Review detailed drawings

00:02

review detailed drawings.

00:05

After completing this video, you'll be able to

00:07

identify and explain G. D. And T.

00:09

Symbols, identify required tool, type size and projections,

00:13

identify required surface finish and identify tolerance, controlled features.

00:19

To get started,

00:20

we want to take a look at the supplied

00:22

drawing dual fixture plate dash 1001 drawing dot pdf.

00:27

We want to make sure that we can identify critical details

00:30

and information from a detailed drawing before we plan manufacturing.

00:34

So as we take a look at this detailed drawing,

00:36

we're going to be focusing on a handful of different areas and make sure that

00:39

we understand what some of the notes and symbols are on a detailed drawing.

00:44

The first thing that we want to identify is

00:45

going to be information in the title block.

00:48

Typically a title block will contain information such as

00:52

tolerances if they're not specified in the detailed drawings,

00:55

annotations anywhere.

00:57

Information about the project, potentially the title

00:60

as well as things like materials.

01:03

Any of this information is missing from a detailed drawing.

01:06

It's important that you go back to the source that supply the detailed

01:09

drawing and make sure that you clarify any areas that are unclear.

01:13

In this case.

01:14

For example, the detailed drawing does not contain information about the material

01:19

and it really should have that information.

01:21

So this would be a case where you'd go

01:23

back to the original person that sent the detailed drawing

01:26

and make sure that you validate the material used and

01:28

get it in writing what material will be manufactured.

01:32

The next thing that we want to take a look at is the overall size of our part.

01:36

As we take a look at this part, there are a handful of different views

01:40

notice this view in the bottom left has an overall dimension of 4.5 inches.

01:45

But this view here doesn't specifically call out the overall height.

01:49

We have to go to another view which shows that

01:51

it's two inches wide and half an inch tall.

01:55

So this tells us that the overall stock size is two by 4.5 by half inch thick.

02:01

We need to look at this information and determine

02:03

how much material we need to start with.

02:05

In order to get our final shape.

02:08

In this case we would need a little bit more material in all

02:11

directions to make sure that we can machine down to the final size.

02:15

The next thing that we want to do is make sure

02:17

that we can identify the differences between dimensions that are displayed.

02:21

For example, 4.5 inches is a linear dimension.

02:25

This is representing a distance between two edges or points on our part.

02:31

You can see that this 0.25 dimension is also a linear dimension.

02:35

However,

02:35

it's displayed in a different manner simply because

02:38

the dimension cannot fit within the leader lines,

02:41

we can see on the far right hand side.

02:43

The half inch dimension is displayed in a different manner as well,

02:46

but it's still a linear dimension.

02:48

So even though the dimensions are displayed in a slightly different manner,

02:52

they are still linear dimensions representing the distance between two edges.

02:56

In most of these cases.

02:58

Oftentimes you'll see dimensions listed to represent angles between faces or

03:03

edges or also to represent things like the radius value as

03:07

denoted by R in front of this dimension or a diameter

03:10

as denoted by this diameter symbol in front of the .201.

03:15

When we look at this, you'll also note that this specific drawing

03:18

calls out the hole diameter in one instance

03:22

as well as quarter 20 through times eight. In another instance.

03:27

In most cases when you have a hole that contains threads,

03:30

you'll see a thread note and you'll need to look at a drill tap chart

03:34

to determine what size hole needs to be drilled or measure it on the detailed part

03:39

as we see here.

03:40

This has eight times eight,

03:41

which means that all eight of these holes are going to be the same size

03:46

as we take a look around this detailed drawing,

03:48

there are also a couple of different annotations

03:51

we can see here, there's a note with a leader line that says break edge.

03:55

Typically these are placed whenever you want to make sure

03:57

that you d bir the edges on a part.

04:00

In most cases you'll have a note that says break all

04:03

edges or it will represent a very specific champ for size.

04:07

We can also see other notes such as this section a scale one half

04:12

this is representing the section line or the section view as denoted by A and A.

04:18

On this top down view.

04:20

You can also see other areas where there are symbols, notes and annotations.

04:25

For example, we can see that we have a box with an A. In it.

04:29

We have a box with a B and we have a box with a seat.

04:32

These are going to be diatoms.

04:35

Diatoms will represent a specific location on a part.

04:38

Typically they'll be representing an edge or a face.

04:42

In this case you can see that A is pointing to the bottom face of our part.

04:47

Next you can see that we have what's called a

04:49

feature control frame listed at the top of our part.

04:53

The feature control frame contains different kinds

04:56

of information depending on what you're referencing

04:59

in this instance we have a symbol that represents parallelism and

05:03

then we have a tolerance of .01 and then we've got the

05:07

reference data of a so this is telling us this top

05:10

face needs to be parallel within .01 reference to the data.

05:17

A.

05:18

As we look at other day Tums and control frames in this part,

05:21

you can see here that we've got a different symbol,

05:24

a different tolerance and two datum reference.

05:27

We can see here that we have a position reference for this whole

05:32

with a tolerance of 20.2

05:35

in relation to both B and C.

05:38

This means that the distance 0.38

05:41

needs to be plus or minus 0.2. As it references B.

05:47

Also the distance from C. Which is 3.5 inches

05:51

as plus or minus 0.2.

05:54

So these feature control frames are going to

05:56

be an important aspect of a detailed drawing

05:58

and will help you identify what sort of

06:01

tolerance values or potentially some geometric tolerance NG.

06:05

That needs to happen on certain features.

06:08

There are other G. D. And T.

06:10

Or geometric dimension NG intolerance NG symbols and

06:12

you should make sure that you do study

06:14

them to ensure that you are up to date on at least most common symbols.

06:19

Let's take a look at the last note that we have on this detailed drawing.

06:23

This is what's called a surface finish note.

06:26

The surface finish note can be displayed in different ways depending on the options

06:30

selected and depending on the type of standard the drawing is being created to.

06:36

In this case we can see that we have a few things.

06:39

We see the word mill at the very top of this surface finish symbol.

06:44

This is going to represent that this part needs to be milled.

06:48

You can also see that we've got some tolerance values .001

06:52

and .0001 below it.

06:55

These are going to be the minimum and maximum surface roughness values.

07:00

The .05 located underneath mill. This is going to be this sample length.

07:06

This determines how long of a sample size You need to take on

07:10

your part to make sure that you're within those men and max values

07:14

the triangle shape at the very bottom is representing material removal required.

07:20

So once again the surface finish has multiple options,

07:23

different tolerances and different types of prep that can be determined

07:28

simply by looking at the symbol in which options were used

07:31

when planning to manufacture apart.

07:33

It's also important that we identify critical areas

07:37

such as the overall height of apart and features

07:40

as well as things like radius values.

07:42

This will help us determine the size of tool that needs to be used.

07:46

As we take a look at this,

07:47

we can see that we've got tapped holes so we know

07:50

that we're going to have to spot drill the holes.

07:52

We're gonna have to drill them with a 0.201 drill or an

07:55

F drill and we have to tap them with a quarter 20.

07:59

Those are three separate tools that we know will be required to machine this part.

08:03

The overall part can be machined with a square end mill.

08:07

All of the internal edges are going to have square bottoms on them,

08:12

which means that we don't need a rounded or ball nose mill

08:15

or one that has a slight radius such as a bull nose mill

08:19

but we still need to determine the size and projection

08:22

or the amount the tool sticks out of our holder.

08:24

As we take a look at these radius values,

08:26

you can see that we have a quarter inch radius,

08:28

which means that we have a half inch diameter.

08:31

This tells us that a half inch diameter tool

08:34

can fit inside of here and machine the part.

08:36

However,

08:37

it's always important to note that an exact match

08:40

of the radius value of our tool and an internal

08:43

typically can cause chatter,

08:45

which means that you'll have a reduced quality

08:48

on your surface finish in those areas.

08:50

For that reason,

08:51

we want to make sure that the diameter of our tool

08:53

is slightly smaller than the radius and diameter of that corner.

08:58

This means that we'd likely want to use a

09:03

As we look at other views, we can see the overall height of our part is half inch.

09:07

The stock that we're going to be using is going to be taller than half inch.

09:11

So we need to make sure that the tool that we're using has at least a three

09:15

quarter inch flute length that can be used to rough the entire part and raw stock.

09:20

We also need to make sure that it is sticking out of the holder at least that far.

09:25

So these are all things that we can gather just

09:27

by looking at some basic dimensions on a detailed drawing.

09:30

It's always important to evaluate the part itself as well as you can get better

09:35

information directly off the part that you'll be using to program your tool paths.

09:39

But for right now we have a good understanding of

09:42

what the dimensions and symbols mean on this drawing,

09:44

we know the overall size of our part,

09:46

and we have a good idea on a handful of

09:48

tools that are going to be required to machine it.

09:51

So once you're done, reviewing this detailed drawing,

09:53

go ahead and move on to the next step.