Create a process plan

00:02

create a process plan.

00:05

After completing this video, you'll be able to

00:08

identify tools required, the machine apart,

00:10

identify tool pass required to machine apart and review a process plan

00:17

for this video.

00:17

We want to carry on with our three axis sample but also

00:20

take a look at a supplied process plan called process plan,

00:23

sample dash mill

00:25

and a process plan is a general plan that's used when setting up

00:30

a part while there is no predefined template for this in general,

00:34

it simply means that you're identifying geometry that needs to be machined,

00:38

thinking about the tool sizes required and then creating a plan

00:42

to put in place in order to machine that part.

00:45

There is not going to be a right or a wrong way to build a process

00:48

plan or to machine apart as long as the outcome is good and within tolerance.

00:54

So in this instance,

00:55

what we want to do is we want to explore a couple of

00:57

different tool paths for our part that are using three D strategies.

01:01

This is going to help us identify the time and place to

01:04

use certain tool paths and certain tools when machining our own parts.

01:08

But let's take a look at a sample process plan and then let's take

01:11

a look at our part and see how we can identify some of these tools

01:14

first inside the sample process plan, you'll notice a few things,

01:18

there is an operation number and type,

01:21

there's a setup number and then there are tools that are identified.

01:25

When we look at a process plan, we want to think about the tools that we need,

01:29

the tool numbers and how those are going to be inside of our tool changer

01:33

as well as any notes that we might want to add

01:35

often times you'll find that process plans are going to be

01:38

some form of documentation that will stay with the part.

01:42

In this instance we're going to be using a three D adaptive clearing

01:45

tool path to remove the majority of the material from our part.

01:49

So then we can focus on different three D

01:51

strategies to see how they apply to different areas.

01:54

We're going to explore a three D contour tool path and how it can

01:57

be used on different angles or slopes as well as different contained areas.

02:02

Then we're going to focus on a three D parallel strategy

02:04

and see how that works on curved and tapered faces.

02:08

And then we'll explore a three D flat strategy which

02:11

can identify flat areas on apart and machine them efficiently.

02:15

When we take a look at the second side, we have a lot more curvature to machine

02:19

but will again start with a three D adaptive clearing to efficiently remove

02:22

the material and then we'll explore spiral scallop and flow tool paths.

02:27

These are going to be various strategies that can be helpful on curved geometry.

02:32

When we look at our tools,

02:33

we can see that we're using a quarter inch end mill a quarter inch ball nose mill.

02:37

We also have a half inch ball nose mill.

02:40

These are going to be the only three tools that are required.

02:42

But of course you can substitute out your own tools

02:44

and sizes as long as you can access the geometry.

02:49

Next Let's take a look at the part Infusion 3 60.

02:53

As we take a look at the part, we want to identify tools that we need.

02:56

Some of the things that we should think about are going to be tool access or how far

03:00

the tool is sticking out of the holder as well as radi I that need to be machined.

03:05

So the first thing I want to do is take a look

03:07

at this section here which is going to have a square corner.

03:11

This means that we are going to be using a flat end mill or square end mill.

03:15

We also need to think about how far it needs to go down from this face.

03:20

In order to do that.

03:21

We're going to go to inspect and measure the overall height that the tool needs to go.

03:26

In this case you can see that it's giving us a straight line distance.

03:29

In order to get that height,

03:30

we're going to rotate around and focus on selecting these faces themselves.

03:35

This gives us an overall depth of .75",

03:38

meaning that we need to have a tool that can extend at least .75" out of the holder.

03:44

The next thing that we need to identify is the height here.

03:47

This is half inch,

03:48

which means that we need at least a half inch cutting

03:51

flute to get a clean cut on that side wall.

03:54

Well, this is very easy to get with a larger tool, such as a half inch end mill.

03:58

You might find that if you're using smaller tools like a quarter inch end mill,

04:01

that you might be running out of flute before you're able to cut this entire wall.

04:06

Some other areas that we should think about are going to

04:08

be things like affiliate in the root of this corner.

04:11

And if we take a look at measuring this film,

04:14

we can see that the radius value is 0.1 to six or the diameter 60.252.

04:19

This means it's just barely larger than a quarter inch tool,

04:23

which means that it will have no problem cutting that geometry

04:27

as we rotate over here,

04:29

you can see that this radius value is 0.26 or a diameter of 0.52.

04:34

This means that we can use a larger end mill in this case a half inch

04:38

ball end mill or a 3/8 ball end mill and have no problem cutting that geometry.

04:42

So these are the kinds of things that we should consider when

04:45

we're looking at a part and thinking about the tool diameter,

04:48

the geometry and how far it needs to stick out of a holder.

04:52

Some other things that we should also think about is how far down

04:55

the part we need to cut on the outside for this part.

04:58

Since we are using one by two stock,

05:01

we're not going to be machining the outside shape.

05:03

So all we need to be concerned with is the overall depth of these inside features.

05:08

There are geometry on the other side.

05:11

So if we hide our vice and take a look,

05:13

we want to make sure that we do rotate

05:14

the part around and identify these heights as well.

05:17

This is also a half inch.

05:19

If we go from this upper face here to the bottom of the bowl,

05:23

you can see that we're not really getting a good measurement here.

05:26

Sometimes it can be helpful for us to identify

05:29

the overall depth of this by referencing other features.

05:33

It looks like the bottom of this bowl is going to

05:36

be roughly the same height as this bottom face here.

05:39

So by just simply selecting this top face and this one,

05:42

we can see that it's three quarters of an inch.

05:44

If you're not sure,

05:46

then we need to take a sketch and section this

05:48

up to get a more accurate measurement or we can

05:51

use fusion 3 60 to calculate how far the tool

05:54

needs to stick out in order to reach that geometry.

05:56

Once we program our tool path

05:59

for now, let's go ahead and close this.

06:00

Let's bring back our vice and let's rotate this part around.

06:04

I'm gonna go back to a home view so I can see it from this angle.

06:10

So once again,

06:11

it's important to remember that a process plan is a general term that's

06:14

used to plan out how you're going to hold and machine apart.

06:19

In this case our part is going to be held in a vice in both operations

06:23

against some parallels.

06:25

The overall stock is one by two by six and the tools that

06:28

we're going to be using our quarter inch and half inch tools,

06:32

we need to make sure that we can machine at least a half inch with a flute

06:36

and have an overall extension or projection from

06:38

the holder of three quarters of an inch.

06:41

That gives us enough information to begin building out our tool library.

06:45

But before we do,

06:46

let's go ahead and minimize the component in the

06:48

browser and save the design before moving on.