A SOLIDWORKS-style workflow for FreeCAD. Free and open source.
Highlights ·
Feature guide ·
Install ·
Quick start ·
Good to know ·
Contributing
MechFlow is a FreeCAD workbench for mechanical engineers who know SOLIDWORKS and don't want to relearn everything to use free software. It sits on top of FreeCAD 1.1: you keep FreeCAD's geometry kernel, solver and open file format, and get the CommandManager, tool names, dialogs and day-to-day workflow you already use, from the first sketch to the supplier pack.
Motion Study, new in 0.31: keyframe a model's parameters and the camera, then export the video.
|
🧊 Part modelling |
✏️ Sketching |
🏗️ Weldments |
|
📐 Drawings |
🔩 Assemblies & Toolbox |
🛢️ Routing |
|
🪛 Sheet metal |
📊 Stress Check |
🎬 Motion Study & Render |
| SOLIDWORKS | MechFlow |
|---|---|
| CommandManager tabs | Features · Sketch · Weldments · Sheet Metal · Evaluate · Drawing · Assembly · Routing |
| Extruded / Revolved / Swept / Lofted Boss/Base and Cut | Same names, same options (end conditions, Direction 2, draft, thin feature) |
| Hole Wizard, Fillet, Chamfer, Shell, Draft, patterns, Mirror | Same names |
| Configurations and Design Table | Configurations with a Design Table |
| Weldments, Structural Member, Cut List | Same names |
| Mates, Toolbox, Smart Fasteners, Exploded View | Same names |
| Routing (Tube and Pipe) | Routing tab: Draw Pipe, Route Pipe, Valves & Instruments, Pipe Specs |
| SimulationXpress | Stress Check |
| Motion Study (Animation) | Motion Study |
| PhotoView 360 / Visualize | Render (studio) |
| Pack and Go for suppliers | Supplier Pack |
Every tool has its own panel, and you edit a feature again by double-clicking it. Click a heading to expand it.
Interface: CommandManager, heads-up view bar, SOLIDWORKS names
- CommandManager with Features, Sketch, Weldments, Sheet Metal, Evaluate, Drawing, Assembly and Routing tabs. It switches tab to match what you're doing (sketching, a drawing, an assembly).
- SOLIDWORKS names throughout: Extruded Boss/Base, Convert Entities, Smart Dimension, Mate, and so on.
- Floating heads-up view bar (you can drag it), Normal To (Ctrl+8), S-key shortcut bar, confirmation corner in sketches, light theme.
- Front/Top/Right planes you can hover, click and right-click → Sketch.
- Optional MechFlow splash screen (MechFlow → Use MechFlow Splash
Screen). FreeCAD reads its splash from a small
branding.xmlnext to the FreeCAD program, so on Windows this asks once for administrator permission. Updating FreeCAD removes the file; MechFlow then offers to put it back.
Part modelling: features, Hole Wizard, nozzles, patterns, configurations
- Extruded Boss/Base and Cut: end conditions, Direction 2, draft, Thin Feature, and a drag arrow with a depth box in the 3D view.
- Revolved Boss/Cut, Swept and Lofted Boss/Cut.
- Fillet and Chamfer on many edges at once, Shell, Draft.
- Hole Wizard: ISO M3–M20 simple, counterbore, countersink and tapped holes; ISO 273 close / normal / loose clearance; Blind, Up To Next (through the first wall only, for tanks and hollow parts) or Through All.
- Nozzle: click a tank or vessel wall, flat or curved, and pick the pipe (EN 10220 or ASME B36.10M) and its standout. The stub is shaped to meet the shell, only the wall it sits on is bored, and a weld neck or plate flange can go straight on the end. Position it exactly by typing X, Y, Z; point it square to the face or along an axis.
- Linear Pattern (with a spacing drag arrow), Circular Pattern, Mirror.
- Reference Plane (offset, at angle, mid plane, through a point, 3 points, normal to curve, tangent) with drag handles, and Axis.
- Rollback, Suppress/Unsuppress, Section View (up to three sections with a drag handle, on parts and whole assemblies), Edit Material and Mass Properties (a body, a weldment part or a whole assembly).
- Configurations with a Design Table: one part file, several versions of it. Columns are named sketch dimensions, feature values (depths, wall thickness, hole depths, member sizes) or a feature's suppression; rows are configurations. Double-click one to rebuild the part to it; Save model values writes your edits back into the table.
Sketching: definition colours, Relations panel, sketch patterns
- Under-defined geometry blue, fully defined black, over-defined red. The status bar shows Under Defined (n DOF) / Fully Defined / Over Defined.
- Relations panel: select entities and add the relations that fit them (Coincident, Horizontal, Midpoint, Tangent, Concentric, Collinear, ...). Display/Delete Relations lists the existing ones.
- Smart Dimension snaps to model edges without a Convert Entities step.
- Linear and Circular Sketch Pattern panels. Linear: Direction 1 and 2 (angle or a picked line, spacing, instances, reverse) for rows and grids. Circular: centre (origin or a picked point), angle, instances, equal spacing, reverse. Both preview live, and the result is constrained so it follows the original.
- The Sketch tab has the full set: Centre Rectangle, 3 Point Arc, Sketch Chamfer, Extend/Split, Move/Copy/Scale, Repair Sketch.
Weldments: structural members, trim/extend, end caps, gussets, cut list
- Structural Member: pick sketch lines (from one sketch or several, so 3D frames work) and a section: UKB, UKC, PFC, equal angle, SHS / RHS (hot finished EN 10210 or cold formed EN 10219) or CHS, in UK sizes. Corners are cut with End miter, End butt 1 or End butt 2; a member that ends on the side of another (a cross rail, a post) is cut square to its face. Rotate or mirror the profile; double-click to edit.
- Trim/Extend: trim or extend one member group's free ends to other members (cut square to the face) or to any body (cut to its shape).
- End Cap on tube ends (outward or inward, inset), or a bigger base plate with an anchor hole in each corner, and Gusset plates between two member faces (legs, thickness, corner relief).
- A weldment part stays one part: members, plates and gussets go into a Part container with the body (named after the file), so Insert Components brings the whole thing into an assembly.
- Cut List: members grouped by section and length, with the cut angles, plus end caps and gussets, saved as a spreadsheet.
Sheet metal: flanges, bends, flat pattern to DXF
- A Sheet Metal tab with SOLIDWORKS names: Base Flange/Tab, Convert to Sheet Metal, Edge Flange, Sketched Bend, Hem, Extend Tab, Extruded Cut, Corner and Bend Relief, Rip, Insert Bends, Forming Tool.
- Flatten shows the flat pattern (click again to fold back) and Save Flat as DXF writes it for the laser.
- Uses the free SheetMetal Workbench (Addon Manager); MechFlow offers to install it the first time.
Drawings: automatic drawings, title blocks, client sheets, Supplier Pack
- Make Drawing from Part: pick a sheet (ISO A4–A0, ANSI A–D) and get a standard 3 view plus an isometric, at a standard scale that fits the sheet clear of the title block, with overall dimensions, an "n x ⌀" callout and a position for each size of hole, and the weldment cut list as a table. Projection is first-angle for ISO sheets and third-angle for ANSI.
- Make Drawing from Assembly (same button, with an assembly open): an isometric with the BOM table and a numbered balloon on every BOM item, plus a dimensioned sheet for each part ("Auto" picks a bigger sheet only when it allows a bigger scale). Save All as PDF writes every sheet, numbered, into one folder. On big assemblies, bolts, nuts and washers are left out of the view by default (FreeCAD's drawing views slow down sharply with hundreds of fasteners); they stay in the BOM.
- Supplier Pack (Assembly and Drawing tabs): everything a fabricator
needs from one button, in a folder and a zip:
- the assembly sheet, and an exploded view sheet with balloons;
- a dimensioned sheet per part (PDF);
- STEP of the assembly and of each part;
- DXF flat profiles for plasma or laser cutting: every flat plate, each wall of a plate-built part such as a tank, and sheet metal flat patterns. Identical profiles (even turned over) are counted together, and the file names give thickness and quantity;
- the BOM and weldment cut list as CSV, and a contents list.
- The title block fills in from the part: name, material, scale, author, date, sheet, and weight on ANSI sheets. Text too long for its box is made smaller to fit (also when you type straight into the drawing).
- Title Block (Drawing tab, or right-click the sheet): every box in a list. Type in it, pick its font and size, bold, nudge it right or up. Move to sheet makes a box's text a note you can drag anywhere and restyle; Put back in box returns it.
- Text Box: type a note, pick the font, size (capital height in mm), bold / italic, colour and a wrap width; drag it into place. Double-click a note to change it; Ctrl + mouse wheel over a selected note makes it bigger or smaller.
- Projected views drag apart: the views are laid out once, then let go, so you can drag the top view up or down and the side view left or right. Each slides along its line from the front view, so they stay aligned (drag the front view to move them all). View Spacing sets the gap between them all at once. Break Alignment (right-click a view) frees it to go anywhere, its dimensions going with it, and Default Alignment puts it back in line.
- Client Sheet: bring in a client's border and title block as DXF (lines, polylines, arcs, circles, ellipses, splines, text, MTEXT and blocks; block attributes become boxes to type in), SVG, or a picture (PNG / JPG; PDF where FreeCAD's Qt can read it). Keep it the size it was drawn or fit it to a standard sheet, tick any text you want to type over, and it's kept in your sheet formats so Make Drawing lists it.
- Right-click on the drawing gives the choices for what's under the mouse (Break / Default Alignment, View Spacing, Edit Text) and Add Text Box Here, Title Block and Client Sheet, above FreeCAD's own.
- The Drawing tab has Model / Projected / Section / Detail views, View Spacing, Break / Default Alignment, Smart Dimension, Text Box, Note, Balloon, Centre Mark, Hatch, Surface Finish, Weld, Sheet Format, Title Block, Client Sheet, Scan View and Save as PDF / DXF.
Assemblies: mates, BOM, Exploded View, Interference Detection
- New Assembly and Insert Components.
- Mate panel: click a face, edge or point on two parts and MechFlow suggests the mate (Concentric, Coincident, Tangent). Other mates: Parallel, Perpendicular, Lock, Distance, Angle, Hinge, Slider. Aligned / Anti-Aligned flips the part. Mates show in a Mates folder with SOLIDWORKS names.
- Bill of Materials with ITEM NO. / PART NUMBER / DESCRIPTION / QTY., counting identical parts and fasteners together.
- Interference Detection: touching parts aren't counted, and results are remembered so re-checking after an edit is quick.
- Exploded View: the biggest part stays put and every other one slides out along the axis it sits on (a nozzle's gasket, flanges and pipe spread out along the nozzle, a door comes off its side), bolts going with what they hold. Click again to put it back; the assembly and its mates aren't changed.
Toolbox and Smart Fasteners: flanges, pipe, fittings, bearings, fasteners
Standard parts, browsed by category and standard:
- Flanges: EN 1092-1 Type 11 weld neck, Type 01 plate and Type 05 blind (PN16, PN25, PN40, DN10–DN600); ASME B16.5 weld neck, slip-on and blind, RF (Class 150 and 300, NPS ½–12).
- Pipe: EN 10220 (ISO 4200 sizes) and ASME B36.10M (Sch 10/40/80), any length.
- Pipe fittings: EN 10253-2 90° elbows (2D, 3D, 5D), 45° 3D elbows, equal tees, concentric reducers and caps, with the EN 10220 pipe wall; ASME B16.9 90° and 45° long radius elbows, equal tees, concentric reducers and caps. Outlet points turns an elbow or tee's branch up, down, left, right, front or back as it's placed.
- Bearings: ISO 15 deep groove ball bearings, 60xx, 62xx and 63xx.
- Click a pipe end and a flange or fitting sizes itself to the pipe; click a shaft end or housing bore for a bearing. Change size or rating later in the properties.
- Flange joints: click a flange's face (also one inside an inserted part, like a tank's nozzle flange) to bolt another flange or a blind to it. It turns to face it, with a gasket (EN 1514-1 IBC / ASME B16.21) and the bolts and nuts from the flange table.
- Fasteners: ISO, DIN, EN and ASME screws, nuts, washers, pins and more. Click hole edges (or a face, for all its holes) and each one sizes itself to its hole: a 9 mm clearance hole gets M8, a 5 mm tapped hole gets M6. Heads sit on the counterbore floor or in the countersink, the length is picked from the hole depth, and you can add a washer under the head and a washer and nut on the far side.
- Parts are named by standard (ISO 4762 M8x25<1>, EN 1092-1/11/B1/DN50/PN16<1>), move with the part they're on, and work in parts and assemblies.
Smart Fasteners: one click fills every empty clearance and tapped hole with the right screw, including holes that line up through several parts. Into a tapped hole it engages up to 1.5 × d; right through, it adds a washer and nut. Counterbores get socket head cap screws and countersinks get countersunk screws; change the type per group before OK.
Routing: Draw Pipe, Route Pipe, valves, pipe specs, size changes
- Draw Pipe: the quickest way in. Pick the pipe spec and size, then draw:
the real pipe, elbows, tees and flanges appear as each line goes in, and a
leg too short for its elbows is flagged straight away.
- Click a flange (a nozzle's, or the open end of any route) to start or finish on it: the pipe bolts to it (gasket, mating flange, bolts) and takes its size.
- Finish on another route's pipe and a tee goes in there; click part way along a pipe to branch off it.
- Route to... (R): click where the pipe has to go (a flange, a pipe or a point) and MechFlow offers the square ways round. Tab for the next, click to take it.
- Exact lengths: type a number (or Tab) in the length box by the corner you're drawing from and press Enter. Move Pipe (M) drags a straight across (the pipes either side stretch) or sets its length. P changes the drawing plane.
- OK builds the route. Select a route and click Draw Pipe to change it the same way.
- 3D Sketch: draw a pipe run straight in 3D space. Start on a nozzle flange, then click along; lines lock to X, Y or Z and round to 10 mm, Tab changes the plane, or type a direction and length. Edit any line in the table and the lines after it follow. Click a corner to start a branch. To change a route's lines, select any of its pipes or fittings and click 3D Sketch: the pipe goes see-through while you edit, and it rebuilds when you press OK.
- Route Pipe: select the 3D Sketch (or ordinary sketches) and MechFlow fills it in: pipe cut to length, elbows at the bends (EN 10253 2D/3D/5D or ASME LR; cut elbows for other angles), equal tees at branches, a gasket, mating flange and bolts where it starts on a flange, and plain ends, weld neck flanges, blinds or caps at the free ends. Edit the sketch and the route rebuilds.
- Valves & Instruments: click a pipe to drop a ball, gate, globe, check or butterfly valve (EN 558 / ASME B16.10 face-to-face), a pressure gauge or a temperature sensor on it. The pipe splits round it and flanges, gaskets and bolts go in. Drag the ring to turn it round the pipe (5° steps), drag the arrow to slide it along, or type both. They stay put when the route rebuilds.
- Pipe Specs: pick a spec (EN carbon steel PN16, ASME CS Class 150 Sch 40, stainless...) and the route takes its standard, material, schedule, elbows, flange rating and free ends. Duplicate a built-in spec to make your own; change it and every route using it follows. The material goes on the parts and in the BOM.
- Change Pipe Size: right-click a pipe of a route. The new size runs on downstream until the next change, with concentric reducers where it steps. Valves and fittings after it take the new size, and a library part with different end sizes (a DN100 × DN80 control valve, say) changes the size after it.
- Author Component: open your own valve, strainer or sensor model, click its port edges (two for an inline part, one for a branch part, three for a tee or Y piece), name it and OK. It joins the Valves & Instruments list and places, turns and bolts up like the built-in ones.
- Save Part As (Routing tab, or right-click a pipe or fitting): save one or more parts on their own, at their own origin, as a FreeCAD part, STEP or both, for spool drawings or to send out. Give each a part number (or number them all: prefix, start, step) and a description; the BOM can list them by number.
Pipe from Scan: reverse-engineer existing pipework from a 3D scan
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Import Scan reads OBJ, STL or PLY meshes and XYZ / ASC / PTS point clouds of any size. The whole scan is kept for measuring, a lighter copy is shown, and it's cached, so opening it again is quick. Any mesh or point cloud already in the document works too.
-
Pipe from Scan: click the pipe wall and MechFlow follows the pipe both ways, through the elbows, until it meets a flange, a plate (bulkhead, deck) or the end of the pipe. It measures:
- the OD, matched to EN or ASME;
- the straights, and the corners where they meet;
- the bend radius (3D / 2D / 5D / LR) and reducers in line;
- the rating and joint face of standard weld neck flanges fitted at each end.
It picks a pipe spec to match and shows the line coloured by how closely it follows the scan. OK makes a 3D sketch and a route of it, so it can be edited, have valves added and go in the BOM like any other. Pipe hangers and clamps along the way are stepped over, not taken for flanges.
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Checking it: the scan's points on the pipe are coloured by how far they are off the model (green close, amber check, red far), orange dots mark anything worth a second look (a flange only half seen, a hanger stepped over, a gap bridged, the line just stopping), and Save report writes a CSV of what was measured and how well it fits.
-
Correcting it: drag the grip on either end of the line or type a cut length; Set an end, Carry on past and Undo corrections. Each straight can be Auto (squared up when within 5° of X / Y / Z), Square or As measured; each end can finish differently. Work a section at a time: one line from flange to flange.
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Remove from Scan: a copy of the scan with the modelled pipe taken out, within a margin you set, so new pipe sits in what's left. The original scan is kept (hidden).
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Scan View (Drawing tab): puts a picture of the scan with the new pipe in it on the sheet as a labelled reference view, with the scan's colour and opacity and the pipe's colour of your choice.
Stress Check: SimulationXpress-style linear static analysis
A linear static check of a part or weldment, on FreeCAD's FEM (CalculiX, which comes with FreeCAD):
- Material: from the part, or pick one.
- Fixtures: click the fixed faces.
- Loads: a force (normal or along X/Y/Z), a pressure, water pressure (click one inside face, e.g. a tank's floor: every face the liquid touches is found, and each point gets ρ·g·depth) and the part's own weight.
- Mesh quality, then Run.
You get a colour plot of von Mises stress, the maximum stress and where it is, the factor of safety against yield (passes at 1.5 or more), and the maximum deflection. Leave out small holes and stubs (on by default) skips bolt holes and small bosses, which cost far more mesh than they change the result on a plate or tank. Fixtures and loads are kept with the part, so the check can be re-run after a design change.
It's a linear check: stresses at sharp internal corners and right at fixed edges read high, and when a plate deflects more than about half its thickness the real plate is stiffer than the result (but it needs stiffening anyway).
Motion Study: keyframe animation, camera moves and video export (new in 0.31)
Find it on the Features, Evaluate and Assembly tabs. A study is saved in the
.FCStd file and opens again with a double-click.
- Keyframes on a timeline: each key sets values at a time. Key from model captures the current parameter values; Key from configuration switches to a whole configuration from the Design Table. Anything a configuration can drive (sketch dimensions, feature values, member sizes, suppression) can be animated; Parameters... picks which values Key from model records.
- Easing: smooth (ease in and out), linear, or hold, per key.
- Camera: Camera from view stores the current view on a key; the camera then flies between keys, set the field of view per key, and add turns to orbit the model on the way.
- Play, Stop, Loop and a scrub slider; double-click a time in the table to go there. Update key, Delete key, Shift keys after... to make room.
- Export: MP4 or GIF from 720p up to 4K (or square), at the frame rate you pick, on the current, white, black or a transparent background, or a folder of PNG frames. Video export uses ffmpeg: point MechFlow at it with the ffmpeg... button if it isn't found on the PATH.
- Look: Viewport (as the 3D view draws it, fastest) or Studio dark / Studio light / White, rendered frame by frame like Render below.
Render: studio pictures of the model (new in 0.32)
Find it on the Features, Evaluate and Assembly tabs. Set up the view, then:
- Render (seconds): MechFlow's own studio renderer, using the VTK that comes with FreeCAD. Image-based studio lighting, a key light with shadows, ambient occlusion and a floor with a soft ground shadow. Backdrops: Studio dark, Studio light or White. Sizes from the current view up to 4K, Draft / Good / Best quality.
- Finishes picked for you: from each part's material (stainless, aluminium, cast iron, brass, rubber, glass, timber...), its Toolbox type (flanges and pipe bare steel, bearings machined, gaskets rubber, bolts zinc plated) or its colour (painted parts keep their colour as gloss paint). Change any group in the Appearances list: paint, powder coat, plastic, bare / machined / brushed stainless steel, galvanised, aluminium, cast iron, chrome, brass, copper, zinc, black oxide, rubber, glass, timber. The choice is saved with the part.
- See-through parts stay see-through: parts shown transparent in the view (context steelwork, decks, guards) render translucent with their outlines.
- Save image as PNG or JPEG.
| Component | Status |
|---|---|
| FreeCAD 1.1 | Required. Older versions are not supported. |
| SheetMetal Workbench | Optional, for the Sheet Metal tab. MechFlow offers to install it. |
| Fasteners Workbench | Optional, for Toolbox screws, nuts and washers. MechFlow offers to open the Addon Manager. |
| ffmpeg | Optional, for Motion Study MP4 / GIF export (PNG frames work without it). |
| CalculiX | For Stress Check. Comes with FreeCAD. |
Once listed: Tools → Addon Manager, search for MechFlow, then Install.
Download the latest release
(or clone this repository) and copy the folder into FreeCAD's Mod folder
as MechFlow:
| OS | Mod folder (FreeCAD 1.1) |
|---|---|
| Windows | %APPDATA%\FreeCAD\v1-1\Mod\ |
| macOS | ~/Library/Application Support/FreeCAD/v1-1/Mod/ |
| Linux | ~/.local/share/FreeCAD/v1-1/Mod/ |
Restart FreeCAD and choose MechFlow from the workbench list. The first time, MechFlow sets itself as the workbench FreeCAD opens in (you can change this under Edit → Preferences → General).
SOLIDWORKS-style mouse navigation: Edit → Preferences → General → Preference packs → MechFlow → Apply.
- New part: pick the Front Plane, right-click → Sketch, draw a profile and dimension it until it turns black.
- Features tab → Extruded Boss/Base: drag the arrow or type the depth, then add holes with Hole Wizard.
- Drawing tab → Make Drawing: pick a sheet and get a dimensioned three-view drawing with the title block filled in.
- Assembly tab → New Assembly → Insert Components, then Mate and Smart Fasteners.
- Supplier Pack: PDFs, STEP, DXF profiles and the BOM, zipped and ready to send.
MechFlow changes how FreeCAD looks and behaves, but the geometry is still FreeCAD's, so a few things work differently from SOLIDWORKS.
Differences and current limits
- Drawings are stored in the part's
.FCStdfile, not a separate drawing file. There is no Model Items import of sketch dimensions: MechFlow adds overall and hole dimensions, and you add the rest with Smart Dimension. - An assembly shows each part in its active configuration; two configurations of the same part can't be in one assembly yet.
- FreeCAD needs an assembly to be saved before it can link parts from other files. It prompts you when this happens.
- Editing an existing mate, and the gear, rack-and-pinion and screw mates, use FreeCAD's own joint dialog.
- Mid-plane and through-point reference planes keep their position when the model changes. Reopen them and press OK to update.
- Weldment members follow straight sketch lines (no curved members yet).
- Toolbox fasteners are attached to their hole edge rather than held by mates, and only metric (ISO 273) holes are sized automatically; for inch fasteners pick the size yourself.
- Bearings are modelled to their boundary dimensions, with simplified rings and balls.
Standards and data sources
- Flange and fitting dimensions come from published EN 1092-1, ASME B16.5,
B16.9, B36.10M and ISO 15 tables; sources are listed in
mechflow_gui/stdparts_data.py. - Steel section dimensions come from British Steel datasheets and
EN 10056-1 / 10210 / 10219; see
mechflow_gui/steel_data.py. - Check critical dimensions against the current standard before manufacture.
tests/ has smoke tests that drive the real FreeCAD GUI: they build parts,
use each panel the way a user would, and check the resulting geometry. On
Linux they run headless under Xvfb (tests/run_tests.sh); on any OS,
including Windows, they run inside FreeCAD from the Python console:
exec(open(App.getUserAppDataDir() + "Mod/MechFlow/tests/run_in_freecad.py").read())See tests/README.md.
Issues and pull requests are welcome, especially for tools that still behave like FreeCAD rather than SOLIDWORKS. Please run the tests before sending a change. Two rules of the codebase:
- Don't install Qt event filters on FreeCAD's own widgets. Use timers,
Gui.Selectionobservers and document observers instead (event filters have crashed FreeCAD). - Never keep references to FreeCAD's tree items. FreeCAD rebuilds the tree, so look the items up again each time.
LGPL-2.1-or-later, the same as FreeCAD. See LICENSE.
MechFlow is not affiliated with or endorsed by Dassault Systèmes. SOLIDWORKS is a trademark of Dassault Systèmes.