SolidWorks Simulation Setup

SimulationXpress vs. Simulation Standard

SolidWorks 2025 ships with two simulation tools. SimulationXpress is free with every SolidWorks license—it is already on your machine. Simulation Standard is a paid add-on with more capabilities. Both will work for this lesson. The table below shows what each one can do.

Step-by-Step Walkthrough

Follow these seven steps in order. Each step builds on the one before it. If something goes wrong, check the troubleshooting reference before moving on.

1. Open the test bar part file

   Open Test-Bar-80x10x4.SLDPRT from the lesson repository’s files folder. This is a simple rectangular bar: 80 mm long × 10 mm wide × 4 mm thick. These proportions follow the ASTM D790 standard for three-point bend testing, which calls for a 16:1 span-to-depth ratio. Using a standard shape means our physical test results will be directly comparable to published data.

   Verify the part opens without errors. You should see a single solid body in the FeatureManager tree.

2. Create a new static study

   Simulation Standard path:

   Go to the Simulation tab in the CommandManager. Click New Study. Select Static and name it 3pt-bend-PLA. Click the green checkmark.

   SimulationXpress path:

   Go to Tools > SimulationXpress. The wizard opens in the Task Pane on the right side. Click Next on the welcome screen to begin.

   In both cases, SolidWorks 2025 creates a study tree at the bottom of the FeatureManager. You will see empty folders for Material, Fixtures, Loads, and Mesh.

3. Assign custom FDM PLA material

   This is the most important step in the entire setup. SolidWorks includes a built-in PLA material, but those properties assume injection-molded plastic. FDM-printed PLA is weaker and more variable because of layer adhesion, infill patterns, and print temperature. We need to create a custom material that reflects how our actual printed parts behave.

   How to create the custom material

   In the study tree, right-click the part name (or the Material folder) and select Edit Material. In the Material dialog, click the Custom tab. Enter the name FDM PLA — 100% Infill and fill in these values:

   Property	Value	Notes
   Young's Modulus (E)	3,300 MPa	CNC Kitchen 3-point bend data; peer-reviewed range is 3,000–3,500 MPa
   Tensile Strength (UTS)	50 MPa	Conservative mid-range from published FDM PLA data at 100% infill
   Yield Strength	40 MPa	Approximate onset of plastic deformation for FDM PLA
   Poisson's Ratio	0.35	Standard value for PLA
   Density	1,240 kg/m³	PLA material specification

   After entering the values, click Save to store the material in your custom library, then click Apply and Close. The part in the graphics area should update to show the assigned material.

   Why these numbers matter

   These values are averages drawn from multiple published sources. Your actual filament, your printer, and your print settings will all cause variation. A spool of PLA from Brand A printed at 210 °C will behave differently from Brand B printed at 200 °C. Engineering accounts for this uncertainty through the Factor of Safety—you deliberately design parts to handle loads well beyond what you expect, so that real-world variation does not cause failure. We will examine FoS results in Section 4.

4. Apply fixtures (supports)

   A three-point bend test has two supports on the bottom of the bar and one load point on top at the midspan. We need to tell SolidWorks where the bar cannot move—those are the fixtures.

   Simulation Standard: Right-click the Fixtures folder > Fixed Geometry. Select the two narrow bottom edges (or small faces) where the physical supports would contact the bar. These represent the two outer support points in a three-point bend rig.

   SimulationXpress: In the wizard, click Add a Fixture. Select the bottom faces at each support location and apply Fixed.

   Common mistake: over-constraining

   Do not fix the entire bottom face of the bar. Fixing too much surface area locks the part down so rigidly that it cannot bend the way it would in real life. The simulation will report artificially low stress and displacement. Only constrain the faces or edges that correspond to where the physical supports actually touch the specimen.

5. Apply the load

   Simulation Standard: Right-click the External Loads folder > Force. Select the top face of the bar at its midpoint. Set the force to 50 N directed downward (negative Y, assuming Y is up in your coordinate system). Click the green checkmark.

   SimulationXpress: In the wizard, click Add a Force. Select the top face at the midpoint. Enter 50 N directed downward.

   Why 50 N? It is a convenient starting reference that produces measurable stress and displacement in our bar without exceeding the yield strength. Think of it as roughly the weight of a 5 kg mass pushing straight down. We will compare this predicted stress to actual test data later.

   Quick check — weight to force F = m × g = 5 kg × 9.81 m/s² ≈ 49 N ≈ 50 N This is why 50 N is a practical lab-scale load.
6. Mesh and solve

   Right-click the Mesh folder and select Create Mesh. For your first run, accept the default mesh settings. Note the default element size that SolidWorks 2025 assigns—write it down in your engineering notebook.

   Click Run This Study (green arrow in the toolbar, or right-click the study name > Run). The solver will take a few seconds to a minute depending on your computer.

   When it finishes, three result plots appear automatically. Record these values in your notebook:

   • Maximum Von Mises stress (in MPa)
   • Maximum displacement (in mm)
   • Minimum Factor of Safety
   Sanity check

   For a 50 N load on this bar with PLA properties, expect a max stress somewhere in the range of 15–50 MPa, a displacement under 1 mm, and a Factor of Safety above 1.0. If your numbers are wildly outside this range, double-check your material values, fixture placement, and load direction before continuing.

7. Optional: mesh refinement study

   FEA results depend on mesh quality. A coarse mesh gives fast but less accurate answers. A finer mesh takes longer but captures stress concentrations more precisely. How do you know when the mesh is fine enough? You run a convergence check.

   Go back to the Mesh folder and edit the mesh settings. Halve the element size (for example, if the default was 2 mm, set it to 1 mm). Re-run the study. Compare the new max Von Mises stress to the previous result.

   If the stress value changed by less than about 5%, the mesh has converged—making it finer will not meaningfully change the answer. If the change is larger than 5%, halve the element size again and rerun. Record all values in a table like this:

   Run	Element Size (mm)	Max Stress (MPa)	% Change
   1	(default)	—	—
   2	(default ÷ 2)	—	—
   3	(if needed)	—	—

   Why this matters

   In professional engineering, publishing simulation results without a convergence check is considered bad practice. If halving the mesh changes your answer by 20%, your original result was not trustworthy. This simple check builds a habit that separates careful engineering from guesswork.