FreeCAD Sketcher guide:
A first part, with fewer dead ends.

For a first part, separate four jobs: create the profile, define its shape with constraints, turn it into a solid, and export the final solid. A Body holds the PartDesign history; a sketch alone is not an STL-ready solid. This guide uses a simple closed rectangle and a positive Pad length, then preserves the editable document before exporting. Exporting a mesh is not a guarantee that a particular printer can manufacture the part.

1. Create a new document and switch to PartDesign. Use its Create sketch command, which creates a Body if needed; choose a Body base plane such as XY and confirm OK.
2. In sketch edit mode, use Rectangle in Corner, width, height mode, with Frame and Rounded corners off. Pick the two opposite corners, then press Esc or right-click to finish the drawing tool.
3. Set the intended width, height and position using dimensional and geometric constraints. Check Solver messages and make sure the regular profile is closed without intersecting or duplicate edges.
4. Press Close to leave sketch edit mode, select the sketch in the tree, invoke Pad, choose Dimension and a positive Length, inspect the preview, then press OK.
5. Inspect the resulting solid and save the document as an FCStd file with File → Save.
6. Select only the intended Body, confirm its Tip is the final solid, then use File → Export, choose STL, enter a filename and press Save. Check the imported part size and shape in the destination application before printing.

Do not select every object in the history or treat Save as an STL export.

Sketcher edits 2D geometry; PartDesign makes features inside a Body. The intended Body must be active when adding its features. Double-clicking a sketch starts sketch edit mode, whereas double-clicking a Body toggles its active state. Close the sketch editor before selecting its profile for Pad. A disabled command or wrong destination is a reason to inspect context, not proof that constraints must be deleted.

1. Check whether a sketch task is still open. If so, finish the current sketch operation and press Close.
2. Switch to PartDesign and locate the intended Body in the tree. If it is not active, activate that Body using its context menu or double-click it.
3. Select the intended sketch inside that Body, then invoke the required feature and inspect its preview before pressing OK.
4. Confirm the new feature belongs to the intended Body and save the FCStd document. If the command still fails, report the exact error and selected object rather than guessing.

An active Body and a selected sketch are different pieces of state; the guide cannot see either one.

The sketch plane determines where the profile lives and which way its normal points. With no face preselected, PartDesign Create sketch lets you choose a Body reference plane. A selected face on the active Body can instead become the support. Base planes avoid a dependency on the changing faces of later features; face support can be convenient, but upstream edits can affect it. This does not establish which support your existing sketch currently uses.

1. For a new first sketch, clear any unintended face selection, invoke PartDesign Create sketch, select the intended base plane and press OK.
2. If deliberately sketching on a face, select that face of the active Body before invoking Create sketch.
3. Confirm the sketch orientation in edit mode and the extrusion or cut direction in the later feature preview. Do not accept a wrong preview just because the sketch looks right from one camera angle.
4. Save the document after the supported sketch and subsequent feature are correct.

Do not promise that referencing a generated face is immune to changes in earlier features.

Closure is about connected contour endpoints and a valid profile. Full constraint is about eliminating the geometry’s remaining freedom to move. A sketch can have fixed endpoints that do not join, so zero degrees of freedom does not prove closure. Conversely, a closed profile can still move or change size and may be usable for Pad before it is fully constrained. Fully constraining the intended design remains useful for predictable later edits.

1. Read the actual Solver messages and the feature error separately; note whether the issue is motion, a conflict or an invalid profile.
2. Inspect the regular contour for tiny endpoint gaps, intersections, duplicate edges or branches. Construction geometry is not the solid profile.
3. Repair only the identified profile issue, then address any remaining intended dimensions or positioning constraints.
4. Leave sketch edit mode, retry Pad and inspect its preview before OK. Save the FCStd document after the intended solid is created.

Adding more dimensions does not close an endpoint gap, and a fully constrained label does not certify the shape as a valid face.

Two endpoints can look coincident at the current zoom without being connected in the sketch. A Coincident constraint between the intended endpoint points makes them share a position. Select the points, not just two whole edges when the goal is an endpoint joint. Depending on Sketcher preferences, coincidence and point-on-object tools may be unified; the intended relationship is still endpoint-to-endpoint coincidence.

1. Save the document before repair. Double-click the relevant sketch to edit it and locate the intended joint.
2. Select the two endpoint points that should join and invoke the Coincident constraint tool; avoid applying a second relation if that joint is already constrained.
3. Check the solver status and inspect the new connection. If a conflict appears, inspect its reported constraints rather than forcing the change.
4. Finish sketch edit mode, retry the feature preview, accept OK only when it is correct, and save the repaired FCStd document.

Dragging an endpoint near another one does not by itself prove a closed profile.

Validate sketch is a targeted analysis and repair tool, not a blanket cleanup command. It runs outside sketch edit mode. Its Missing coincidences section can find nearby endpoints lacking coincidence constraints, mark them, and add those constraints with Fix. The tolerance controls which points qualify; increasing it indiscriminately can connect points that were meant to stay separate. Review the marked joints against the intended shape first.

1. Save a copy of the FCStd document, leave sketch edit mode, and select the sketch in the tree.
2. Invoke Sketch → Validate sketch. In Missing coincidences, keep Ignore construction geometry checked when diagnosing the solid profile, and press Find.
3. Dismiss the count dialog and inspect the marked positions. Use Highlight troublesome vertexes if needed; change the tolerance only when the intended joint has been identified.
4. Press Fix only if all the found joints are intended connections at the chosen tolerance, then press Close. Otherwise repair the intended endpoints individually in sketch edit mode. Reopen the sketch and check solver messages and the profile.
5. Retry the intended Pad or Pocket preview; confirm OK only for the correct result and save the repaired FCStd document.

Do not use a large tolerance or unrelated validation repair options to make an unknown sketch appear valid.

Construction geometry supports dimensions and geometric relationships inside a sketch; it is excluded from the profile used to generate a solid. Its default appearance differs from regular geometry, but colors are configurable. Toggle construction geometry has two behaviors: with geometry selected it changes those elements, and with nothing selected it changes the mode of future drawing tools. Choose the behavior deliberately.

1. Edit the sketch and identify which elements should form the real outline and which should remain helpers.
2. Select only the intended profile elements and invoke Toggle construction geometry to convert them to regular geometry if necessary.
3. Check the remaining regular contour for closure and solver issues. Do not convert every construction helper into a profile edge.
4. Close the editor, retry Pad, inspect the solid preview, confirm OK and save the FCStd document.

With no selection, toggling construction changes what future tools draw; it does not convert the existing outline.

Dimensions can fix a shape’s size while leaving its position or orientation free. Solver messages report the remaining degrees of freedom; clicking the underlined under-constrained message selects the affected elements. The number alone does not say which constraint your particular design needs. Constrain the intended geometric relationships and position, then dimensions, rather than adding arbitrary constraints just to reach zero.

1. Edit the sketch and read Solver messages. Click the under-constrained message to locate the affected elements.
2. Inspect what can still move or change relative to the sketch origin and existing geometry. Distinguish translation, rotation and size.
3. Add only the missing intended relationship or dimension and recheck solver status after each change; stop to investigate any redundant or conflicting result.
4. Once the intended shape and location are defined, leave edit mode, inspect downstream features and save the FCStd document.

Width and height alone do not necessarily locate the rectangle, and this guide cannot infer an unseen missing constraint from a DoF count.

Geometric constraints specify relationships such as horizontal, vertical, coincident or equal. Driving dimensional constraints specify values such as width and height. Horizontal distance measures separation along the sketch X direction; vertical distance measures separation along Y. Selecting one endpoint makes these distances relative to the origin. Existing automatic constraints count too, so inspect them before repeating a rule.

1. Edit the rectangle sketch and inspect its existing geometric relationships and solver status.
2. For width, select the intended horizontal edge or its endpoint pair and invoke Constrain horizontal distance. Enter the required value if prompted, or edit the resulting constraint value.
3. For height, select the intended vertical edge or endpoint pair and use Constrain vertical distance in the same way. Give explicit units for intended physical dimensions.
4. Locate the rectangle relative to the origin with an intended relationship or coordinate dimensions, then check for remaining freedom, redundancy or conflict.
5. Close the sketch, inspect its feature result and save the FCStd document.

Do not add a horizontal or equal constraint again just because its icon was overlooked; existing automatic constraints can already impose that relationship.

A redundant constraint repeats information already imposed by the constraint system. The solver can identify involved constraint indices, and clicking its underlined message selects them. The reported set is diagnostic help, not an instruction to erase the sketch’s design rules. More than one possible constraint choice can resolve redundancy; decide which rule is unnecessary for the intended design, then recheck the result.

1. Save a copy before changing the constraint system. Edit the sketch and record the solver message and involved indices.
2. Click the redundant-constraint message to select the reported constraints, then inspect their types, values and affected geometry.
3. Remove only an identified unnecessary rule, or turn an appropriate extra dimensional measurement into a reference dimension instead of a driving rule.
4. Recheck Solver messages and the intended dimensions and shape. If the evidence is insufficient, describe the selected constraints rather than delete more blindly.
5. Close the editor, inspect the resulting features and save the repaired FCStd document when correct.

Deleting all constraints may remove intended dimensions and relationships rather than repair the specific redundancy.

Conflicting constraints cannot all hold simultaneously. Solver messages identify involved indices, and clicking the underlined message selects that set. The guide cannot choose a constraint number from an unseen sketch: its type, value, affected elements and intended shape matter. Inspect the proposed set and the latest change, correct only the identified incompatible rule, and verify that the intended design survives.

1. Save a copy, edit the sketch and record the exact solver message and constraint indices.
2. Click the conflict message and inspect the selected constraints and their geometry. Compare the dimensions and relationships with the intended design.
3. If the conflict followed a new unintended constraint, undo that change; otherwise edit or remove only a rule whose incompatibility has been established.
4. Recheck Solver messages after that single change. Verify the intended dimensions and shape before continuing.
5. Close the sketch, inspect downstream features and save the correct FCStd document.

Do not delete the entire reported set or guess a constraint index without the sketch details.

A fully constrained sketch has no remaining free motion, so dragging it is not the normal way to change its design. For a dimension-controlled sketch, edit the relevant driving constraint value. Double-click the value in the view or the constraint in the Sketcher Dialog to edit it. This preserves the rule while changing its target value; it is different from deleting constraints to free the geometry.

1. Double-click the sketch in the tree to enter edit mode and identify the driving dimension for the desired change.
2. Double-click that dimensional constraint’s value or its entry in the Constraints list, enter the intended value and confirm the dialog.
3. Check Solver messages and the changed profile. If the chosen item is only a reference measurement, inspect which driving rules actually determine it.
4. Close the editor, refresh the document if needed, inspect dependent features and save the updated FCStd file.

Fully constrained does not mean permanently uneditable, and freeing every edge is not a prerequisite for changing a driving dimension.

A driving dimension constrains geometry; a reference dimension reports the value produced by other constraints and does not add a new restriction. Reference dimensions are useful for checking a result without over-constraining it. Toggling a selected dimensional constraint changes that item, while invoking the tool with none selected changes the creation mode for future dimensional tools. Converting a measurement to driving can conflict with existing rules.

1. Edit the sketch and identify whether the item is a driving dimension or a reference measurement; appearance alone can vary with preferences.
2. To change the design, edit an existing driving dimension that controls it instead of trying to force a reference result.
3. If a dimensional constraint should become a measurement, select that constraint and invoke Toggle driving/reference constraint.
4. Check that the intended driving rules remain and Solver messages are acceptable; close the editor and save the FCStd document.

Toggling with nothing selected changes future dimension tools, not the existing selected measurement you meant to edit.

Closure is only one profile requirement. Regular contours used to form a solid must not cross themselves or other contours, share edges, contain duplicate edges, or form T-junctions. Separate nested closed contours can define voids. Construction helpers are excluded from these profile rules. A closed-looking drawing or zero degrees of freedom therefore does not establish a valid face.

1. Save a copy, edit the sketch and distinguish regular profile edges from construction helpers.
2. Inspect the intended contours for crossings, coincident duplicate edges, shared segments and branch points. Locate the specific issue before modifying geometry.
3. Correct only the identified unintended element or connection and review any affected constraints and Solver messages.
4. Leave edit mode, retry the feature preview, accept OK only when the intended solid is shown and save the repaired FCStd document.

Do not use Validate sketch’s missing-coincidence repair as proof that duplicates or intersections have been resolved.

Pad extrudes a selected sketch into a solid feature. For a simple first extrusion, Dimension uses a positive Length; Reversed changes direction. A sketch must have a valid closed regular profile, but being fully constrained is a separate design-quality question. An existing supported face can also be padded, though this note describes the selected-sketch workflow. The preview must match the intended shape and direction before the operation is committed.

1. Finish sketch editing with Close. Switch to PartDesign, activate the intended Body and select its valid profile sketch in the tree.
2. Invoke Pad, choose Dimension and enter the intended positive Length. Use Reversed if the preview points the wrong way.
3. Inspect the solid preview for the expected outline, length and direction; address any profile or solver error rather than accepting a guessed result.
4. Press OK to create the Pad, inspect the resulting feature in the Body and save the FCStd document.

Typing a length prepares the operation; OK commits it. A fully constrained open contour still cannot generate the required solid.

Pocket is subtractive: the selected profile is extruded as a cut through material already present in the Body. A closed sketch outside the solid or a cut directed away from it cannot remove the intended material. Dimension gives a chosen depth; Through all cuts through the encountered material in its direction, and Reversed changes that direction. The guide cannot infer your sketch support or solid from a symptom.

1. Confirm the intended Body already contains the solid to cut. Finish sketch editing, activate that Body and select the valid closed cut-profile sketch.
2. Invoke Pocket and choose Dimension with the intended positive Length, or Through all when the intent is a through-cut.
3. Inspect the preview: the cutting volume must intersect the intended material. Check the sketch support and Reversed setting if it does not.
4. Press OK only for the intended cut, inspect the resulting solid and save the FCStd document. If the result is wrong, provide the support, type, direction and exact error.

Do not add a new Body or delete constraints as a generic cure for a cut that misses its material.

A Body’s Tip is the feature whose shape the Body exposes to other tools. It is normally the latest created feature but can be moved to an earlier one. Visibility is separate: showing an older feature does not by itself change the Tip. Exporting the Body therefore requires checking its Tip, while exporting an explicitly selected older feature exports that selected stage. The guide cannot tell which object your current export selected.

1. Expand the intended Body and inspect its Tip property and the feature it references.
2. Compare that feature with the intended final result. Check whether the export selection was the Body, an older feature, or several history objects.
3. If the Tip was intentionally rolled back for editing, complete that workflow and verify the intended final Tip before exporting again; do not move it blindly to hide errors.
4. Save the correct FCStd document, clear the prior selection and export only the intended Body or final solid feature. Verify the new exported shape.

Seeing the final Pocket in the tree is not proof that the Body’s exported Tip or selected export object is that result.

Refresh recomputes a document that needs updating; it does not repair invalid profiles or contradictory constraints. Solver messages distinguish malformed constraints, conflicts and other failures. Validate sketch can inspect malformed constraints or degenerate geometry, but those are different from a missing endpoint joint. Part Check geometry can inspect the resulting solid and highlight reported faulty geometry; a successful check does not certify printer-specific manufacturability.

1. Save a copy before structural repairs. Record the affected object, exact error and the last intended change.
2. If the document requires recompute, use Edit → Refresh. If a feature still fails, inspect its profile and the sketch’s Solver messages rather than repeatedly refreshing.
3. For a malformed sketch, leave edit mode, select it and use Validate sketch’s relevant analysis; avoid unrelated Fix options until the cause is established.
4. For a completed solid, switch to Part, select the whole intended Body or solid, invoke Check geometry and press Run check if its settings panel is shown. Inspect any reported errors.
5. Correct only the established modeling issue, recompute and inspect the result, then save the FCStd document. Ask for help with the exact error if it remains unresolved.

Recompute and geometry checking are diagnostics, not automatic mesh repair or a promise that all errors are fixed.

FreeCAD parameters carry units, while STL does not encode a unit system. The official STL export tutorial describes millimetre-based export coordinates, so the receiving application must interpret those numbers consistently. Changing display units is not the same as resizing geometry. Check one intended physical dimension in the editable model and in the imported mesh before guessing a scale factor; this guide cannot see your model or slicer’s interpretation.

1. Check the intended sketch dimensions and Pad or Pocket lengths. Give explicit units such as mm or in when entering physical dimensions.
2. Inspect the document Unit System through File → Document information when display values are confusing; document units can override the default preference.
3. Save the correct FCStd document and export the intended final solid to STL.
4. Compare a known expected dimension with the imported mesh in the receiving application. If the values differ, identify that application’s assumed units before resizing or re-exporting.

Do not prescribe a universal scale factor or remesh the part just because an STL import appears too small.

Save writes the FreeCAD document, preserving the modeling work for later edits. Export writes selected objects in another format. An STL is a mesh handoff, not a substitute for the document containing the sketch, constraints and feature history. Keep the FCStd master and the STL as separate files. Save As can create a separately named document before making a repair; exporting again does not itself save the updated master.

1. Finish the current sketch or feature operation and inspect the intended result.
2. Use File → Save for the active document; for a new document, supply an FCStd filename and press Save. Use File → Save As when keeping a separately named version before changes.
3. Select the intended final Body or solid and use File → Export to write the STL separately.
4. After later modeling changes, save the FCStd document again and create a new STL export when needed. Confirm both filenames and the exported shape.

An STL cannot replace an editable sketch-and-constraints document or preserve the parametric history as such.

File → Export operates on selected objects. Selecting everything can include hidden objects and multiple intermediate stages. For a PartDesign part, select the Body itself or its final solid feature, not both plus the entire history. The Body’s Tip must expose the intended final result. Direct STL export creates a mesh from that selected solid; keep the editable FCStd document separately.

1. Finish the current operation, recompute and inspect the intended final solid. Save the FCStd document.
2. Clear any previous selection. In the tree select only the intended Body or final solid feature; confirm the Body’s Tip if exporting the Body.
3. Choose File → Export, select the STL mesh file type, enter the intended .stl filename and press Save.
4. Open or import the resulting mesh in the receiving application and inspect its shape, object count and known dimensions before printing. If it is wrong, check selection, Tip and units rather than exporting the whole tree.

Select all also selects hidden and intermediate objects; their invisibility is not a guarantee that they will be omitted.

A solid’s curved surface is represented by planar facets when exported as STL. The official direct-export tutorial provides Maximum mesh deviation as a mesh-resolution control: a lower value makes a higher-resolution exported mesh. This changes the approximation of the selected solid, not its driving sketch dimensions. It cannot repair an invalid profile, choose printable wall thickness, or prove which mesh settings your current export used.

1. First confirm the intended solid shape and dimensions are correct, and save its FCStd document.
2. Load the Mesh workbench if the mesh format preferences are not available. Open Preferences and find Import-Export → Mesh Formats.
3. For the direct solid-to-STL export workflow, reduce Maximum mesh deviation when a finer approximation is required; do not change unrelated mesh repair settings.
4. Select only the intended final solid and export a new STL. Compare the curved surface, dimensions and resulting file with the previous export before choosing the result.

A denser mesh does not repair a bad solid or establish that a printer can reproduce the design.