Types of Views in Engineering Drawing: Orthographic, Section, Isometric
The six principal views, first-angle vs third-angle projection and their symbols, auxiliary, sectional, detail and broken views, and isometric vs oblique vs perspective, all drawn on one L-bracket with the correct line types. Includes what India's SP 46 and ISO 5456-2 require and how SolidWorks, CATIA and AutoCAD generate each view.

The main types of views in engineering drawing are orthographic (principal) views, such as the front, top and side views; auxiliary views of inclined faces; sectional views that show the inside of a part; detail, broken and partial views that enlarge, shorten or crop a view; and pictorial views (isometric, oblique and perspective) that show the part in 3D. Orthographic views are laid out in either first-angle or third-angle projection. India's BIS practice uses first angle and the US uses third angle.
This guide draws one simple part, an L-bracket with a hole and a slot, and shows it in every kind of view. Each view uses the correct line types, and we have checked the projection rules against the BIS and ISO standards. You will also see how SolidWorks, CATIA and AutoCAD generate the same views from a 3D model.
In short
- An object can be drawn in six principal views, labelled A to F: front, top, left, right, bottom and rear. Most parts need only two or three (IS SP 46:2003, Section 8B, which follows ISO 5456-2:1996).
- First angle puts the top view below the front view and the left view on the right. Third angle puts the top view above and the right view on the right. The views themselves are identical; only where they sit on the sheet changes.
- BIS's drawing code SP 46:2003 says first-angle projection is the basic requirement for drawings prepared after 31 December 1991. ASME Y14.3 practice in the US is third angle.
- Line types carry meaning. Visible edges are continuous wide lines, hidden edges are dashed narrow lines and centre lines are long-dash dotted narrow lines. Wide lines are twice the width of narrow lines, for example 0.7 mm and 0.35 mm (SP 46 Tables 6.8 and 6.9).
- An isometric projection shrinks every edge by . Most people draw full size instead, an isometric drawing, which is 1.225 times larger.
What are the types of views in engineering drawing?
An engineering drawing has to describe a 3D part on a flat sheet so precisely that someone else can make it. No single picture can do that, so drawings use a set of views, each of which answers a different question. The table sums them up; the sections below explain each one.
| View | What it shows | Use it when |
|---|---|---|
| Orthographic (principal) views: front, top, side | The part seen square-on from one direction, with no distortion | Always: these carry the shape and the dimensions |
| Auxiliary view | The true shape of a face that is inclined to the principal planes | A sloping face carries a hole, slot or outline that would look distorted in the principal views |
| Sectional view (full, half, offset, aligned, broken-out, revolved, removed) | The part as if cut by a plane, with cut material hatched | Internal features would otherwise be a confusing mass of hidden lines |
| Detail view | A small area redrawn at a larger scale | A feature is too small to see or dimension at the drawing scale |
| Broken (interrupted) and partial views | A long part with its uniform middle removed, or only the needed part of a view | A full view would waste space without adding information |
| Pictorial views: isometric, oblique, perspective, exploded | The part in 3D in a single picture | Explaining a concept, showing assembly order or helping a non-specialist read the drawing |
The example part used in this guide
Every figure below shows the same part, so you can see how each kind of view describes it differently. The part is an L-bracket. Its base plate is 80 × 50 × 12 mm, and the upright at the left end is 60 mm high and 12 mm thick. A 14 mm diameter hole passes through the base, and a 26 × 10 mm slot passes through the upright. The script that draws every figure takes its geometry from one shared file, so the views cannot disagree with each other.
What are the six principal views in orthographic projection?
Orthographic projection draws the part as seen from very far away along one direction, so the lines of sight are parallel and meet the sheet at right angles. Faces parallel to the sheet appear at true size and shape. An object can be shown in six principal views, labelled by the direction of viewing. In SP 46 and ISO 5456-2, these are A (from the front), B (from above), C (from the left), D (from the right), E (from below) and F (from the rear).
The front view, A, should be the most informative view of the part. It is normally drawn in the part's functional, manufacturing or mounting position. The standard then asks for as few views as will define the part completely and without ambiguity. It also asks you to choose views that avoid hidden lines and do not repeat detail. In practice, that usually means two or three views.
The bracket needs three. The front view shows the L, but the hole and slot appear only as dashed hidden lines. The top view shows the hole as a circle. A side view shows the slot's true shape. Leave out any one of the three and some feature's shape or position becomes a guess.
First angle vs third angle projection: what is the difference?
In first-angle projection the object sits between you and the projection plane, so each view is drawn on the far side of the object. In third-angle projection the plane sits between you and the object, so each view is drawn on the side you looked from. The views themselves are identical in both systems; only their positions on the sheet differ.
Imagine the part inside a glass box. In third angle you look through each glass wall, trace what you see onto it and unfold the box, so each view lands next to the face it looks at. In first angle you trace each view onto the wall behind the part, so after unfolding it lands on the opposite side.
| First-angle projection | Third-angle projection | |
|---|---|---|
| Object position | Between the observer and the projection plane | Behind the projection plane |
| Top view (B) | Below the front view | Above the front view |
| View from the left (C) | On the right of the front view | On the left of the front view |
| View from the right (D) | On the left of the front view | On the right of the front view |
| View from below (E) | Above the front view | Below the front view |
| Rear view (F) | Left or right, as convenient | Left or right, as convenient |
| Symbol | Truncated cone on the left, circles on the right | Circles on the left, cone on the right |
| Where it is used | India (IS SP 46), most ISO countries, Europe | United States (ASME Y14.3) |
How do you read the first- and third-angle symbols?
The symbol shows a truncated cone in two views: its side view (a trapezoid) and its end view (two concentric circles). In both symbols, the narrow end of the cone points left.
- First angle: the circles sit on the right. That is where first angle places the view from the left, which looks at the small end.
- Third angle: the circles sit on the left, next to the cone's narrow end.
IS 15021 (Part 2), which is identical to ISO 5456-2, sets the proportions. The small end's diameter equals the drawing's lettering height h. The large end's diameter and the cone's length are both 2h, so with 5 mm lettering the cone is 10 mm long. The symbol must appear in the space provided for it in the title block.
A drawing laid out with the reference-arrow method needs no symbol. In that method, each view is labelled with a capital letter and placed wherever is convenient, and a matching arrow on the principal view shows the viewing direction.
Which projection is used in India, the US and Europe?
India uses first-angle projection. BIS's SP 46:2003, Engineering Drawing Practice for Schools and Colleges shows both methods. It states that "as a basic requirement" first-angle projection only is to be followed for drawings prepared after 31 December 1991. Its projection rules are based on IS 15021 (Part 2):2001, which is identical to ISO 5456-2:1996.
Internationally, ISO 128-3:2022 (views, sections and cuts) follows the projection methods in ISO 5456-2, which defines both first and third angle. SOLIDWORKS' own help says first angle is typically used in Europe and third angle in the United States. US drawings follow ASME Y14.3, Orthographic and Pictorial Views, whose current edition is Y14.3-2012, reaffirmed in 2024; US engineering-graphics textbooks teach third angle as the US method.
If you work for an Indian supplier to a US customer, expect both kinds of drawing. Always check the symbol before reading a single view.
One exception is easy to miss. For a symmetrical item, SP 46 allows a local view of a single feature, such as a keyway end, instead of a complete view. It says that local view should be drawn in third angle, whatever system the rest of the drawing uses.
Which line types are used in orthographic views?
A view uses different line types to tell the reader what each line is. A dashed line means an edge you cannot see, and a chain line means an axis, not an edge. SP 46 Table 6.8, which follows ISO 128, lists the line types for mechanical drawings. These are the ones used in the figures here:
| Line | Name in SP 46 / ISO 128 | Used for |
|---|---|---|
| Continuous wide | 01.2 | Visible edges and outlines |
| Dashed narrow | 02.1 | Hidden edges and outlines |
| Long-dashed dotted narrow | 04.1 | Centre lines, lines of symmetry, pitch circles of gears and holes |
| 04.1 with wide ends and wide changes of direction (04.2) | 04.1 + 04.2 | Cutting planes |
| Continuous narrow | 01.1 | Hatching, dimension, extension and projection lines, outlines of revolved sections |
| Continuous narrow freehand, or straight with zigzags | 01.1 | Limits of partial or interrupted views and local sections |
| Long-dashed double-dotted narrow | 05.1 | Adjacent parts, extreme positions of moving parts |
Wide and narrow lines come in pairs from a line group, and the wide line is always twice the narrow one. SP 46 prefers the 0.5 mm group (0.5 and 0.25 mm) and the 0.7 mm group (0.7 and 0.35 mm). Line widths are where CAD templates most often go wrong. If every line plots at the same width, the drawing loses the visual separation between outline and annotation.
What is an auxiliary view?
An auxiliary view looks square-on at a face that is inclined to the principal planes, so that face appears at its true shape and size. In the principal views a sloping face is foreshortened: a round hole in it looks like an ellipse, and its length looks shorter than it is. The auxiliary view is projected at right angles to the sloping edge instead.
In the example in the figure below, a block has a 45° face that is 42.4 mm long (30√2) and 30 mm deep, with a 12 mm hole drilled square to it.
- In the front view, that face is just an edge, and the hole walls are hidden lines.
- In the top view, the face would be drawn only 30 mm long (cos 45° = 0.707), and the hole would be an ellipse.
- The auxiliary view shows the 42.4 × 30 mm face, and the hole as a true circle you can dimension.
Usually only the inclined face is drawn in the auxiliary view, which makes it a partial auxiliary view; the rest would be distorted and add nothing. SOLIDWORKS describes an auxiliary view as "similar to a Projected View, but it is unfolded normal to a reference edge in an existing view". SP 46 handles any viewing direction outside the six principal ones with a reference arrow and a letter.
What is a sectional view?
A sectional view shows a part as if a plane had cut through it and the material between you and the plane had been taken away. Internal features then appear as visible edges, not hidden lines, and the solid material the plane cuts through is hatched.
Sections replace the clutter of dashed lines. In the bracket's front view, the hole and slot were four dashed lines. In section A-A they are clean gaps you can dimension.
The rules that make a section readable all come from SP 46 Section 10:
- Hatching uses continuous narrow lines, preferably at 45° to the main outlines. Every cut area of the same part gets identical hatching. Adjacent parts are hatched in different directions or at different spacings. Thin sections may be filled black, with at least 0.7 mm between adjacent ones.
- The cutting plane is drawn as a long-dashed dotted narrow line, thickened at its ends and wherever it changes direction. It carries capital letters and arrows for the viewing direction. When the plane's position is obvious, it need not be shown.
- Some features are never cut lengthwise. Ribs, fasteners, shafts and wheel spokes cut along their length are drawn unhatched, because hatching them would make a solid part look like a thin web, or a thin web look solid.
What are the types of sectional views?
There are seven common types: full, half, offset, aligned, broken-out (local), revolved and removed sections. They differ in the path the cutting plane takes and in where the section is drawn. Figure 5 shows each one on a simple part.
- Full section: one plane cuts right through the part, as in section A-A of the bracket (clause 10.2.5.1).
- Half section: for a symmetric part, one half is drawn as an outside view and the other half in section, divided by the centre line. You get the inside and the outside in one view (10.2.7).
- Offset section: the plane steps through two or more parallel planes to pass through features that are not in line, such as the three holes in figure 5. The section is drawn as if the cut were flat; the steps do not appear in it (10.2.5.2).
- Aligned section: for round parts, the plane is bent at the centre, and the inclined part is revolved into the plane of projection before it is drawn. Both holes then appear at their true radius (10.2.5.4).
- Broken-out (local) section: a small cut where a full or half section would be overkill, bounded by a continuous narrow freehand line or a zigzag line. The old version of this post called it a "cut-out view" (10.2.8).
- Revolved section: the cross-section of an arm, rib or spoke is turned 90° and drawn in place with continuous narrow lines (10.2.6.2).
- Removed section: the same cross-section moved clear of the view and drawn with continuous wide lines. It is either joined to the view by a chain line or placed elsewhere and labelled, for example B-B (10.2.6.3).
What are detail, broken and partial views?
These views do not show new directions. They make an existing view easier to read or fit on the sheet.
- Detail view (element on a larger scale): the area is framed with a continuous narrow line and identified by a capital letter. It is then redrawn at a stated larger scale with the same letter, such as "B (2:1)" (SP 46 clause 10.3.8). Use it for undercuts, grooves, small radii and thread runouts.
- Broken (interrupted) view: for a long part with a uniform middle, such as a shaft or a rail, only the portions needed to define it are drawn, placed close together. The break limits are drawn as for partial views (clause 10.3.6). The dimension still states the true length, 300 mm in the figure, even though the drawn length is shorter.
- Partial view: only the part of a view that adds information is drawn, cut off with a freehand or zigzag narrow line (clause 8B.3.9). A symmetric part may be drawn as a half or a quarter. The line of symmetry is then marked at each end with two short parallel narrow lines at right angles to it (clauses 10.3.5.1 and 10.3.5.2).
Isometric vs oblique vs perspective: what is the difference?
All three are pictorial views: they show the part in 3D in one picture. The difference is accuracy.
- Isometric keeps all three edge directions at the same scale.
- Oblique keeps the front face true and fakes the depth.
- Perspective looks most natural, but no edge is true length.
SP 46 recommends isometric, dimetric and oblique axonometry for technical drawings. It also says that hidden edges are best left out of pictorials, and that dimensions on them are normally avoided.
| Isometric | Oblique (cavalier / cabinet) | Perspective | |
|---|---|---|---|
| Projectors | Parallel, perpendicular to the picture plane | Parallel, at an angle to the picture plane | Converge to one point, the eye |
| Axes on paper | Vertical, plus two at 30° to the horizontal | Front face square-on, depth usually at 45° | 1, 2 or 3 vanishing points |
| Scale along the axes | Equal on all three (1:1:1 when drawn full size) | Cavalier 1:1:1; cabinet halves the depth | Shrinks with distance |
| Circles on faces | Ellipses on all three faces | True circles on the front face | Distorted ellipses |
| Typical use | Pictorials on working drawings and manuals | Quick sketches of parts with round front features | Industrial design and architecture renderings |
Why does an isometric drawing look bigger than the part?
In a true isometric projection, each of the three axes is tilted 35.26° to the picture plane. So every edge along an axis is foreshortened by the same factor:
The bracket's 80 mm base would therefore project as 65.3 mm, the 50 mm depth as 40.8 mm and the 60 mm height as 49.0 mm. Measuring with an "isometric scale" is tedious, so SP 46 notes that in practice the unit lengths are taken as 1. You simply draw every axis-parallel edge full size, which gives an isometric drawing enlarged by . The shape is identical, just 22.5% larger. That is how the figures here are drawn, and it is what the old version of this post meant by "same measure", the meaning of the Greek word isometric.
Circles turn into ellipses. In the isometric drawing of the bracket, the 14 mm hole on the base top becomes an ellipse 17.15 mm across its long axis and 9.90 mm across its short axis. The axis ratio is always . The figure script and the calculation file both reproduce those two numbers.
Dimetric and trimetric are the other axonometric views. Dimetric uses two equal scales and one different; SP 46 gives a dimetric with scales in the ratio 1/2 : 1 : 1. Trimetric uses three different scales and needs a separate scale for each axis, as the old version of this post noted.
Oblique views keep the front face true. In cavalier oblique the depth axis is drawn at 45° at full scale, which is easy to draw but makes deep parts look stretched. Cabinet oblique halves the depth scale, so the bracket's 50 mm depth is drawn 25 mm, and the proportions look much more natural.
Perspective (central projection) views are classified by how many sets of edges converge.
- One-point: a face is parallel to the picture plane, and only the depth lines converge.
- Two-point: the verticals stay vertical, and the horizontals run to two vanishing points on the horizon.
- Three-point: no edge is parallel to the picture plane.
An exploded view is a pictorial of an assembly. All its parts are drawn to the same scale and correctly oriented, but pulled apart along common axes in the order they go together. It is the standard way to show which part fits where, for example in a pulley support assembly or a service manual.
How do SolidWorks, CATIA and AutoCAD generate these views?
In 3D CAD you model the part once, place a base view, and derive every other view from it. The software projects the geometry, so the views always agree with each other. You still decide which views, sections and details the drawing needs, and you set the projection method.
| Task | SOLIDWORKS | CATIA V5 (Drafting) | AutoCAD (model documentation) |
|---|---|---|---|
| Principal views | Standard 3 View, Model View, Projected View | Front view, projection views, view creation wizard | VIEWBASE, then VIEWPROJ |
| First or third angle | Sheet Properties, "Type of projection" | Sheet Properties, "First angle standard" or "Third angle standard" | VIEWSTD, "Projection type" |
| Auxiliary view | Auxiliary View, unfolded normal to a selected edge | Auxiliary view | Not a separate command |
| Sections | Section View, Aligned Section View, Broken-out Section | Offset section view or cut, aligned section view or cut, breakout view | VIEWSECTION: Full, Half, Offset, Aligned, Object |
| Detail, broken and other views | Detail View, Break, Crop View, Alternate Position | Detail view, clipping view, broken view | VIEWDETAIL |
| Pictorial | Named isometric model view | Isometric view, exploded view | Base view in the model's current or a preset orientation |
| Keeping views up to date | Part, assembly and drawing are linked documents | View wizard links projected views to the main view | Associative views; VIEWUPDATE refreshes views made out of date by model changes |
A few cautions apply to all three tools:
- Check the template's projection setting. SOLIDWORKS' help says the "Type of projection" setting chooses first or third angle for the Standard 3 View. AutoCAD's VIEWSTD setting applies only to base views created after the change, and CATIA's help notes that the sheet style sets the starting projection method.
- Check the symbol in the title block against the layout of the views.
- Don't accept every hidden line the software draws. A drawing full of auto-generated dashes is usually a sign that a section view was needed.
Skill-Lync's tool hubs compare the courses that teach this drafting work: AutoCAD courses, SolidWorks courses and CATIA courses. For a walk-through, the CATIA V5 drafting guide generates front, section, detail and isometric views from a 3D model. Our beginner's guide to machine drawing covers the rest of a production drawing.
Views are only half of a working drawing; the other half is dimensions and tolerances. For a shaft and hole drawn with a fit such as H7/g6, the free Skill-Lync limits and fits calculator gives the ISO 286 limits of both parts and the resulting clearance or interference. To read geometric tolerances on the same views, see our guide to GD&T symbols.
Common mistakes when choosing and drawing views
- Mixing projection systems on one sheet, or drawing in one system while the symbol shows the other. The views still look plausible, which is why the error survives review.
- Too many views. If a view adds no feature that the others do not already define, delete it.
- Dimensioning to hidden lines. Section the part instead, so the feature becomes a visible edge.
- Hatching ribs, shafts or bolts that the cutting plane runs along.
- Using different hatching for two cut areas of the same part in one section, or the same hatching for two adjacent parts.
- Forgetting the scale on a detail view, or the designation letters on a removed section.
- A front view that is not the most informative view. For the bracket, the L-shaped face is the right choice; a front view looking at the 80 × 12 end would hide the L.
Frequently asked questions
How many views are needed in an engineering drawing?
As few as will define the part completely and without ambiguity. SP 46 and ISO 5456-2 allow up to six principal views, but most machined parts need two or three. A cylinder or washer may need only one view plus a diameter symbol, while a complex casting may need several views plus sections and details.
Is first angle or third angle projection used in India?
First angle. BIS's SP 46:2003, the drawing code for schools and colleges, makes first-angle projection the basic requirement for drawings prepared after 31 December 1991. Indian companies that make parts for American customers also receive third-angle drawings, so engineers need to read both.
How can I tell whether a drawing is in first or third angle?
Look at the symbol in the title block. If the circles are to the right of the cone, it is first angle; if they are to the left, it is third angle. With no symbol, check where the top view sits: below the front view means first angle, above means third angle.
What is the difference between a section view and a cut-out view?
A section view cuts through the whole part along a plane. A cut-out view, properly called a broken-out or local section, removes only a small region, bounded by a freehand or zigzag line, to expose one internal feature without sectioning the whole view.
Is an isometric view an orthographic projection?
Yes. A true isometric projection uses parallel lines of sight that are perpendicular to the picture plane, with the object tilted so its three axes make equal angles with that plane. What makes it different from orthographic views is that it shows all three dimensions in one view.
Do CAD tools draw first or third angle by default?
It depends on the template and the drafting standard. SOLIDWORKS and AutoCAD both let you choose first or third angle, in Sheet Properties and VIEWSTD respectively. Set it before placing views, because AutoCAD's setting does not change views that already exist.
Sources and further reading
- Bureau of Indian Standards. SP 46:2003, Engineering Drawing Practice for Schools and Colleges: notes on use (first angle after 31 Dec 1991), Section 6 (lines), Section 8 (projection methods), Section 10 (sections and conventions).
- Bureau of Indian Standards. IS 15021 (Part 2):2001 / ISO 5456-2:1996, Technical drawings: Projection methods, Part 2: Orthographic representations: view designations, first- and third-angle layouts, symbols and their proportions.
- Estonian Centre for Standardisation (EVS). ISO 128-3:2022, Views, sections and cuts: catalogue entry and scope; ISO 128-2:2020 record (replaced by ISO 128-2:2022).
- ASME. Y14.3-2012 (R2024), Orthographic and Pictorial Views.
- Corradi Dell'Acqua and Mohammadi, Illinois Institute of Technology. Orthographic projections, LibreTexts (CC BY 4.0).
- Bethune, J. D. "Orthographic Views", from Engineering Design and Graphics with SolidWorks 2016, Peachpit, 10 March 2017.
- Dassault Systèmes SOLIDWORKS Help: Views of Parts and Assemblies, Derived Drawing Views, Auxiliary View, Sheet Properties.
- Autodesk AutoCAD Help: Commands for working with model documentation drawing views, VIEWSECTION, Drafting Standard dialog box (VIEWSTD).
- Dassault Systèmes. CATIA V5 Generative Drafting User's Guide: View creation and Creating views via the wizard (copies hosted by City, University of London); About the projection methods (CATIA help).

