral surface (dashed line) to be right in the middle of the beam. But for many plastics, the compressive stiffness is higher, the tensile stiffness is lower, and so the neutral surface shifts upward, (a smaller net cross-sectional area in compression is stiff enough to resist the larger cross-sectional area under tension). If you simply assume that the Compressive stiffness and the Tensile stiffness are the same, you would under-predict the overall strength of the beam.
The ASTM test for Flexural Modulus will therefore subject the test specimen to pure-bending instead of pure-tension. You then report the Flexural (Bending) Modulus by hand-calculating from the measured load, what the bending-moment must have been, and then from this number you back out the peak tensile stress (bottom surface) and compressive stress (top surface) – As if they were the same, (so as if the neutral axis were in fact in the center). What this does is give you a number that is generally stiffer than the real pure-tensile stress, but lower than the real pure-compressive stress. It’s a pretty good average.
SO: If you are simulating a plastic part that is loaded mostly in tension, input the Elastic Modulus. If it is loaded mostly in bending, (or is subjected to a wide mixture of stress directions in the most-highly loaded regions), input the Flexural Modulus as the Elastic Modulus. And if your chosen vendor gives you ONLY the Flexural modulus, then the choice is easy!
The next tech tip in this series will explain Poisson’s Ratio. It has nothing at all to do with fish.