Engineering drawings are the most important deliverables that a design engineer produces.
They provide all the instructions needed to make your parts exactly as you intended. But
bad drawings will make you look like a bad engineer, and parts made from them are sure
to have problems. In addition, many machine shops refuse to quote jobs that have bad drawings,
because nothing is more disruptive to them than having to call the engineer for missing
dimensions or clarification. In this video, we’re going to give you some tips for making
clear, complete drawings so you don’t embarrass yourself.
We’ve tried to make this video as painless as possible, so we’ve provided lots of extra
free resources on our website that cover the more tedious details. Our checklist will help
you ensure your drawings are complete, and this reference sheet shows some different
ways to dimension common features. We’ve also provided a fully-dimensioned drawing
package with both detail and assembly prints to serve as an example. And if you really
need to dive into the details, we’ve also provided references to the relevant ASME drafting
standards throughout the video.
These days, the vast majority of 2D drawings are made in the computer from a 3D parametric
CAD model. In this video, we’re going to be using Autodesk Inventor, but the information
we’re giving you applies to any software package, or even hand drafting. If you’re
new to CAD, Fusion 360 is free for hobbyists and startups and is a great option.
We’re going to be working to the drafting standards of the American Society for Mechanical
Engineers, which is the default in the United States and much of Canada and Mexico. In the
rest of the world, ISO standards are typically used. There are some minor differences between
the standards, but a lot of the fundamental concepts we’re covering in this video apply
to either system.
For the rest of this video, we’re going to use this brake caliper assembly as an example.
We’ll highlight some rules, best practices, and tips for both the detail and assembly
drawings, but we’re not going to show placing every dimension because that would make for
a very tedious video.
When making a drawing, you’ll usually start with a template, which is typically the same
for both detail and assembly prints. At the time of this video, the template that is built
into Fusion 360 is not compliant with the ASME drawing standards. We’ve made our own
standards-compliant template for Fusion 360 which you can download from our website.
The title block gives information about the company and people responsible for the design,
as well as the drawing name, number, and revision. It also specifies the sheet size and primary
scale, and you’ll want to choose these so that you have enough room to place all the
dimensions in each view.
Within the title block, there is also a list of blanket tolerances that apply when a dimension
is given on the face of the drawing without an explicit tolerance. A big problem we see
with drawings are title block tolerances that are unreasonably tight. In the format we’ve
provided, we’ve tried to choose tolerances that are reasonable for most modern CNC machines,
but you may want to increase these even more depending on the type of work you do.
The title block on subsequent sheets of the same drawing usually contains less information,
and is called a continuation title block.
The revision table shows when the drawing was changed, for what reason, and by whom.
The notes list provides information like the material and coating specifications, relevant
standards needed to interpret the drawing, special instructions for manufacturing certain
features, and other information that can’t be conveyed with a dimension.
The border defines zones with letters and numbers that allow you to identify specific
features with coordinates. This is really handy on a big drawing, because you can say
something like “change the .19 hole diameter in zone A7” and be able to jump right to
it, instead of having to scour the entire drawing to find something.
The face of the drawing will usually have two or more views, and they must have a particular
alignment to each other. We’re going to switch to hand drafting for a second to talk
about where this convention comes from.
To draw this example part, we’re going to choose a view to be our primary, or front
view. But, there’s other features of the part like the larger tapped holes and the
slot, that can’t be seen, so we need to create additional views around the front view
that show them.
To draw these projections, we have to imagine that we are rotating the part in space. If
you’re making drawings in the United States, you would rotate the part in this direction.
This is called third-angle.
To detail the other views, you’ll project the lines from your front view to define the
features.
You need to make it clear in the title block which convention you are using, and that’s
what the cone symbol is for.
3D CAD can create problems because it allows you to very easily break the alignment and
place a view wherever you want. You should really avoid this because the person reading
the drawing will use the orientation of the views to reconstruct the part in 3D, and breaking
the standard alignment makes this process much more confusing.
It's also great idea to drop an isometric view to help clarify things. Isometric views
don’t have to be strictly aligned to the orthographic views, but you should draw them
in the correct corner for the orientation you want to show. You can put notes in an
isometric, but you don’t put any dimensions since the features don’t appear in their
true size or shape.
You’ll usually want to show hidden lines to help depict the internal features of a
part. However, having a lot of hidden lines can sometimes add confusion, so you can omit
some lines for clarity. This is really a case-by-case thing, and your primary objective should be
to make the drawing as clear as possible.
The same is true of tangent lines. You will usually omit them in orthographic views, but
sometimes they are needed to make the view recognizable.
You should avoid dimensioning to hidden lines, so you will often need to create section views
to dimension internal features.
Smaller features often need to be shown at a larger scale, and detail views can help
you do this.
With your views arranged, you can start adding dimensions. When placing dimensions, you need
to fully define the size and position of every feature, and this is where new engineers typically
struggle the most, so be sure to check out the reference sheet on our website.
The general rule is that dimensions should be placed outside of the view. You are not
allowed to cross the dimension lines with either extension lines or leaders. Round features
and arcs greater than 180 degrees should be dimensioned according to their diameter, and
a diameter symbol will precede the dimension. Arcs less than 180 degrees, like fillets,
should be dimensioned by their radius, and the letter R should precede the dimension.
There are some feature you don’t have to explicitly dimension. If two edges meet at
a 90-degree angle, you don’t need to place an angle dimension. It’s just assumed to
be 90 degrees. Similarly, edges that appear to be tangent, like fillets, are assumed to
be tangent.
You cannot have multiple dimensions that conflict with each other. For example, this view of
the bore cap has an overall length dimension, as well as these dimensions that define the
thread length and flange thickness. These dimensions conflict and one of the three is
redundant. To minimize the tolerance stack, it’s best to dimension it with these two,
but having the overall length is helpful and we want to show it on the drawing. To resolve
the conflict, we can place parenthesis around the overall length, denoting it as a reference
dimension. This means it doesn’t control the part in any way, and is simply for informational
purposes. It can be very helpful to provide reference dimensions that show the overall
size of parts so you can easily see the size of stock needed to make it.
Threads are called out with a note that specifies the size, standard, and usually the tolerance
class. You can also specify the depth in the note or with a dimension in a view.
Many times, you’ll have multiple instances of the same feature like these fillets. You
can use a note like 2X to indicate this, or multiple leaders. Sometimes people will put
TYP for “typical” but you should avoid doing this because it can be extremely confusing
when there are multiple features that look similar, but are really different.
Critical features in your drawing will often require tighter tolerances than what is stated
in the title block. A lot of times, the tolerances will be provided to you by somebody else.
For example, this hole holds a special type of hydraulic plug from the Lee Company. Their
technical references call out the dimensions and tolerances and we can just copy that onto
our drawing.
In an earlier video, we talked about how to use design tables to set the tolerances for
the fit you need between components. For more complicated interfaces you can use a technique
called geometric dimensioning and tolerancing. GD&T is fairly complicated, and we’re going
to have to make multiple videos just to cover all the nuances, but until then, here’s
the elevator pitch. GD&T gives you a way to describe the functional requirements of features
by controlling things like flatness, perpendicularity, position, and runout. When using GD&T to control
a feature, the locating dimensions are typically enclosed with a box to indicate that they
are “basic” or “theoretically exact”. The feature is controlled by a special note
called a feature control frame, which may also reference other features as “datums.”
If it sounds complicated now, don’t worry, because we’re going to break it all down
into much simpler terms in future videos.
The important thing we want to emphasize is that there is a systematic way to calculate
what every single tolerance should be to achieve the intended functionality. It’s terrible
practice to put an arbitrarily tight tolerance on a dimension just because you think it’s
a critical feature.
You will often need to specify surface finishes in locations where you have a seal. There
is a special symbol to do this. The number indicates the root-mean-square height of the
surface in micro-inches, and this is inspected with a special type of instrument called a
profilometer.
Notes are critically important for clarifying the drawing and fully defining the part. A
lot of engineers try to abbreviate and shorten notes to the point that they become cryptic
and confusing. Just use succinct, plain language and make sure you are conveying all the information
you need to.
A lot of notes will apply to the entire part or drawing. For example, you can use notes
to specify things like materials or coatings. When listing a material, it’s critical to
specify the alloy, heat treat, and material specification. Just saying something like
“316L Stainless” is not enough because this particular stainless alloy can be made
for normal industrial applications, or in ultra-high purity and cleanliness for pharmaceutical
and biomedical applications. You need to list a specification to clarify which version you
need.
You should not use notes to specify things like quantity, delivery date, or payment terms.
This information will be listed in the request for quote and purchase order.
Other notes will only apply to a specific feature. These are often called “flag notes”
because a little flag symbol is sometimes used.
You typically don’t want to have sharp edges on any finished part because it presents a
safety concern and burrs can interfere with components fitting together. If all you want
is an edge break, best practice is not to model or dimension small chamfers or fillets.
Instead, you can use a general note asking the manufacturer to remove burrs and sharp
edges, and perhaps supply a loose range for the size of the edge break. If you use a note
like this, you’ve given them the option to deburr on the machine, using a hand tool,
grinder, bead blast, or vibratory finishing machine. But if you place dimensions in a
view to specify the edge break, you’ve pretty much forced them to machine it, and it becomes
a feature that is held to a tolerance and must be inspected.
Assembly drawings are critical for showing how complicated assemblies go together. Enough
views should be chosen to clearly show every component. Parts are often identified with
a find number in a bubble. A parts list on the face of the drawing indicates the corresponding
part number, description, and quantity required of each find number. Notes can be used to
provide information like torque specifications or testing requirements. You may also want
to include some reference dimensions for mounting features.
We’ve given a lot of little details in this video, but we want to emphasize that your
primary objective is to make drawings that are totally clear. We’ve posted a checklist
to our website to help when reviewing a CAD drawing, but you should always do a final
check by asking yourself “can a total stranger that knows nothing about my company or product
look at this drawing and make exactly what I want without needing to call me?”
A lot of new engineers really struggle with making drawings, especially because most universities
do an awful job teaching the concept. With this video, we’ve tried to start you in
the right direction, but ultimately, the only way to get better is practice. If you work
at a company, your drawings will almost always be checked by an experienced designer or engineer,
and that feedback is critical to improving your skills.
We have more engineering videos coming soon, so be sure to subscribe so you don’t miss
them. Thanks for watching!