Whet pixel markWhet

Whet user guide, chapter 4, 2026-10-09

Strength and Heat

Whet checks a part two ways. A Strength study asks how much the part deforms and how hard its material is stressed under a load. A Thermal study asks how hot each place gets when heat goes in and out. Both follow the same path: choose a material, mark faces, make a mesh, solve, read the result.

The meshing and the solving run on your computer. They are done by the open engines gmsh and CalculiX. The window sets them up and shows you what came back.

Open a study

Open the part first. Then choose Analysis > Strength for a stress study or Analysis > Thermal for a heat study. The window switches to that workspace and shows a panel with the study's rows. The same rows are reached from the command row: SETUP, LOADS, SUPPORTS, SOLVE, RESULTS and REPORT in Strength; SETUP, LOADS, SOLVE and REPORT in Thermal.

Under Analysis, the Strength Study and Thermal Study submenus bring one row of the panel to the front.

At the bottom of each panel is a list called Steps. It shows what is still needed, in order, and each line reads needed, optional, running or done. Read it first when the Solve button is grey. The line that says needed is the one to fix.

Put a condition on a face

A condition belongs on a face of the part. The quickest way is to click the face in the viewport and then press the matching tool in the LOADS or SUPPORTS panel. The tool writes that exact face into the panel. You do not type a face name.

If no face is picked, the tool is grey and its tooltip says why. After a result is on the part, the RESULTS panel takes over. Choose Analysis > Results > Clear Results to get the condition tools back. Picking a new face does this on its own.

To check which face you picked, look at the Faces row in the panel. It warns you before the run when the fixed face and the loaded face touch.

You can also pick the face in the panel's own list. The list names the sides of the part, and the face you picked in the viewport is offered first.

Strength conditions

These are the names used in the window.

NameWhat it meansWhere you set it
Fixed SupportThe face is held in place, as if bolted or clamped.Strip and Analysis > Fixed Support
ForceA push in newtons on a face, with x, y and z parts.Strip and Analysis > Force
PressureA push spread over a face, in MPa, positive into the material.Strip and Analysis > Pressure
MomentA turning load, in N mm, applied through a point.Force Through a Point row

Fixed Support holds all three directions by default. The Constrained axes row lets you hold fewer, so a face can act as a pin. The Selection tolerance, mm row sets how far from the face a mesh node may be and still count as on it. Too small a value catches nothing. Too large a value holds a slab.

Force and Pressure share the Load face row. Choose the Load kind to switch between them. A force is a total. A pressure is per area, so the total is the pressure times the face area.

Force Through a Point puts a force and a moment on one reference point, and the point drives the face you chose. Use it when you need a turning load.

Load Cases asks for more than one load on the same mesh. Peak stress over several cases is reported as an envelope, and no single load produces it.

Own Weight adds gravity with a direction. It needs a density in the material.

Strength material

Choose a material in the Card list. A card carries Young's modulus, Poisson's ratio, yield strength and density when they are known. If you choose Typed values instead, you type them yourself: Young's modulus, MPa, Poisson's ratio, Yield, MPa and Density, kg/m3.

A factor of safety needs a yield strength. If the card does not state one, the window shows a dash and tells you so. It does not guess. Many generic cards, steel and aluminium among them, carry no yield. Type the yield from your own supplier.

The panel starts with a default material. The Steps list keeps that step marked needed until you choose a material yourself.

Thermal conditions

Thermal conditions live under Thermal Loads and Thermal Boundary Conditions in the panel. The LOADS panel holds Temperature, Convection, Heat Flow, Heat Flux and Radiation, and each is also under Analysis.

NameUnitWhat it does
TemperatureCHolds a face at a set temperature.
ConvectionW/m2/KA face loses or gains heat to the air or liquid around it. You set the Heat Transfer Coefficient and the Ambient Temperature, C.
Heat FlowWA total power put into a face, shared evenly over it.
Heat FluxW/m2Power per area, positive into the part.
RadiationemissivityA face exchanges heat with its surroundings by radiation. You set Emissivity and the surrounding temperature.

The panel gives guidance for the heat transfer coefficient: still air is about 5, and boiling water reaches 100000.

Every thermal study needs at least one Temperature or Convection boundary. Without one the part has nowhere to send its heat and the result would only be arithmetic, so the window refuses. The panel offers a First boundary and a Second boundary, and the second can be None.

A material per body. When the part has more than one body, the Material section lists each body with its material. Pick a body in the Body list, under Bodies in the Model Tree, or by clicking it in the viewport, then choose its card in Material. Solve Heat waits until every body has one. The study file names each body by a point inside it, which the window finds from the body's own faces. The Strength panel has the same Body row under Card. Assist does the same when you name the body, for example "make Solid2 copper", and its study steps, applied in the window, fill these panels and solve there.

Do not put a Heat Flow on a face that is also held at a fixed Temperature. A held temperature discards the heat on it. The Faces row warns you.

A peak that sits on a Heat Flow face or on a held face has no converged value. Mesh it finer and it keeps climbing. Read the temperature a little away from such a face.

Heat over time

Switch on Transient under Over Time to see how a part warms up. You set the length in Seconds, the Step, s, and the Initial Temperature, C. The result is a set of instants, each with its peak and mean temperature.

A transient study cannot be combined with a Thermal Stress step yet.

Thermal stress

Switch on Thermal Stress to ask what the heat does to the part. You add a Fixed Support, set Stress free at, C (the temperature at which the part carries no stress), and the material needs an Expansion, 1/K. Fixing a whole face against growth creates a stress concentration of its own. The result marks it.

Mesh before Solve

Every study needs a mesh. Under Mesh you set the Element size, mm and the Element order. The window offers a size from the part: a fifteenth of the longest side, and no more than half of the shortest. Type a number to change it. Hover the box to see the reason.

Pressing Mesh makes the mesh and shows it. This step is optional. If you press Solve Stress or Solve Heat without it, the window meshes for you first.

The Mesh line in Steps tells you where you are:

  • not generated: the size is set and no mesh exists. Press Mesh to look at it, or Solve to make it and solve.
  • done: a mesh exists and Solve will use it.
  • stale: the mesh drawn was made with other settings. Press Mesh again, or press Solve and it meshes anew.

Finer elements give a better answer and cost more time. Order 2 elements bend better than order 1 for the same size.

Solve

Press Solve Stress or Solve Heat. You can also use Analysis > Solve Strength Study or Solve Thermal Study. The line for Solve in Steps reads running while the engine works. Stop ends the run.

Time limit, s sets how long the window waits. The default is 900 seconds. The engines also have their own fixed limit of 300 seconds per mesh and per solve, and you cannot move that one.

The Cost section shows how many solves the run needs and what files the run writes. Check it before you start a convergence series.

Name sets the name the study's files carry. They are written beside the part.

If the window shows Run Locally after a refusal, the refusal came from a server you set up in Your own server. Run Locally runs the same study on this computer.

Read a strength result

When a study finishes, the result opens on the part as a colour field, with a legend. The Result panel lists the figures. Open it with Analysis > Results > Result Panel.

Peak von Mises, element. This is the highest stress the solver printed. It is read at a point inside an element, so it is the number to compare with yield.

Peak, nodal average. This is the largest value in the coloured field. The solver's element values are carried to the mesh nodes and averaged where elements meet. So the nodal number differs from the element number; it is usually lower, and at a corner it can be higher. The legend's top is the nodal figure. That is why the legend top does not match the peak in the panel. Neither number is wrong. They are two different readings.

Factor of safety. This is yield divided by the element peak, never the nodal average. It shows a dash when the material states no yield. With more than one material, each material has its own.

Peak displacement. This is the largest movement of any node, in mm. The viewport can show the shape with Analysis > Results > Deformation. The choices are Auto, Actual, x10, x100 and Show Undeformed. The exaggeration is a display setting only.

Probe reads the value at a point you click. Minimum and Maximum marks the lowest and highest values on the part.

A study with no load at all, such as a natural-frequency study, has no stress or deflection. The panel says nothing pushes the part and shows the frequencies instead.

Examples you can check

Type the same sizes and the answers should land close to these.

  • A bar clamped at one end with a load at the other end: the tip deflection came out 1.09 percent from the Timoshenko beam formula at 4 mm elements.
  • A thin steel tube, 20 mm bore, 2 mm wall, with 1.5 MPa inside and open ends: the peak von Mises came out 16.25 MPa against the Lame value of 16.59 MPa.

These show the engines are set up correctly. They do not prove that your own part is right.

Mesh convergence

One mesh gives one answer, and the answer depends on the mesh. The window says so. A one-mesh study carries a note that reads "one mesh" and says convergence was not checked, because nothing finer was solved.

Switch on Mesh convergence to solve several meshes. You set how many meshes (two to six) and how much finer each one is. You also set Settle (%) and a time budget in seconds.

An observed order of convergence needs at least three meshes at a constant ratio. The element size you typed is the coarsest.

The result tells you for each figure whether it settled. Read these notes with care.

  • Settled means the largest relative move at the last refinement was inside your Settle percentage. It does not mean the number is right. It means it stopped moving.
  • Growing means it kept changing as the mesh got finer.
  • Singular, no converged value means the peak sits at a sharp inside corner, a point load, or a point support. It will keep growing as you refine. No factor of safety taken from it can be trusted either, and the window says so.

If the budget runs out, the meshes that did solve are kept.

Other strength studies

These are under Also Solved, Fatigue, Past Yield and Closed Form in the Strength panel.

Natural Frequencies. You ask for a number of modes. The material needs a density. The answer is a list of frequencies in Hz.

Buckling. You ask for a number of modes. Each mode gives a load factor and a critical load. A pressure cannot be combined with buckling.

Harmonic Sweep. Needs natural frequencies first. You give a range in Hz, a Damping ratio and a Sweep force, N. The damping ratio is a number you type. The engine has no measured damping for any material. The response at resonance depends mostly on that number. The sweep only answers at the frequencies you name.

Fatigue Life. Gives a life for one stated cycle, using the Goodman and Gerber corrections and a Basquin line through two points you type. It needs an ultimate tensile strength and an endurance limit or two points of an S-N curve. It ignores surface finish, size, notches and temperature effects.

Plasticity. Solves past yield with a hardening curve you type. A factor of safety taken from a plastic peak is bounded and approaches one.

Pressure Vessel. Compares the study's peak with the thin-wall and Lame formulas for a long cylinder. The ratio tells you whether your mesh and supports reproduce the textbook answer. It is not a design-code check.

Contact. Two bodies pressed together can be solved with contact, with or without friction. Two 20 by 20 by 10 mm steel blocks under 10 MPa gave a peak contact pressure within 0.9 percent of that figure. The Strength panel has no row for contact today (to be checked).

Materials

Analysis > Materials opens the shelf of material cards. Each card lists the properties it states and what is missing. A card with no density gives no mass and no natural frequency. A card with no yield gives no factor of safety. You can add a card of your own. A shipped card is copied before you change it.

Clear Results

A result stays on the part until you remove it. Analysis > Results > Clear Results takes it off and brings the condition tools back.

Limits

  • Every mesh is made of tetrahedra. There are no shell or beam elements. A thin sheet part is studied through its thickness with solid elements, and that needs many elements.
  • There is no local refinement at a fillet. The mesh size is global.
  • A bearing load through a hole is not available.
  • A pressure cannot be combined with buckling, a harmonic sweep or plasticity.
  • No transient structural dynamics, no creep, no hyperelastic materials, no ties, no springs.
  • A thermal study takes no mechanical load, and a transient thermal study cannot drive a stress step.
  • Without a licence a study is limited to 5,000 mesh nodes. See Licence, trial and updates. A licensed copy has no node limit and is bounded by your computer.
  • The coloured field is an average. Check the element peak before you decide.
  • A good-looking colour map is not a design check. Whet gives you numbers and their caveats. It does not apply a design code.

More limits are listed in Known limits.