Check stress and deflection (Simulation)

The Simulation workspace answers "will it bend or break under this load?" for the part you are modelling. It is a linear static study (small deflections, the material stays elastic) or a natural frequency study, solved on a mesh of quadratic tetrahedra that follows the part's faces (or, if you choose, of small equal cubes). It needs the exact kernel (see The exact kernel and the mesh kernel).

Choose Simulation in the Workspace box at the left of the toolbar. Your part is not changed; the study is saved inside the part file and every change to it can be undone.

Set up a study

1. Press New study in the right panel.
2. Choose the Material. The panel shows its stiffness (E), Poisson's ratio, density and yield strength. The values are typical handbook figures; your supplier's certified values may differ.
3. Choose the Mesh:
   • Tetrahedral (accurate), the default: 10-node tetrahedra whose outer faces lie on the part's faces, with curved edges on holes, fillets and other round faces. The nodes on flat, cylindrical, conical, spherical and toroidal faces, revolved and extruded faces and freeform (B-spline) faces sit on the exact surface; any other kind of face follows its display mesh, and the results table says how many faces did. The mesh is made finer by itself near curved faces, thin walls and sharp edges.
   • Voxel cubes (fast): the part filled with equal cubes. Quick, but curved faces become steps. Studies saved before the tetrahedral mesh existed keep this.
4. Leave Element size empty for an automatic size (about 12,000 tetrahedra, or 20,000 cubes), or type one in millimetres. The panel shows about how many elements that makes before the finer spots are added. With tetrahedra, Smaller elements on curved faces (on by default) refines holes and fillets, where stress usually peaks.

Refine automatically

With tetrahedra, a static study (without a thermal load) and a steady thermal study offer Refine automatically (adaptive). Tick it and set:

• Target error (%): solving stops when the estimated error is below it (1 % to start with).
• Most passes: the most solves it may run (5 to start with, at most 10).

Each pass solves, finds the elements with the largest estimated error, splits them (and as few neighbours as needed to keep the mesh whole), and solves again. New nodes on curved faces go onto the exact surface. The results then show a table and a chart with, for each pass, the elements, the unknowns, the estimated error and the peak stress (or temperature) and displacement (or heat flux), and a line saying why it stopped: the target was met, the passes ran out, the next mesh would be too big, or a pass failed (you then see the last good pass).

Read the estimate as an estimate. It (Zienkiewicz–Zhu, compared with exact answers it reads about 0.6 to 0.95 of the true error) measures the error over the whole part, so a peak stress at a hole or a fillet is usually still a little off when the estimate looks small: for a stress concentration, set the target under 1 % and watch the peak settle from pass to pass. At a sharp inside corner or the edge of a fixed face the true stress is infinite, so the estimate never gets there: the passes run out instead.

Hold it and load it

Every study needs at least one support and, for stress, one load.

1. Press Fixed in the toolbar. The new support is selected and waiting for faces: click the faces that are held still (click a face again to drop it). Press Done picking or EscEsc when finished. Blue cones mark the held faces.
2. Press Force and click the faces the force acts on. In the panel type the Total force in newtons and choose its Direction: into the face, or along an axis. The force is shared over the picked faces by area. Orange arrows show it.
3. Press Pressure for a pressure in MPa (N/mm²) pushing into the picked faces; a negative pressure pulls.

More kinds are in the panel's Add list: a Frictionless face (the face may slide along itself but not move away from it — use it for symmetry planes and smooth supports) and Gravity (the part's own weight, 9.81 m/s², in the direction you choose).

A support that leaves the part free to slide or spin is refused, saying which motion is left free.

Solve and read the results

Press Solve. The work runs in the background; Stop cancels it. Then:

• The part is coloured by von Mises stress; choose Displacement or Safety factor in Show. The legend gives the scale.
• Point at the part to read the values under the pointer.
• Tick Deformed shape to see the part bent (the motion is enlarged by the Scale; the real one is the table's).
• The table lists the largest stress and where it is, the largest displacement, the smallest safety factor (yield strength ÷ von Mises stress; below 1 the material yields), the applied load and the reactions at the supports (they balance the load), and the mesh used.

For natural frequencies, choose that Type, set how many Modes, and solve. Each mode shows its frequency and shape (shapes are scaled to 1 at their largest motion).

If you change the part, the results are marked out of date: solve again.

How far to trust it

PartCraft checks its solver against hand formulas (a cantilever's tip deflection PL³/3EI within 1 %, a bar's stretch PL/AE exactly, a cantilever's first frequency within 3 %, the stress around a hole in a plate). Still, keep these limits in mind:

• The mesh. With tetrahedra, PartCraft checks a cantilever's deflection and bending stress (within 0.3 %), the stress at a hole in a plate (Kt, within about 1 %), a thick tube under pressure (Lamé, within 0.3 %) and the first frequency (within 0.4 %). The table shows the mesh quality (the smallest and largest angles between element faces; below about 10° an element is poor) and an estimated stress error: if it is more than a few percent, solve again with a smaller element size, or let Refine automatically do it. On a plate with a hole and a bar with two edge notches, automatic refinement got within 1 % of the textbook Kt with about a sixth of the unknowns that making the whole mesh finer needed. With voxel cubes, a hole or a fillet is a staircase at the cube size, so stress there is rough.
• Sharp inside corners and the edges of fixed faces have no true peak stress. The value there keeps growing as the elements get smaller. Read stresses a little away from such places, or round the corner in the model.
• Results to read. Besides von Mises stress, displacement and safety factor, a tetrahedral study shows the maximum and minimum principal stress (tension and compression) and the equivalent strain. Tick Show mesh to see the elements.
• Linear and elastic only. No yielding, contact between parts, large deflections or fatigue. Heat, thermal stress and linear buckling are their own study types: see Heat, thermal stress and buckling.
• Every material is the same in all directions. 3D-printed plastics are weaker across their layers, often by a third or more.
• This is a lab build: check parts that matter another way.

Related

• Heat, thermal stress and buckling
• Grow a shape from loads (Generative)
• Measure distances, angles and mass
• What is not built yet