ForemkaCAD
PLEN
Open the editorEditor

Basic Part Design

The part from FreeCAD's Basic Part Design Tutorial, built feature by feature: sketches, extrusions, a mirror and projected edges.

7:12 · English narration, subtitles in English and Polish · Watch on YouTube

Step by step

Exactly what the narrator says, chapter by chapter. Click the time next to a chapter to jump the video there.

0:00 Introduction and drawing

  1. In this tutorial we model the part shown in this drawing, using Foremka.
  2. It follows FreeCAD's Basic Part Design Tutorial step by step.
  3. We start with a sketch, build the base solid, and then add and remove material with features.
  4. Foremka opens with an empty design. Every step you take lands on the timeline at the bottom.

0:30 Base sketch on the YZ plane

  1. Click Sketch. Foremka asks for a sketch plane.
  2. Pick the YZ plane. You can click it in the view, or in the Origin folder of the browser.
  3. Zoom out a little with the mouse wheel, then choose the Line tool.
  4. Starting at the origin, draw a closed shape roughly like this. It does not have to be exact.
  5. While you draw, Foremka adds horizontal and vertical constraints, and closes the contour at the start point.
  6. The first point sits on the origin, so the shape is anchored. Three degrees of freedom are left.
  7. Choose Equal, then click the bottom line and the vertical line. Both get the same length.
  8. Select the bottom line, click Dimension, place the dimension and type 26 mm.
  9. Do the same with the top line: 5 mm. The sketch is now fully constrained.
  10. Click Finish Sketch.

1:38 Symmetric extrude, 53 mm

  1. Select the profile and click Extrude.
  2. The part is 53 mm long. Set Direction to Symmetric and Distance to 53 mm: half on each side of the sketch plane.
  3. This symmetry will pay off when we mirror features. Click OK.

1:59 Notch sketch on the back face

  1. Drag with the left mouse button on an empty area to orbit, until the back of the part faces you.
  2. Click Sketch and pick the back face. The new sketch is attached to that face.
  3. The outline of the face is projected into the sketch automatically. These purple lines play the role of external geometry in FreeCAD.
  4. Use 2-Pt Rect to draw a rectangle near the top corner.
  5. Dimension the top edge to 11 mm and the side edge to 5 mm. The D key is a shortcut for Dimension.
  6. Choose Coincident, click the corner of the rectangle and then the corner of the face. The sketch is fully constrained.

2:48 Cut through all

  1. Finish the sketch, select the rectangle and click Extrude.
  2. Set Operation to Cut and Extent Type to All. This is FreeCAD's pocket with Through all: the cut goes through the whole part.
  3. Click OK.

3:09 Mirror the cut

  1. Now the mirror. Click the cut on the timeline to select it.
  2. Open the more menu of the CREATE group and choose Mirror. The dialog starts in Features mode, with our cut already in it.
  3. For the mirror plane, click YZ in the Origin folder. It lies in the middle of the part, which is why we extruded symmetrically.
  4. Click OK. The second notch appears at the other end.

3:41 Side blocks and their mirror

  1. Next, the side blocks. Start another sketch on the same back face.
  2. Draw a rectangle in the lower corner and dimension it: 7 mm wide and 16.7 mm high.
  3. Make its corner coincident with the corner of the face.
  4. Finish the sketch, select the rectangle and click Extrude.
  5. Set Operation to Join and Distance to minus 26 mm. The minus sign sends the extrusion into the part, like Reversed in FreeCAD.
  6. Click OK, then mirror this feature the same way: select it on the timeline, choose Mirror, plane YZ, OK.

4:36 Square on the sloped face

  1. Orbit back to the front and fit the view.
  2. The part already looks like the drawing.
  3. The drawing places a 17 mm square on the slope, but the hole runs perpendicular to the back face. So we draw the square on the slope first, as a reference. Click Sketch and pick the sloped face.
  4. Draw a rectangle. Make two adjacent sides Equal and dimension one of them to 17 mm: a 17 mm square.
  5. Click the top right corner of the square, hold Ctrl and click the top right corner of the face. Then choose H Dist and type 7 mm.
  6. Select the same two points again and add V Dist of 11 mm. The square is fully constrained.
  7. Finish the sketch. This square only marks where the opening lies on the slope. The cut itself starts from the back face.

5:48 Hole from the back face

  1. Orbit to the back again and start a sketch on the back face.
  2. The square from the slope shows through the part. Choose Project, click all four of its edges, then OK.
  3. The four projected edges already form a closed profile, so there is nothing else to draw.
  4. Finish the sketch, select the projected outline and extrude it with Cut and All.

6:32 Result

  1. Hide the sketch on the slope. We only needed it as a reference for the projection.
  2. Orbit to the front. The opening on the slope is exactly 17 by 17 mm.
  3. Unlike in FreeCAD, there is no need to refine the shape: Foremka merges the coplanar faces for you, so no extra lines remain.
  4. Every step stays on the timeline. Double-click a feature to change it later.
  5. This tutorial and your model are complete.

More tutorials

5:59

Introduction to Foremka

Your account, the settings, the interface and moving around the view, then a first part you change later from the timeline.

3:14

A drinking glass, rendered in Blender

A profile revolved around an axis, a shell and fillets, then green glass and a photorealistic render straight from the editor.

8:34

Surface modeling a spoon

An outline, a side profile and cross sections, a patch over the bowl and a lofted handle, stitched and thickened into a solid.

8:30

Joints, standard parts and gears

Bearings from the parts library, a block sliding along a shaft between limits, two gears turning together and a rack that turns rotation into straight motion.