TMCoreShape Documentation
Everything you need to go from an empty viewport to an exported part — every tool, what it does, and how the pieces fit together.
Getting Started
CoreShape is a parametric, sketch-to-solid CAD editor that runs entirely in your browser. There's nothing to install — click Open Dashboard and you're modeling.
The basic workflow is the same one every CAD tool uses:
- Sketch a 2D profile on a plane or an existing face.
- Extrude or Revolve that profile into a 3D solid.
- Modify the solid — round edges with Fillet, bevel them with Chamfer, hollow it out with Shell, or combine it with other bodies.
- Export to STL, OBJ, STEP, 3MF or AMF when you're ready to 3D print, render, or hand the model to another CAD tool.
Every one of those steps becomes an entry in the Timeline at the bottom of the screen, so you can go back and change any step later and the rest of the model rebuilds around it.
Interface Overview
- Top bar — the CoreShape logo (click to return to the home page), the File, Preferences, and Export menus, your document's title centered in the bar (double-click it to rename), and your account profile on the right.
- Sketch + Create toolbar — directly under the top bar. Shows the Sketch tools, and once you're not sketching, the Create, Modify, Construction Plane, and Inspect tool groups, then AI (CoreShape AI) and Simulation & Test (3D Printability and the Part Simulator) at the far end.
- Viewport — the 3D scene in the center. The ViewCube in the top-right corner lets you snap to a standard view; Fit, Grid, and Wire buttons sit just below it.
- Browser panel (top-right) — a tree of every sketch and body in your document. Solids are listed as Body 1, Body 2 and so on; right-click one to give it a name of your own, which then sticks no matter how you edit it later. (The Timeline along the bottom names each step instead — Extrude1, Fillet2 — because that's a record of what you did, not of what you have.) Click an entry to select it; double-click a sketch to re-edit it; right-click either one to rename or delete it. Every sketch and body has its own eye icon to show or hide it in the viewport without affecting the model itself.
- Properties panel (bottom-right) — details about whatever is currently selected.
- Timeline (bottom of the window) — every feature in your document's history, left to right, in the order it was created.
- Status bar — bottom-left of the viewport; shows the active tool and contextual hints for what to do next.
Sketching
Click Create Sketch (or press S), then click one of the three standard XYZ planes or a flat face on an existing body. The view snaps to look straight at that plane and the sketch toolbar unlocks.
Sketch tools
| Tool | Key | What it does |
|---|---|---|
| Line | L | Click to place points, connecting each to the last. |
| Rectangle | R | Click two opposite corners. |
| Circle | C | Click a center, then a point on the circle. |
| Polygon | G | Regular N-sided polygon; choose the side count when you pick the tool. |
| Arc ▾ | A | A dropdown with three ways to draw an arc: 3-Point (start, end, then a point it passes through), Center Point (center, then start/end), and Tangent (continues smoothly from the end of an existing line or arc). |
| Ellipse | E | Click a center, then a point to set the two radii. |
| Spline | N | Click a series of points; the curve fits smoothly through all of them. |
| Point | O | Places a single reference point — handy as a snap target or a Sweep/Revolve reference. |
| Text | T | Click to place, then type — turns lettering into real sketch geometry you can extrude. |
| Dimension | D | Click an entity (or two points) to add a persistent, editable length/radius label. Double-click any placed dimension later to change its value. Selecting a single line doesn't jump straight into editing — start typing a number to set its value, so a plain click can still just select it. |
| Construction | X | Click existing entities to toggle them to dashed, reference-only geometry — useful for alignment guides that shouldn't become part of the final solid. |
| Finish Sketch | F | Leaves sketch mode. You can also right-click and choose Close Sketch, or jump straight to Extrude/Revolve from that same right-click menu. |
Snapping
While drawing, your cursor snaps (in priority order) to: a grid point, an endpoint/vertex of an existing sketch entity, the center of an existing circle or arc, any other point along an existing entity's shape (including along a curve), a corner of the face you're sketching on, the center of that face (handy for starting a concentric circle on a cylinder's cap), and any point along that face's border. A line drawn on top of a face's edge always takes priority over the face's own edge underneath it, so it stays reachable to snap onto. Hold Alt while drawing to temporarily disable grid snapping for freehand placement.
Constraints
The CONSTRAIN toolbar appears while you're sketching. It works two ways — whichever order is more convenient: click a constraint first, then click the entities it applies to; or select entities first, then click the constraint to apply.
Modifying a sketch
The MODIFY toolbar appears once you're sketching, alongside Dimension:
| Tool | What it does |
|---|---|
| Trim | Click a line or arc where it overshoots another entity, and just that overshooting piece is deleted — works on curved entities as well as straight lines. |
| Fillet | Select two lines that share a corner to round that corner with a tangent arc, at a radius you set — a 2D version of the body-level Fillet, for cleaning up a sketch's own corners before you extrude it. |
| Move | Select entities, click Move, then drag or type an offset to reposition them. |
| Rotate | Select entities, click Rotate, then drag or type an angle to spin them around a center point. |
| Mirror | Select entities, click Mirror, then click a line to reflect the selection across it. |
| Linear Pattern | Select entities, set a direction, spacing, and count, and repeat them in a straight line. |
| Circular Pattern | Select entities, then either type a center point or click Pick Center Point and click one directly in the sketch — it snaps onto an existing entity's endpoint just like the draw tools do. Set a count and total angle to repeat the selection around that center. |
Editing an existing sketch
Double-click any sketch in the Browser panel to jump back into it. CoreShape automatically rolls the timeline back to that point while you edit, so you're working with exactly the geometry that existed at that step — finish the sketch again and the rest of your model rebuilds on top of your change.
Creating Solids
| Tool | Key | What it does |
|---|---|---|
| Extrude | E | Click one or more closed profile faces from a sketch, then drag the arrow handle or type an exact distance. Toggle Symmetric to extrude equally in both directions, or Cut to subtract the extrusion from an existing body instead of adding new material (dragging past the target body auto-checks Cut for you). |
| Revolve | V | Click a closed sketch profile (if the sketch has more than one, pick which one), then click a line in the sketch to use as the axis, and set the revolve angle. |
| Sweep | — | Drags a closed profile along a path. Click the path first — one or more connected lines/arcs, which can live in their own sketch on a different plane — then click the closed profile to sweep along it. The path segments must form one unbroken chain; a live preview shows the resulting solid before you commit. |
| Loft | — | Blends a solid through two or more closed profiles — a square base flowing up into a round top, say, which neither Extrude nor Revolve can do. Draw each profile in its own sketch on its own plane, then click them in order from one end of the shape to the other; the panel lists the sequence as you go, and clicking a picked profile again removes it. Each profile must be on a different plane. Tick Straight sides for flat, faceted transitions instead of the default smooth curve through every profile. |
| Shapes ▾ | — | Drop straight-in primitives without sketching first: Box, Cylinder, Sphere, Cone, Torus. |
Modifying Bodies
| Tool | What it does |
|---|---|
| Fillet | Click Fillet, then click the edges you want rounded (a body can be selected ahead of time, or your first edge click picks it) and set a radius. Works on any body shape — click any segment of a curved rim (like a cylinder's cap) and the whole curve is selected and rounded in one smooth pass, not just the segment you clicked. Only real corners are offered — a curved primitive's own seam and a flat face's edges are left out, since there's no actual corner there to round. If an edge can't be rounded on its own (a short edge meeting another at a sharp vertex), CoreShape automatically pulls in the connected edge it needs to blend the corner. |
| Chamfer | Same edge-picking as Fillet, but cuts a flat angled bevel instead of a round, at a distance you set. |
| Shell | Hollows a body out, leaving walls of the thickness you set. Click the faces you want left open — click a picked face again to close it, and pick several to open more than one. If there's only one body, its top face is selected for you, so a box becomes an open-top container without any picking. |
| Move / Rotate / Scale | M / Shift+R / Shift+S — click the tool, then pick a body (or pick it first), and an interactive 3D gizmo appears with a live numeric readout as you drag or type exact values. |
| Mirror | Pick a body, then choose which standard plane (XY/XZ/YZ) to mirror it across. |
| Union | Select exactly two bodies (in the order you want) and click Union to merge them into one solid with real CSG geometry — not just visual overlap. |
Inspecting
| Delete | Del — deletes whatever's currently selected (a body, a sketch, or a feature). |
Timeline & History
Every sketch, extrude, revolve, modify, and boolean operation appears as its own step in the Timeline at the bottom of the window, in creation order. Click any step to select the sketch or body it produced.
Ctrl+Z / Ctrl+Y undo and redo — including individual entities while you're mid-sketch, so you don't lose an entire sketch's progress from one misclick.
Testing Your Part
Two tools at the end of the toolbar, under SIMULATION & TEST, look at a finished body and tell you something about it. Both are Pro plan features, and both run entirely on your own machine — nothing about your model is uploaded to run either one.
3D Printability
Checks a body for the three things that most often ruin a print:
- Thin walls. Measures wall thickness across the body and flags anywhere too thin to print reliably at the nozzle size you set.
- Overhangs. Finds surfaces angled too far from vertical to hold themselves up, which are the parts that will need support material.
- Orientation. Compares how the part would print in six orientations — as modelled, upside down, and on each of its four side faces — so you can see which way up gives you the least trouble before you send it to a slicer.
The panel finishes with plain-language suggestions rather than raw numbers alone — which way to rotate the part, and what to thicken.
Part Simulator
Finite element analysis: hold part of a body still, push or press on another part of it, and see how far it moves and how hard the material is working. The panel walks through seven steps in order — Setup, Material, Constraints, Loads, Mesh, Simulate, Results.
| Step | What you do |
|---|---|
| Material | Pick from ten real materials — aluminium 6061-T6 and 7075-T6, A36 structural steel, 304 stainless, 4140 alloy steel, Ti-6Al-4V titanium, ABS, PLA, nylon 6/6, and polycarbonate. Each carries its own stiffness and yield strength, which is what makes the results mean anything. |
| Constraints | Click the faces that are held fixed — bolted down, clamped, welded. A part with nothing fixed has nothing to push against, so at least one is required. |
| Loads | Apply a force (in newtons, in a direction you choose) or a pressure (in kPa, spread over a face). |
| Mesh | Divides the solid into elements to solve over. A finer mesh is more accurate and slower; CoreShape picks a sensible size and warns you if the mesh is too coarse to represent the part's thinnest dimension. |
| Results | Displacement (how far each point moved), Von Mises stress (how hard the material is working), and factor of safety (yield strength divided by stress — below 1 means the material yields). Each is shown as a colour map on the part. |
One thing worth understanding, because it looks like a bug and isn't: stress at a sharp corner where the part is held fixed rises without limit as the mesh gets finer. That is a mathematical artefact called a singularity, not a real prediction — the true stress there is limited by the fillet that exists on any real part. CoreShape detects this and says so in the Results panel. When it does, read the displacement and the overall stress pattern, and disregard the single peak number.
CoreShape AI
The AI group in the toolbar opens the CoreShape AI Builder. Describe a part in plain English and it writes a modelling plan — an ordered list of the same sketches, extrudes, and modifications you would have done by hand — which you can read before anything is built. Run it and the steps land in your Timeline as ordinary features, so you can edit, delete, or build on any of them exactly as if you had made them yourself.
If the result isn't what you meant, Revise it: describe the change, and it plans again knowing what the previous attempt did.
- Pro plan only, and there's a daily allowance shown in the panel. The meter tells you what's left and when it resets, in your own local time.
- It is a starting point, not an oracle. It's at its best on parts that are describable in a sentence or two — a bracket with a given bolt pattern, a plate of a given size with holes in it. Complex, precisely-dimensioned work is still faster by hand.
- What gets sent. Your description, a snapshot of the design you're working on, and the list of operations available. Our Privacy Policy covers who processes it; your designs are not used to train models.
File, Export & Preferences
File
| New Document | Ctrl+N |
| Save | Ctrl+S — saves locally in this browser. Signed out, this is the only way your work is kept, so use it. |
Signed in, there's nothing to click: your document saves to your account automatically a couple of seconds after you stop editing, and shows up on your My Projects dashboard from any machine you sign in on. Open one from there to keep working on it — there's no separate in-app Load command. Rename a saved project right from the dashboard with the pencil icon on its card.
Export
Export your current model as STL to bring it into a slicer or another 3D tool. The Standard plan adds OBJ, and a true STEP file — an exact B-rep export straight from the underlying solid geometry, not a tessellated approximation, so a cylinder or fillet reopens in another CAD tool as a real curved surface rather than a faceted mesh.
Pro adds two richer 3D-printing formats. 3MF is the modern replacement for STL — the same mesh, but a compact zipped package that carries units and model metadata. AMF (ISO/ASTM 52915) is the open standard for the same job, written as plain XML with units declared in the file; reach for it when a slicer or a workflow asks for AMF specifically. Both export every visible body as its own object, welded so slicers accept the mesh as manifold.
Tools your plan doesn't include are marked with a small blue dot in the toolbar. Click the dot (or the tool) to see what it unlocks. Standard adds Sweep, Loft, Shell, the construction planes under More, the Center Point Arc, Tangent Arc and Spline sketch tools, and the OBJ and STEP exports above. Pro adds CoreShape AI, the Part Simulator, and the 3D Printability check. See Your Account & Plans.
Preferences
- Units — mm, cm, in, or ft. Changes how every length is displayed and typed throughout the app.
- Theme — Dark or Light.
- Keyboard & Mouse — remap any of the single-key tool shortcuts (see below) to whatever's comfortable for you.
Your Account & Plans
An account is required to open the editor. Signing up is free and takes a minute — see the Plans page for what each tier includes.
Signing in and staying signed in
- New accounts verify their email address with a one-time code before the first sign-in. Forgotten passwords are reset the same way, from the sign-in page.
- You are signed out automatically after 24 hours without using CoreShape. The clock resets every time you do anything that reaches our servers, so working normally never signs you out mid-session — it's there so a session left open on a shared or borrowed computer doesn't stay open indefinitely. A session also ends 30 days after you sign in, whichever comes first.
- Changing your password signs out every other device immediately. If you think someone else has reached your account, that is the fastest thing you can do — then email us.
- From account settings you can change your name, change your password, switch plans, cancel a free trial, and permanently delete your account and its projects.
What each plan includes
| Plan | What it adds |
|---|---|
| Free | The full sketching and solid-modelling toolset covered above, STL export, unlimited saved cloud projects, and up to 10 of them editable at a time. Not a trial and not time-limited — commercial use is allowed, so you can sell what you make. |
| Standard | Unlimited editable projects, OBJ and STEP export, Sweep, Loft, Shell, the full set of construction planes, and the Center Point Arc, Tangent Arc and Spline sketch tools. |
| Pro | Everything in Standard, plus CoreShape AI, the Part Simulator, and the 3D Printability check. |
Standard and Pro both start with a 7-day free trial. A trial becomes a paid subscription automatically when the week is up unless you cancel first — cancelling keeps the features for the rest of the trial rather than ending them the moment you click. Current prices are on the Plans page, and the details are in Terms §4.
Projects on the Free plan
Free accounts can save an unlimited number of cloud projects, but only 10 stay editable at a time. Creating a new one past that limit doesn't delete anything — your oldest editable project automatically becomes read-only, so it's still there to open, export, and read. Deleting a project, or upgrading, makes a read-only one editable again. Nothing you made is ever taken away from you.
Keyboard Shortcuts
These are the defaults — every shortcut in the first table is remappable from Preferences → Keyboard & Mouse.
| Action | Default key |
|---|---|
| Create Sketch | S |
| Extrude | E |
| Revolve | V |
| Move | M |
| Line (while sketching) | L |
| Rectangle (while sketching) | R |
| Circle (while sketching) | C |
| Polygon (while sketching) | G |
| 3-Point Arc (while sketching) | A |
| Ellipse (while sketching) | E |
| Spline (while sketching) | N |
| Point (while sketching) | O |
| Text (while sketching) | T |
| Dimension (while sketching) | D |
| Construction Geometry (while sketching) | X |
| Finish Sketch (while sketching) | F |
Fixed, non-remappable shortcuts (standard conventions):
| Undo | Ctrl+Z |
| Redo | Ctrl+Y |
| New Document | Ctrl+N |
| Save | Ctrl+S |
| Delete selection | Del |
| Rotate | Shift+R |
| Scale | Shift+S |
How to CAD — tips if you're new to this
The tools above are simple individually; the skill in CAD is mostly about order of operations and habits that keep a model editable. A few that apply everywhere, not just in CoreShape:
- Sketch on the right plane first. Think about which direction the part actually needs to grow before you draw — it's much easier to pick the correct plane up front than to fix it after extruding.
- Rough shape first, details last. Get the basic solid extruded/revolved before you add fillets, chamfers, or shells. Adding a fillet early and then editing the sketch underneath it is one of the most common ways to break a model in any CAD tool.
- Use dimensions to make sketches exact. A sketch that "looks about right" will bite you later. Add a Dimension to anything that needs to be a specific size.
- Use Construction geometry for guides. If you need a reference line or point just to align other geometry, mark it as Construction so it doesn't accidentally become part of your extruded profile.
- Cut, don't rebuild. If you need to remove material from an existing body, sketch the shape to remove and use Extrude's Cut option instead of modeling a separate body and subtracting it later — it keeps the timeline shorter and easier to follow.
- Name things. Double-click a sketch or feature's name where available so your Timeline reads like a list of steps, not a wall of "Extrude 4".
- Lean on the Timeline. If something looks wrong, click backward through the Timeline to find the step where it broke, rather than undoing blindly.
- Save often. Ctrl+S is cheap insurance — your document persists locally, but a named save is easy to come back to on purpose.