Understanding stress vs. strain is fundamental for engineers working with material properties. However, a critical distinction exists between the stress-strain data obtained during tensile tests and the true stress-strain data required for accurate simulations in software like Ansys Mechanical.

In this article, we’ll uncover the essential differences, explain how to calculate true stress and strain, and explore why these concepts are indispensable for accurate elastic-plastic material simulations.

What is Measured and Calculated During Material Tensile Testing?

If you were to internet search for a material’s stress vs. strain data or look in the back of an engineering mechanics textbook, the stress vs. strain data provided is typically in the form of engineering stress and strain. Tensile testing for stress vs. strain is performed using tensile coupons like the layout shown in Figure 1.

This layout includes data that is measured as part of the test, where:

• P = the applied load
• A = the initial cross-section area
• l₀ = the initial extensometer length
• l = the new extensometer length after applying load P

The calculated stress and strain are:

σ_engineering = P / A

ε_engineering = (l – l₀) / l₀

These are engineering stress and strain because the calculation is performed using the initial cross-section area. However, as the tensile coupon is loaded the cross-section area reduces due to the Poisson Effect. For small values of stress and strain, the difference between engineering stress and strain and true stress and strain is low and approximated as equivalent.

Determining True Stress and Strain

There’s a handy pair of equations to calculate true stress and strain using the calculated values.

σ_true = σ_eng (1+ε_eng)

ε_true = ln (1+ε_eng)

These are simple to evaluate using the engineer’s second-best tool, Excel (the first being Ansys, of course).

Why is this Distinction Important?

You may be saying to yourself, “This doesn’t seem like that big a deal. Why are you telling me this?” It’s important to understand how simulation codes perform finite element calculations.

Let’s consider a hypothetical test procedure, where we take the tensile test coupon shown in Figure 1 and stretch it from 10mm to 12mm. This is a change in length, ∆l, of 2mm. Using the equation above for engineering strain, we can calculate an engineering strain value of:

ε_engineering = 2/10 = 0.2 mm/mm

Okay… straight forward. Let’s break that up into two steps on a second tensile test coupon. Step 1 will stretch the coupon from 10mm to 11mm and step 2 will stretch it from 11mm to 12mm; then we can simply add these two strain values to get the total strain. Pretty simple, eh?

ε_engineering = 1/10 + 1/11 = 0.191 mm/mm

What you should notice is that these two measurements do not produce identical strain values, despite both tests stretching the tensile coupon the same amount. So, what does this mean for simulation?

The second tensile test, where strain is calculated in incremental stages, directly resembles how strains are calculated in Ansys Mechanical simulation from incrementally applied loads. If analysts use engineering stress and strain as input to the plasticity material models in Ansys Mechanical, each additional increment in load represents error in the strain calculation.

Let’s redo the calculation above using true strain. The third tensile test coupon:

ε_true = ln (12/10) = 0.18232 mm/mm

And the fourth:

ε_true = ln (11/10) + ln (12/11) = 0.18232 mm/mm

As you can see, we calculate identical results using true strain. This behavior is desirable in Ansys simulation and is why Ansys Mechanical requires using true stress vs. strain as input for the elastic-plastic material models.

In fact, if you peruse the Ansys Help documentation you’ll find this note:

Hmmm… this just stated what I spent ~600 words saying. That’s alright; hopefully the illustrated examples with the tensile test coupons are helpful.

Where Else Can Analysts Learn About Ansys and Plasticity?

If you are interested in learning more about Ansys and plasticity in simulation, DRD has on-demand training content on our website. This particular topic is covered in our Nonlinear Structural Simulation course, in Chapter 3.

Ansys Mechanical Nonlinear Structural Simulation – DRD Technology

Released on July 23, 2024, Ansys Mechanical 2024 R2 introduces a powerful new native feature: Fluid Penetration Pressure. While this isn’t entirely new to Ansys, as it has long been part of Ansys APDL, it’s the first time this functionality is available natively in Ansys Mechanical. This feature provides engineers with an efficient way to simulate fluid interactions with structures without explicitly modeling the fluid in finite element analysis (FEA).

What is Fluid Penetration Pressure?

Fluid pressure penetration is a method to capture impinging fluid on a structure, without explicitly modeling the fluid in the finite element analysis.

The fluid penetration pressure method employs information of contact status between contacting bodies to determine where the fluid pressure is applied. The benefit is that this is determined as the contact status evolves over the simulation time, so the region where pressure is applied changes as contact between bodies changes under loading.

Users provide a contact region for the searching algorithm, a starting location for fluid impingement, and the fluid pressure; the solver does the rest. Figure 1 provides a simple view of the starting point on the exterior surface of the structure and the ‘flow’ of the fluid outward.

Figure 1: Schematic of Fluid Penetration Pressure Behavior

What is the Application of Fluid Penetration Pressure?

As you perhaps have guessed, the application of fluid penetration pressure is in seals and gaskets for valves, hydraulic cylinders, coil-overs, etc. This allows determination of sealing surface leakage as the structure is loaded and deforms, both from the fluid pressure itself and additional loads in service.

Figure 2: Examples of Gaskets

If engineers can determine seal capability before selling the product, expensive redesign can be circumvented. Seals do not need redesign, re-machining of the sealing surfaces is lessened, and a potentially hazardous leak can be avoided.

Example Simulation with Fluid Penetration Pressure

Here we have a simple representation of a tube, sleeve and O-ring seal in a vehicle strut or coil-over. During the assembly process, the tube is pushed downward to interface with the O-ring. In service, fluid is pushing against the seal from the top in the shown orientation, annotated by the blue arrows in Figure 3. The sleeve is fixed in place.

Figure 3: Layout of Simulation with Fluid Impingement Load Direction

As stated previously, analysts need to supply a contact, a starting point, and a fluid pressure magnitude. In the 2D axisymmetric representation of the structure in Figure 3, frictional contact is defined between the three bodies. The Fluid Penetration Pressure object is defined as shown in Figure 4.

Figure 4: Example Use of Fluid Penetration Pressure Feature, Details, Load, and Graphics

As you can see, we’ve applied the fluid pressure in the second load step; the first load step is moving the tube downward.

I’ll leave you with these final output animations, and a recommendation to visit our website to get access to on-demand training.

We walkthrough this simulation example as part of our Ansys Mechanical Nonlinear Structural Simulation course. Follow the link here: Ansys Mechanical Nonlinear Structural Simulation – DRD Technology.

In our last blog post of this series, I dive into how we can simulate cracked structures using Ansys simulation software, Ansys Mechanical. As before, if you’ve not read the previous two posts, go back and read ‘em!!! 

How Engineers Use Ansys Mechanical Software to Model Cracks 

Ansys Computer Aided Engineering (CAE) simulation software allows engineers to study cracks in structures via fracture mechanics, along with a host of other structural simulation needs. Ansys has a long history of simulation development since the 1970’s in creating tools for engineers to design and virtual prototype their products. As a quick note, Ansys is not limited to just structural physics either. Fluids, electromagnetics, systems and optics are some of the other fields Ansys offers in its portfolio of simulation capabilities. 

The options to create a crack in Ansys simulation software generally fall in two categories: either a) use a CAD surface that represents the crack, that overlaps with the structure or b) use the auto-generation tool in Ansys to add a crack at the mesh level. 

The former works well in all scenarios but is very useful when the crack is not a simple analytical shape, i.e., a penny-shaped crack. The latter is great for those simple, penny-shaped cracks, where the engineer can input two radii to define the shape, input where the crack is located, and they’re done. 

Here’s an example; take this simplified cast bearing/shaft support. The machinist finds a crack when machining the bearing support housing (outlined in the blue box). Perhaps this is caused by an incorrect casting process. 

Representative CAD Model, Crack Surface on Right 

When magnafluxed or cut open, the crack is not a simple shape. This is perhaps an extreme example, but it gets the point across. With a few inputs and clicks, Ansys overlaps the crack surface with the solid CAD, splits the mesh where these intersect, buffers the elements from the new crack mesh into the existing base mesh, and voila! The finite element model crack is ready to analyze.

Representative Finite Element Mesh of Structure with Crack Inserted: Back View on Left, Top View on Right (with red line indicating part boundary) 

What About Crack Growth? 

Ansys requires no special treatment of the crack to determine the relevant fracture parameters when evaluating a crack for simple comparison to material fracture toughness. The simplicity of the Ansys workflow mirrors the simplicity of what the engineer is after, i.e., a single value for Stress Intensity Factor. Using the methods described previously, engineers can model a crack and then mesh the structure with hexahedra, tetrahedra, or a mix of element shapes and get results for Stress Intensity Factor. 

For fatigue cracks, the requirements are greater. Engineers must provide the crack growth equation constants, i.e., the Paris constants C and m, then Ansys will do the rest. Ansys’ technology for general, 3D crack growth is quite extraordinary. This technology is referred to as SMART – Separating, Morphing, and Adaptive Remeshing Technology. To put it simply, automatic remeshing occurs as the crack grows in simulation. 

Representative Crack Growth Simulation Showcasing Automated Solution Remeshing 

For a nice overview of fracture mechanics in Ansys, you can watch an on-demand webinar on DRD’s website. In the webinar, I provide a brief overview of fracture mechanics and Ansys capabilities in fracture analysis, much like this paper. I also discuss damage tolerant design, material data acquisition, and Ansys CAE simulation of cracks in structures. 

Head over to DRD’s website for two on-demand webinars I conducted in October and November, ‘Simulating Crack Propagation Part 1 and 2.’ 

https://www.drd.com/resources-all/simulating-crack-propagation-part-1-webinar-recording/ 

https://www.drd.com/resources-all/simulating-crack-propagation-part-2-webinar-recording/ 

This concludes our 3-part series on fracture mechanics. We have a few other resources engineers can dig into on this topic, including the two on-demand webinars mentioned above. DRD has a fracture mechanics training course that I teach as demand requires, https://www.drd.com/project/ansys-mechanical-fracture-mechanics/. If you are interested in this course, please let us know at support@drd.com. 

Let’s continue our discussion on fracture mechanics with this second blog post, where I dive into the methods engineers have available to evaluate cracked structures. If you’ve missed part 1 of this blog series, go back and read it here. 

Stationary, Static and Fatigue Cracks 

When evaluating a structure with cracks, engineers have a few options with respect to the level of involvement in solving the problem. From least to most involved: 

• Stationary: review of status of crack, ignoring crack growth. 
• Static: review of status of crack under single, monotonically increasing load, crack growth is assumed. 
• Fatigue: review of status of crack under cyclic loading, crack growth is assumed. 

Stationary cracks provide an instantaneous view of the state of a crack in the structure. The engineer can only know one thing from this type of analysis: will the crack grow or not. No insight is provided into the second and third of the common questions asked in the previous section. Simple closed-form solutions are available for engineers to estimate the integrity of a cracked structure, and these can be found in literature reviews and textbooks. Many closed-form solutions take the resulting stress field caused by loading, the current crack length, and an empirically determined factor to determine stress intensity. A few examples are shown here, for plate geometry of varying sizes. 

Image Source: Elementary Engineering Fracture Mechanics, 4th Ed., Broek, pg. 85 

Static cracks allow the engineer to determine if a crack will grow and fast fracture, or if the crack will arrest. Static cracks are subjected to a single, increasing load, from unloaded to fully loaded. In this case, we are not interested in a time frame for the crack to grow or arrest; ultimately, engineers simply determine if the structure will break with the presence of the crack. 

Fatigue cracks, or fatigue crack growth, is the most complex case, both for understanding and to consider when designing a product. Fatigue crack growth considers the structure under cyclic loading, where the structure is repeatedly loaded and unloaded. There are variations to this load pattern as well, which we will not go into here. 

When it comes to fatigue cracks, there are additional test procedures to determine a crack growth rate versus the applied stress intensity. Engineers will typically see this abbreviated as da/dN vs. dK, i.e., the change in crack extension (da) over cycles per extension (dN) vs. change in stress intensity (dK). Like critical fracture toughness, every material will have a different crack growth curve. Examples of some different material curves are shown here. 

Image Source: Effects of ductile laminate thickness, volume fraction, and orientation on fatigue-crack propagation in Ti-Al3Ti metal-intermetallic laminate composites, Adharapurapa et al, 2005. 

The unique aspect of fatigue crack growth that harkens back to what Griffith found is the stress levels in the structure can be much less than those that would normally cause plastic collapse. Cyclically loading the structure will continue to grow the crack, under no threat of plastic collapse, and when the maximum stress intensity factor is less than the critical fracture toughness; we call this subcritical crack growth. 

Most crack growth data focus on this subcritical crack region, however, two other regions exist. Let’s limit the data shown in the previous graph to one material’s data set and expand the representative data out; we get a graph that looks like this. 

Image Source: A review of fatigue crack propagation modelling techniques using FEM and XFEM, Rege et al, 2017. 

The material data mentioned fits into the area marked ‘Region II’; on a log-log plot of crack growth rate versus change in stress intensity, this is commonly referred to as the Paris regime, and it is generally a straight line on this plot. A simple equation is used to describe this region, which takes the form of: 

where C and m are material constants determined via the graphed data. The other two regions, I and III, refer to the threshold and fast fracture regions, respectively. The threshold region describes when the crack grows slowly, either by small stress intensity or small crack size. Conversely, the fast fracture region describes rapid crack growth, which may result in surprise failure of the structure. Engineers use this crack growth data in damage tolerance assessment. 

In both the first and second blog posts, I’ve not touched on Ansys simulation to solve fracture mechanics problems. In the next blog post, I will discuss Ansys’ capability to model cracks and solve crack growth problems. 

Before we jump into the topic at hand, I’d like to introduce myself. My name is Alex Austin, and I am the Structural Team Lead at DRD Technology, an Ansys Channel Partner. I studied Mechanical Engineering at the University of Tulsa, OK, from which I graduated with a BS and MS in Mechanical Engineering a little over a decade ago (woo… it’s already been that long!). My graduate work was in the fatigue and fracture space. My primary area of expertise is structural mechanics; as many engineers may know, this is quite a large field of physics when we look at Ansys simulation capabilities. Fracture mechanics is a small part of that overall field, is relatively new in the world of engineering, and is very complex. 

What is Fracture Mechanics? 

When engineers evaluate stress in a structure, the common, simple equation that comes to mind is stress = force/area. This equation carries several assumptions: static equilibrium, uniform cross-sectional area, uniaxial stress, to name a few. With the introduction of a crack to the structure, the state of stress at the crack tip is not uniaxial. Cracks are sharp corners, or notches. In the computer simulation (finite element) world, we call these singularities. In fact, singularities are locations where the theoretical stress is infinite. A strength of materials approach does not account for these singularities. When a crack exists, we need a method to analyze it. Fracture mechanics is that method. Fracture mechanics is the study of crack propagation in materials. 

Image Source: Wikipedia 

Motivation for Fracture Mechanics 

Often, cracks naturally form during the manufacturing process, either through casting or machining methods. Cracks can exist in a product and never cause issues with the working of the structure. In fact, cracks may be invisible to the naked eye. However, when this is not the case, what happens? 

Let’s say we’ve designed and manufactured structure that is currently out in the field, and our customer notices a crack… is this a problem? Let’s say a customer reported cracks popping up on some rotating machinery housings and they simply asked, ‘Is this a problem?’ though, the more likely case is no questions and, ‘Please fix this!!!’. What is the engineer typically tasked with determining? The common questions we ask are: 

1. Will the crack grow? If so, 

1. How quickly will the crack grow? And then, 

1. Will the structure fail catastrophically? 

As stated, the customer absolutely thinks the presence of a crack is a problem. This is commonly the case when the customer is not an engineer, and even if they’re an engineer, they had no insight into the design and manufacture of the product. Answering the above questions will directly determine if the crack is or is not a problem. 

What about the case where the engineer designs a structure and during the design process must consider a structure that has cracks? This is a common practice in regulatory bodies, namely, the FAA (Federal Aviation Administration). In this case, the engineer assumes a crack or cracks exist in the designed components and must design for this potential failure mode. This is referred to as Fatigue and Damage Tolerance. The engineer establishes inspection intervals for components based on this analysis. The maintenance crew knows how many hours the component can be used before it needs to be checked for integrity and possibly replaced. 

In the next blog post, we will discuss the methods to evaluate cracked structures.