# How I Set the Curve: Using Stress-Strain Data in SOLIDWORKS Simulation

A Stress-Strain curve is a collection of data describing how resistant a material is to stretching. Naturally, if you are looking to run a stress analysis on your products in SOLIDWORKS, there’s a good chance you know this information may be important too. The first thing to determine about Stress-Strain curves is when you actually need to use them. If you've ever seen one, you know that it’s usually a line graph with stress on the y-axis and strain on the x-axis (typically from a uniaxial tensile load). You likely know that for ductile materials like metals, there is a relatively straight, steep section at the beginning followed by a sudden bend and then a section with more curvature. This bend is known as the yield point, at which the material begins to deform permanently (and generally do interesting things).

In most cases, yielding is rather undesirable, so engineers are trying to make sure the maximum stress in a product doesn't get close to the yield strength. If that’s true for you, the full stress-strain curve isn’t needed; a quick-running Linear Static stress analysis in SOLIDWORKS ignores the post-yield behavior and only requires Young’s Modulus to be entered, a simple number that describes the straight, elastic region of the curve.

If you are looking to see the real behavior of the material even after yield (like a sagging Beam or your Phone being dented on the ground), you’ll need to run a study that allows a Plasticity material model, such as Nonlinear Static or Drop Test. Assuming you have chosen an appropriate study type, the option will be available under the Model Type drop-down in the Material Library. There are multiple Plasticity models, but the most common one is the von Mises model, which assumes yielding occurs when the von Mises equivalent stress (published in 1913 by a suave young Austrian) exceeds the yield strength.

The stress-strain curve can now be defined on the Tables & Curves tab under the “Type” drop-down menu. In this case, the curve is already visible because I’ve picked one of the default SOLIDWORKS materials that include the data, noted by the “(SS)” annotation at the end.

If you want to use a material that isn’t in the library or doesn’t have the stress-strain curve, you’ll need to create a custom material and fill in this table (default SOLIDWORKS materials cannot be modified). Additional Stress-Strain curves are available in the file “cosmosworks curves.cwcur” under [SOLIDWORKS Installation directory]\SOLIDWORKS\Simulation\CWLang\English. Access these by right-clicking the name of your study and selecting Define Function Curves.

It’s important to be careful when entering the data as three common mistakes can occur if you are not paying attention.

First, make sure the units match your material data before you fill in the table. Strain is always entered as a decimal (i.e. 1% strain is 0.01), and in this example, stress has been set to N/mm^2 or Megapascals. If you change the stress unit after entering the data, SOLIDWORKS will convert the values for you, making them very wrong very quickly. The cells can be filled in by clicking in the table and typing, or by pasting (Ctrl+V) copied data from an external spreadsheet program such as Microsoft Excel. HTML tables, text files, or other documents may work as well.

The second common mistake is not putting the correct range of values in the table. If you've obtained Stress-Strain data from a material vendor or text, it probably starts at a strain of 0, indicating no load applied from the test fixture. In SOLIDWORKS however, only the post-yield information needs to be entered because the pre-yield region of the curve is assumed to be perfectly linear and perfectly elastic (or, a straight line with the slope of the Young’s Modulus). So, the first cell in the table should always be at the yield stress of the material (this is why the preview of the curve may look different than your source). Ideally, the last entry for the stress-strain curve will be the fracture point of the material (when it literally broke), so remember that any areas of your model showing strain above this value would, in reality, be cracking and coming apart.

Finally, one more adjustment may be necessary depending on how the strain information of your material was provided. By default, SOLIDWORKS Simulation uses the more common engineering strain, which is simply calculated as the change in length of some material divided by its original length:

By contrast, true strain (some would call it perfectionist strain) is calculated as the natural log of a material’s final length divided by its original length:

If your Stress-Strain data was supplied using this more precise true strain calculation, you’ll need to go to the Properties menu (right-click on the name of the study in the analysis tree) and select “Large strain option". The option is aptly named using a curve defined with true strain, which will be more accurate at extreme deformations where the cross-sectional area of the material begins to shrink from stretching.

Assuming you've checked these steps off your list, upon running the study you should be warmly greeted by results showing realistic stress, displacement, and strain of your design even after yielding.

In fact, by using the Probe tool on a displacement plot and clicking the Response button, it’s often easy to see the yielding in the material occurring as the load is applied followed by the permanent deformation when the load is removed.