CAM toolpath basics in Fusion

00:04

In previous videos,

00:05

you learn how to create machining setups and looked

00:07

in depth at fusion's adaptive clearing roughing strategy.

00:10

In this tutorial,

00:11

let's delve into some of the basics of creating tool

00:14

paths to turn your designs in the machine components.

00:18

Fusion 360 organizes operations into five categories,

00:21

two D operations which contains operations aimed

00:24

at cutting parts with prismatic surfaces,

00:26

meaning parts with vertical and horizontal faces,

00:32

machining parts with more free form surfaces,

00:34

drilling which can be used to program holes from simple

00:37

to tapped to compound holes such as counter bores and countersinks

00:42

multi

00:42

axis operations that use more than three axis of your machine simultaneously.

00:47

Finally probing operations to ensure your

00:50

part is located properly on the machining

00:52

table and to verify your operations and the accuracy of your machine parts.

00:57

Notice that each operation has a tool tip when the cursor hovers over it,

01:00

giving more information about that strategy.

01:03

So it's easier to choose between them.

01:06

We'll start out with a simple two D facing operation like you saw in the last video.

01:10

But taking a closer look at the five tabs tool geometry

01:14

heights passes and linking

01:17

every tool path. In fusion.

01:23

Even as you make more and more complex tool paths,

01:27

I'll work through the tabs from left to right, starting with the tool tab. In

01:31

this case,

01:31

we're going to use a two inch face mill and I'll use the

01:34

filters at the top of the tool library to find it quickly.

01:37

When I select the tool,

01:38

the feeds and speeds are automatically updated based

01:40

on what was set in the tool library.

01:42

And I can fine tune them for this operation if desired.

01:46

The next tab is geometry where I'll make any necessary geometry selections. In

01:50

this case,

01:51

I don't need to make a selection as we want the tool path to go to the stock

01:55

extents which are automatically pulled in from the setup

01:57

shown as a yellow rectangle around the part.

01:60

The geometry tab also lets you define a tool orientation for positional multi

02:04

axis

02:05

which we cover at length in the positional multi axis course linked in the quarter.

02:09

Now

02:10

the heights tab limits the tool

02:11

pa and Z with top and bottom heights as

02:14

well as defines the clearance retract and feed heights

02:18

for this facing operation.

02:20

We want to remove the material from the top of the stock to the top of the model.

02:24

Any of the heights can be set relative to another height or

02:26

can be set using a selection directly from a model or sketch.

02:30

If you'd rather set the heights visually,

02:32

you can simply drag the heights into position

02:35

the passes tab defines how the tool goes

02:37

about removing material including parameters like step over,

02:40

step down.

02:41

And more that relates specifically to the selected strategy

02:44

for phrasing,

02:45

we can set a pass extension to extend the tool past the machining boundary.

02:50

The last tab contains the linking lead and transition options that

02:54

control how the tool enters exit and moves between cutting passes

02:58

at this point. We can press OK and view our tool path in the graphics window

03:03

we covered creating two D adaptive clearing for this part in the previous video.

03:08

So I'll skip ahead to machining the inside of the component.

03:12

Let's use another adaptive clearing and again, start by selecting a tool.

03:17

Next,

03:17

we can move on to the geometry tab and

03:19

first select the pocket contours using a model face.

03:23

Since we've already removed the material from the outside of the component,

03:26

I'm going to specify a stock contour,

03:28

stock contours define the outer limits of the tool path.

03:31

Ensuring we're not performing any unnecessary cutting

03:34

moves in optimizing our tool path.

03:36

It will also ensure that the material will be removed

03:38

across the top of the circular internal pocket regions.

03:41

Rust machining can be used to avoid cutting fresh air.

03:44

If we've already removed some material using a larger tool size,

03:49

we can now move to the heights tab and we can see

03:52

that the default bottom height is automatically set to the contour.

03:55

We have selected

03:56

as we face the top of the part, the top height can be set to the model top.

04:02

This time,

04:02

let's enable both ways to ensure we are both climb and conventional milling.

04:07

As this is a roughing tool path.

04:08

Let's specify stock to leave to cut with a finishing path. Later,

04:12

this can be defined both axially which is along

04:14

the tool axis and radially which is perpendicular.

04:18

Lastly, let's look at the linking tab.

04:20

Again,

04:21

we have a few options this time including the ability to set ramp

04:24

options that control the vertical transition between

04:27

different levels in the tool path.

04:29

I'm going to modify the retraction policy which controls how high

04:32

the tool will move before transitioning to other tool path sections

04:35

and the state on level which controls the

04:37

likelihood of the tool lifting between sections.

04:40

Remember hovering the mouse over the parameter provides more details

04:44

on what the parameter is and how it works.

04:46

At this point. We can take a look at the tool path.

04:52

I'm going to follow the same principles to program a few more operations to remove

04:56

the material from the inside of the component as well as finish the outer profile.

04:60

Remember the five tab system means each tool path is easy to understand,

05:04

allowing you to find the parameters you need to dial in each tool path.

05:09

Now it's time to program some drilled holes and

05:11

we'll see how drilling differs slightly from other milling operations

05:15

in the geometry tab.

05:16

You can select faces points or a diameter range to define the holes we want to cut.

05:21

I'm going to use faces and graphically select the

05:23

cylindrical surface that represents one of my holes.

05:27

I can then use the select same diameter option to also include

05:31

all the other holes in a model that are the same diameter

05:34

advanced options like boundaries, additional selection filters and ordering,

05:38

help you select and optimize your drilling operation quickly.

05:42

The heights tab looks familiar with the

05:44

added option of drill tip through bottom which

05:47

drive the shoulder of the tool to the bottom height rather than the tool tip.

05:51

The cycle tab is where you can change the type

05:53

of drilling cycle you want to use for these holes.

05:55

Each hole type is mapped to the machine

05:57

can cycle automatically by the post when possible,

06:00

ensuring safe material removal from the holes.

06:04

Again,

06:05

I'm going to use the same workflow to program

06:07

spot drill and tapping operations at this point.

06:10

Set up.

06:10

One is fully programmed so we can take a

06:12

look at a quick simulation to verify our programming.

06:15

As you can see, we are now ready to move on to set up two and continue programming.

06:19

Our part,

06:21

we have already programmed a facing operation for the second setup.

06:25

So I'm going to begin by creating a

06:26

roughing operation to remove the bulk of the material

06:29

due to the free form surfaces.

06:31

Let's use a 3D adaptive clearing which will be generated using the model surfaces.

06:35

Even though we are using a 3D tool path, we are still presented with the same five tabs

06:41

in the geometry tab. I'll select a stock contour to keep the toll pa

06:45

within the remaining material. Since the outside was roughed in a previous setup

06:50

for the heights,

06:51

we can use an edge from the model to define

06:53

the bottom of the tool path to prevent further duplicate machining

06:57

in the linking tab. I'm going to define the horizontal radius with an expression.

07:01

If you right click on any box,

07:03

you can choose to define the parameter using

07:06

an expression rather than specifying an exact number.

07:09

This expression can use a range of operation or tool variables.

07:12

And in this case, we can use 15% of the tool diameter.

07:16

This parameter will now update if I make a tool change,

07:19

meaning the tool path will parametric adapt to match my intent,

07:22

saving me downstream work.

07:23

If there are any changes.

07:26

Now let's take a look at some 3D, finishing operations,

07:30

finishing in fusion 360 is quick and intuitive since

07:33

containment can generally be selected directly off the model.

07:36

On this part,

07:37

we're going to take a look at two tricks when working with tool containment,

07:40

namely when there is a steep edge at the boundary that can cause a lot of noise

07:47

to start out.

07:47

I'll select the ball and mill and then

07:49

select the machining boundaries dynamically from the model

07:52

note that when a boundary is contained inside of another,

07:55

the tool path generates between these two boundaries,

07:58

we can now customize how the tool will behave when it reaches these boundaries.

08:03

First, we can set the tool containment to tool center,

08:06

which means the tool will be driven until the center

08:09

of the tool touches the boundaries we have already specified.

08:11

Don't forget we can use the tool tips to fully understand each parameter.

08:15

Now I'll check contact point boundary which drives the tool

08:19

contact point to the boundary rather than the tool center.

08:23

We're now going to use an option we haven't used so far avoid touch surfaces.

08:28

Since we have already finished the horizontal surface at the top of the model,

08:31

we can set this as an avoid surface with a clearance of zero

08:35

note that the touch surfaces checkbox allows us

08:37

to invert the meaning of avoid surface.

08:39

So the surfaces selected are targeted instead of avoided

08:44

in the passes tab,

08:45

I'll use an expression to drive the step over setting it to be 10% of the tool diameter

08:52

for the linking.

08:53

We can again change the retraction policy to minimum and

08:56

we're ready to take a look at our tool path.

08:57

As you can see,

08:58

we are getting some noise caused by the steep fall

09:01

up at the edge of the boundaries to solve this.

09:03

I'll edit the tool path by right clicking and selecting edit,

09:06

navigating to the geometry tab and setting an

09:08

additional offset equal to the negative tolerance.

09:13

This will keep fusion from looking over the

09:15

steep edge when it generates the tool bath,

09:16

reducing the noise.

09:18

And we are left with a much smoother tool path.

09:21

The last area of the model we need to program are the 3d champed

09:25

edges to do this.

09:26

We'll hijack another 3D operation scallop which creates passes at a constant

09:31

distance from one another by offsetting inwards along the underlying surfaces.

09:35

For this

09:36

cham,

09:36

let's use the same ball end mill we used

09:38

in the last tool path to minimize tool changes.

09:40

By searching the document to a library,

09:42

we can see the tools that have been used in other tool

09:45

paths and we can even look at which operations we use them in

09:50

for the geometry. I'll select the inner and outer edges of the model chamfer.

09:54

And once again specify that the tool path be

09:56

contained by the tools center at the boundaries.

09:58

Again,

09:59

we can set an offset equal to the negative

10:01

tolerance which will remove the noise at the boundaries.

10:05

We want to enable contact point boundary.

10:07

And this time we can specify a boundary overlap

10:10

of zero which will avoid any unnecessary cutting moves in

10:13

this passes tab. The step over can be set to 25 thou.

10:17

And the retraction policy in the linking tab

10:19

can once again be set to minimum retract.

10:23

Let's take a quick look at another stock simulation to make sure we're happy

10:26

with everything and there's no collisions and it looks like we're good to go.