CADsmit Watch on YouTube

Unit 06 · Lecture 12

Center marks, hole notes and dimensions

Views alone don’t make a drawing usable. This lesson adds the symbols and dimensions a machinist needs, and edits the part along the way to show how the drawing follows the model.

Video 16:26Reading 9 minUpdated 26 October 2026

Lecture video, 16:26. The written steps below follow the video, with timestamps for each part.

What you will build

The finished curved disk drawing: center marks, a center pattern, hidden lines, centerline bisectors, chamfer and thread notes, DIN-style horizontal dimensions and a units note.

You will learn

  • Center Mark vs. Center Pattern
  • Sketching on a curved part with an offset plane and Project Geometry
  • Hidden lines and centerline bisectors
  • Chamfer and Hole/Thread feature notes
  • Style Editor, decimal comma, precision and tolerances

Before you start

Continue from the drawing in Lecture 11.

Step by step

  1. 01

    Add center marks

    0:00

    On the Annotate tab, click each circle’s circumference with Center Mark. Skip the three patterned holes.

  2. 02

    Use Center Pattern for patterned holes

    0:42

    Choose Center Pattern, click the pattern centre, then each hole in turn and back to the first. Right-click → Create. The marks follow the pattern circle instead of sitting square, which shows the holes came from a pattern.

  3. 03

    Add the Ø5 hole on the curved face

    1:30

    You can’t sketch on a curved face. In the part, create an Offset from Plane work plane from the YZ plane at 100 mm. Sketch on it, Project Geometry the curved face’s outline, and centre a Ø5 circle using vertical and horizontal constraints to the midpoints.

    Extrude in Cut mode with To, picking the inner face so the hole stops there. Hide the plane with Alt+V and save. The drawing updates.

  4. 04

    Show hidden lines

    6:28

    Double-click the base view and turn on Hidden Line. Dashed lines now show the new hole and other internal cuts.

  5. 05

    Add centerline bisectors

    7:09

    For holes seen side-on, use Centerline Bisector and click the two edge lines of each hole. Add them for the new hole, the three holes in the section and the centre cavity.

  6. 06

    Chamfer and hole/thread notes

    8:39

    Feature Notes → Chamfer: click the angled line first, then the outer edge, to get 0.5 × 45°. The opposite order gives wrong values.

    Hole/Thread: the outer box of a threaded hole is the thread and the inner circle is the drill. Edit the note to add the # quantity, delete the depth and type THRU for through holes.

  7. 07

    Set DIN dimension styles

    11:30

    Manage → Style Editor → Default Standard (DIN) → Dimension → Default (DIN). Keep millimetres, use a comma decimal marker, set precision, and make text horizontal, first line centered for linear, radius, diameter, and notes and leaders. Save.

  8. 08

    Dimension, tolerance and finish

    12:53

    Add dimensions such as R45. Turn off Edit dimension when created if the pop-up gets in the way. Tolerance types (Symmetric, Deviation, Limits) are set per dimension. For the slanted 15.5, right-click → Dimension Type → Aligned and raise the precision to 1 decimal. Add a text note: All dimensions are in millimetres.

Why the symbols matter

Center marks are references

A machinist measures from centres, not edges. Center marks and center lines give those references, and tolerances can only be applied to features that have them.

Drawings stay linked to parts

Because the IDW reads the IPT, adding the Ø5 hole in the part updated every view. Change the model and the drawing follows. Never redraw geometry in the drawing.

Common mistakes

Practice exercise

Open your curve part drawing and fully annotate it: a center pattern for the three M10 holes, a thread note with quantity, chamfer notes and DIN-style dimensions.

Check yourself

Which symbol marks holes made by a circular pattern?

Center Pattern.

How do you sketch on a curved face?

You can’t. Create an offset work plane and project geometry onto it.

What replaces the depth in a through-hole note?

THRU.

A 15.5 dimension shows as 16. What do you change?

The dimension’s precision.

Want the graded version? Take the 5-question lesson quiz in the course player after the video.

Written by the CADsmit instructor from the lecture recording and checked in Autodesk Inventor Professional 2027. Last updated 26 October 2026. Spotted an error? Tell us.