Create 2.5 axis toolpaths

00:02

Create 2.5 access tool paths.

00:05

After completing this video, you'll be able to

00:08

create a drilling operation, create a 2.5 axis roughing tool path

00:11

and create 2.5 axis finishing tool baths.

00:16

To get started in fusion, we want to begin with the supply data set. CM two X tool

00:21

pass mm dot F 3D.

00:23

When we open this design up,

00:24

it should automatically be in the manufacture workspace.

00:27

But if not ensure that you do navigate there

00:29

and double check the units are set to metric.

00:32

This design already contains a setup,

00:34

the setup has the stock set and the coordinate system in the correct location.

00:38

The design also contains tools inside of its document.

00:41

You can take a look at the very top in the document for C AM two X tool paths.

00:45

There are tools and if we clear our filters,

00:49

we can see that tools will be available for

00:51

our milling operations as well as our drilling operations.

00:55

So now that we know that we have tools and our set up,

00:58

let's go ahead and get started creating our tool paths.

01:01

There are a couple of main objectives when we're machining apart,

01:04

first,

01:05

we want to remove as much material as possible as

01:08

quickly as possible in what are called roughing operations.

01:11

And then we wanna create finishing operations that will get down to the

01:15

final shape and size of our part and leave a good surface finish.

01:18

Now, there are some general approaches to this for nearly all parts.

01:22

So we're gonna take a look at that with this part here

01:25

to get started. The first operation we want to do is create a facing tool path.

01:29

When we take a look at this thing from the front view,

01:31

we can see that there's stock above the top of our part

01:34

and there's plenty of stock below the bottom of our part.

01:37

For this example, we're not going to be discussing holding it in a vice or a fixture.

01:42

We're just going to assume that we've got plenty of space below the bottom of our part

01:46

and we're holding it inside of some sort of work holding

01:49

that we need to make sure that we don't go all the way to the bottom of our stock.

01:53

We'll talk more about vices and fixtures in some of the three Xs tool paths.

01:58

So from here, we want to face the top of our part

02:01

back in a home view, we're going to go to our two D drop down and select two D face

02:06

from here. We need to select a tool.

02:09

There are only certain types of tools

02:10

that will be applicable for facing operations.

02:13

Our flat end mill as well as a larger face mill would be a good choice

02:17

because we're working on a limited set of tools.

02:19

We're going to be using our 12 millimeter flat end mill or tool. Number one,

02:24

we're gonna be using aluminum finishing for our cutting data.

02:27

This is because a facing tool path does remove raw

02:30

or rough stock from the outside of our part.

02:32

But the surface that it cuts down to will be the final top surface of our part,

02:36

we'll select the tool and that cutting preset.

02:39

Noting that in the feeds and speeds section, those values are now populated

02:43

from here. We're gonna move on to our geometry section

02:46

and with a facing tool path, it automatically gets the outside profile of our stock.

02:51

So we see an orange border on the screen and this tells us that no selection is needed.

02:56

Next in our height section,

02:58

we've got various planes that are gonna dictate what happens with the tool.

03:02

And when

03:03

we have a clearance plane at the very top, followed by a retract plane,

03:07

our feet height plane, the top height and the bottom height.

03:11

By default, with a facing tool path,

03:13

the top height will be the top of our stock

03:15

and the bottom height will be the top of our model

03:18

because of this, we don't need to make any changes or selections.

03:22

But as you begin machining more and more.

03:24

You'll find that reducing the height between things like our clearance plane,

03:28

retract plane and the feed height can drastically speed up the programs.

03:33

What I mean by this is there are different speeds at which the tool is gonna travel,

03:37

the rapid movements and the feed movements

03:39

changing where those happen can really speed up the machining process.

03:43

Reducing the amount of time you're spending, not cutting material.

03:47

Next, we're gonna move over to our passes section

03:50

in the passes section.

03:51

We've got a couple of options, but we're not going to change too much here.

03:54

First note that we've got our pass direction reference.

03:58

This is gonna allow us to change which direction the tool is going by default,

04:02

it'll be going along the X and Y directions.

04:05

Also as we go down, you can see that we've got a pass extension.

04:09

This is gonna be half of our tool or the radius value of our tool.

04:13

This means that the tool is going to extend past

04:15

the end of our stock before it turns around.

04:18

There's also a step over value and in this case, 1.7 millimeters is relatively low.

04:23

I'm gonna set this just shy of the diameter of our tool at 11 millimeters.

04:29

Next, we have a direction reference by default, it's gonna go both ways.

04:33

But if you have a specific machining direction, for example,

04:36

climb or conventional, you can change those.

04:38

Here.

04:39

There is a new option called order for shorter links that can reduce

04:43

the amount of time it takes to machine or face our part.

04:46

However, order for shorter links only works.

04:48

If you change your direction to a specific climb or conventional direction,

04:52

it won't work with the both option.

04:55

There's also a from other side and use chip

04:57

thinning which we're going to omit for right now.

05:00

And in the linking section,

05:01

this is gonna dictate how the tool moves into and out of our cuts.

05:05

And we're gonna leave these as default for now and say, OK,

05:08

once done, we'll get a preview on the screen,

05:10

showing us a green preview of the stock as well as

05:14

the lines that the tool is going to be traveling.

05:16

If we go back to our front view,

05:17

we can now see that the stock is cut down to the top of our part.

05:21

This is done showing us in process stock and

05:24

the visibility can be changed by going down to this

05:26

bottom section in fusion and turning on or off the

05:29

in process stock or by going to our tool,

05:32

visibility

05:32

going on and off for the tool.

05:35

And we can also turn on and off our tool paths.

05:39

This can help especially once we get into more complex

05:41

tool paths that have much more movements on the screen.

05:44

But for right now, we're gonna leave them as is.

05:46

So anytime we click on our facing tool path, we'll get a preview

05:50

now that we face the top of our part,

05:52

we're going to move on to doing some roughing operations

05:55

in the two D tools.

05:56

We've got a two D adaptive clearing,

05:58

which is a wonderful option for nearly all types of parts.

06:02

There are other options such as two D pocket for clearing.

06:05

But the two D adaptive is going to allow us to cut

06:07

a little bit deeper and keep a consistent load on our tool.

06:10

We're going to select two D adaptive clearing.

06:13

We're gonna be using the same tool moving on to our geometry selection

06:17

and we're going to select the bottom outside edge of our part.

06:20

There'll be a blue preview on the screen and this is gonna

06:23

let us know which side of the part is gonna be cut.

06:26

You also note that this goes out to the size of our stock,

06:29

so no other selections are needed.

06:31

Next, we're gonna go to our height section at

06:34

this point.

06:35

All of the heights are going to be ok because

06:37

the bottom height is based on our selected contour.

06:39

However, a two D adaptive tool path is a roughing tool path,

06:44

which means it's intended to leave stock behind.

06:47

And that's gonna not allow us to cut all the way down to the bottom of our part.

06:50

So if we view this from a front view again,

06:52

and we go down to our bottom height and the selected contours

06:55

and we add, say two millimeters

06:58

that's going to allow the tool to go two

06:59

millimeters relative to the bottom of our part.

07:02

However, the positive value is in the positive Z direction.

07:06

Because of the coordinate system, we need to use a negative value.

07:09

If we make this change, all we need to do is edit our tool path,

07:13

go to our height section

07:14

and change the offset value to minus two millimeters and say, OK.

07:19

Now the preview on the screen shows the tool path

07:21

cutting two millimeters below the bottom of our part.

07:24

Let's go ahead and take one quick look at the rest of the settings.

07:27

Before we move on to the next tool path.

07:30

In the passive section,

07:31

we have some values in here such as optimal load that are going to determine

07:35

how much engagement we have between our tool and the material that it's cutting.

07:39

We have a default stock to leave.

07:41

In this case,

07:42

it's half a millimeter in the radial direction and the axial direction.

07:46

This means on the side of the tool and on the bottom of the tool.

07:49

Next, we also have a multiple depths option.

07:52

In this case, our tool can make this cut with a single depth.

07:55

But if we had to cut extremely deep into a part, we may need to toggle that on.

08:00

The next option here is multi

08:02

axis which we're not taking a look at. And the last one is linking

08:05

by default, it'll do a helo

08:07

entry and we're gonna leave all of these values as default and say, OK,

08:12

back in a home view,

08:13

we can now see that we've cleared the material around the outside

08:15

of our part all the way to two millimeters below the part

08:19

minus that extra half a millimeter that it's leaving for a stock to leave.

08:23

Now, we want to remove the material from this phase.

08:26

We can do this in a single operation,

08:28

but it's good practice to go back and do this a couple of different times.

08:31

So we're going to use the same process using a two D adaptive clearing.

08:35

Note that when we're using two D adaptive clearing,

08:38

there is a rest machining option.

08:40

However, with two D tool pass,

08:41

rest machining is really taking a look at a previously

08:45

sized tool and the material that would be left behind

08:48

when we get into 3D tool pass,

08:49

those are model aware and they make better use of

08:52

the material that was left behind from previous operations.

08:55

So for us,

08:56

we're gonna use a closed chain selection and not worry about rest machining

09:01

next.

09:01

In the height section,

09:02

we need to be careful here because we are gonna

09:05

be leaving stock and we can't have a bottom height offset

09:08

because the bottom of the tool is hitting stock,

09:11

we need to make sure that it's stopping at that area.

09:14

And in our passive section, we're leaving a half a millimeter of stock.

09:18

So for this tool path, we're gonna say, OK,

09:21

now that we've got our roughed material,

09:23

we need to go back and finish it and this can

09:25

generally be done with a couple of different tool paths.

09:28

For our part. It's gonna make the most amount of sense to use a two D contour.

09:32

Once again, we're gonna do this in two separate operations.

09:36

We're gonna select our tool.

09:37

We're gonna move to our geometry and select this bottom edge for our contour.

09:41

We're gonna move to our passes, make sure that we're not leaving any stock.

09:45

And we're gonna say, OK,

09:47

because of the size of our tool and the size of material that we need to remove,

09:51

we can do this in a single pass.

09:53

The reason we didn't do the bottom edge at the same time is

09:56

because the bottom edge needs to be cut a little bit lower.

09:59

So we're gonna do a two D contour one more time

10:02

this time selecting our bottom edge.

10:04

But inside of our passes section, we need to make sure that we are not leaving stock.

10:08

And in our height section, we need to make sure that we're using a negative offset.

10:13

When we did our two D adaptive, we had negative two millimeters.

10:16

However, that left half a millimeter of stock behind.

10:20

If we do this, it's going to engage too much stock at the bottom of our cut.

10:24

So we're gonna use minus 1.5 millimeters and say, OK,

10:28

this should get us down to the exact same height as our two D adaptive clearing.

10:33

Now that all of the outside of our part has been machined.

10:36

The last thing that we need to do is take care of the holes,

10:38

the holes are taken care of with drilling operations.

10:42

We're gonna start the drilling operations by using a spot drill.

10:45

This is gonna be tool number two in our tool library.

10:48

And we're gonna select aluminum drilling.

10:51

Then for our geometry, we're gonna select the insides of each of these holes.

10:56

By default. Fusion wants to drill all the way to the bottom of the hole.

10:59

This is a problem because we're using a spot drill and we

11:02

only need to start the hole so that it centers our drill.

11:05

So from our height section,

11:07

the very bottom, we're gonna change the from

11:09

to be the top of our hole.

11:12

And we're going to use the drill tip through bottom and say, OK,

11:15

this is gonna leave a small indent at the center of

11:18

each hole that allows the larger drill bit to be centered.

11:22

Next.

11:22

We're gonna do another drilling operation once again,

11:25

selecting each of these center holes.

11:26

However, this time we're gonna use the final size drill bit.

11:29

It's gonna be tool number three, a six millimeter drill.

11:32

And we'll select aluminum drilling for our preset.

11:35

We're going to go to our geometry selection, select each hole

11:39

and in our height section from our front view,

11:42

we want to make sure that we're drilling through the bottom.

11:45

And in this case, we've got two values,

11:47

we've got an offset value and a breakthrough depth,

11:50

the offset value is going to be based on our Z coordinate orientation.

11:54

This means that we need a negative value to go

11:56

further down and a positive value to go further up.

11:59

However, with the breakthrough depth,

12:01

if we use a positive value of two millimeters,

12:03

this is going to extend beyond the bottom of our part.

12:06

There is one more thing that we need to change and that's gonna be the drilling cycle.

12:11

This is gonna be a canned cycle that gets called inside of our coat.

12:14

Typically, when we're doing a spot drill,

12:17

the drill bit can come down spot the hole relatively quick and retract away.

12:21

However, when we're actually drilling in the material,

12:24

we want to use something like a chip breaking cycle.

12:27

This allows the drill bit to go in a small amount and

12:29

either pause or retract to allow the hole to clear the chips

12:33

and allow coolant to get into that hole.

12:35

This is especially important when we're drilling deep holes to ensure

12:38

that the quality and the diameter of the hole are consistent.

12:42

We're gonna say, OK, and we'll go back to our home view

12:46

at this point, everything looks ok.

12:48

However, the drill bit size is too small for the size of our hole.

12:52

If we use our inspect measure tool and we measure this hole,

12:55

we can see that it's currently at a diameter of eight millimeters.

12:59

We've already created our tool path with a six millimeter drill.

13:03

And if we expand this, you can see that tool number three is a six millimeter drill.

13:07

If we right click, we are able to edit the tool.

13:10

This means that we can go in and modify its parameters.

13:13

You should only do this if you have direct control

13:16

over which tools you have available on your machine.

13:18

In

13:19

this case, I'm gonna just simply change the diameter to eight millimeters

13:22

except

13:23

and now it tells me that this tool path is out of date

13:26

to fix this. All we need to do is go to actions and select generate.

13:31

It's gonna redo the tool path with the updated tool diameter,

13:34

our eight millimeter drill.

13:36

And now we can see the preview on the screen shows

13:38

that the holes are being drilled to the correct size.

13:41

Now, at this point, we've created our facing tool path,

13:44

our two D adaptive tool path to rough the stock

13:47

and our two D contours to finish the outside shape.

13:50

Then we went back with a spot drill to start

13:52

the holes and a drill bit to finish the holes.

13:55

So at this point,

13:56

let's go ahead and make sure that we save everything

13:58

we've done before we move on to the next step.

Video transcript

00:02

Create 2.5 access tool paths.

00:05

After completing this video, you'll be able to

00:08

create a drilling operation, create a 2.5 axis roughing tool path

00:11

and create 2.5 axis finishing tool baths.

00:16

To get started in fusion, we want to begin with the supply data set. CM two X tool

00:21

pass mm dot F 3D.

00:23

When we open this design up,

00:24

it should automatically be in the manufacture workspace.

00:27

But if not ensure that you do navigate there

00:29

and double check the units are set to metric.

00:32

This design already contains a setup,

00:34

the setup has the stock set and the coordinate system in the correct location.

00:38

The design also contains tools inside of its document.

00:41

You can take a look at the very top in the document for C AM two X tool paths.

00:45

There are tools and if we clear our filters,

00:49

we can see that tools will be available for

00:51

our milling operations as well as our drilling operations.

00:55

So now that we know that we have tools and our set up,

00:58

let's go ahead and get started creating our tool paths.

01:01

There are a couple of main objectives when we're machining apart,

01:04

first,

01:05

we want to remove as much material as possible as

01:08

quickly as possible in what are called roughing operations.

01:11

And then we wanna create finishing operations that will get down to the

01:15

final shape and size of our part and leave a good surface finish.

01:18

Now, there are some general approaches to this for nearly all parts.

01:22

So we're gonna take a look at that with this part here

01:25

to get started. The first operation we want to do is create a facing tool path.

01:29

When we take a look at this thing from the front view,

01:31

we can see that there's stock above the top of our part

01:34

and there's plenty of stock below the bottom of our part.

01:37

For this example, we're not going to be discussing holding it in a vice or a fixture.

01:42

We're just going to assume that we've got plenty of space below the bottom of our part

01:46

and we're holding it inside of some sort of work holding

01:49

that we need to make sure that we don't go all the way to the bottom of our stock.

01:53

We'll talk more about vices and fixtures in some of the three Xs tool paths.

01:58

So from here, we want to face the top of our part

02:01

back in a home view, we're going to go to our two D drop down and select two D face

02:06

from here. We need to select a tool.

02:09

There are only certain types of tools

02:10

that will be applicable for facing operations.

02:13

Our flat end mill as well as a larger face mill would be a good choice

02:17

because we're working on a limited set of tools.

02:19

We're going to be using our 12 millimeter flat end mill or tool. Number one,

02:24

we're gonna be using aluminum finishing for our cutting data.

02:27

This is because a facing tool path does remove raw

02:30

or rough stock from the outside of our part.

02:32

But the surface that it cuts down to will be the final top surface of our part,

02:36

we'll select the tool and that cutting preset.

02:39

Noting that in the feeds and speeds section, those values are now populated

02:43

from here. We're gonna move on to our geometry section

02:46

and with a facing tool path, it automatically gets the outside profile of our stock.

02:51

So we see an orange border on the screen and this tells us that no selection is needed.

02:56

Next in our height section,

02:58

we've got various planes that are gonna dictate what happens with the tool.

03:02

And when

03:03

we have a clearance plane at the very top, followed by a retract plane,

03:07

our feet height plane, the top height and the bottom height.

03:11

By default, with a facing tool path,

03:13

the top height will be the top of our stock

03:15

and the bottom height will be the top of our model

03:18

because of this, we don't need to make any changes or selections.

03:22

But as you begin machining more and more.

03:24

You'll find that reducing the height between things like our clearance plane,

03:28

retract plane and the feed height can drastically speed up the programs.

03:33

What I mean by this is there are different speeds at which the tool is gonna travel,

03:37

the rapid movements and the feed movements

03:39

changing where those happen can really speed up the machining process.

03:43

Reducing the amount of time you're spending, not cutting material.

03:47

Next, we're gonna move over to our passes section

03:50

in the passes section.

03:51

We've got a couple of options, but we're not going to change too much here.

03:54

First note that we've got our pass direction reference.

03:58

This is gonna allow us to change which direction the tool is going by default,

04:02

it'll be going along the X and Y directions.

04:05

Also as we go down, you can see that we've got a pass extension.

04:09

This is gonna be half of our tool or the radius value of our tool.

04:13

This means that the tool is going to extend past

04:15

the end of our stock before it turns around.

04:18

There's also a step over value and in this case, 1.7 millimeters is relatively low.

04:23

I'm gonna set this just shy of the diameter of our tool at 11 millimeters.

04:29

Next, we have a direction reference by default, it's gonna go both ways.

04:33

But if you have a specific machining direction, for example,

04:36

climb or conventional, you can change those.

04:38

Here.

04:39

There is a new option called order for shorter links that can reduce

04:43

the amount of time it takes to machine or face our part.

04:46

However, order for shorter links only works.

04:48

If you change your direction to a specific climb or conventional direction,

04:52

it won't work with the both option.

04:55

There's also a from other side and use chip

04:57

thinning which we're going to omit for right now.

05:00

And in the linking section,

05:01

this is gonna dictate how the tool moves into and out of our cuts.

05:05

And we're gonna leave these as default for now and say, OK,

05:08

once done, we'll get a preview on the screen,

05:10

showing us a green preview of the stock as well as

05:14

the lines that the tool is going to be traveling.

05:16

If we go back to our front view,

05:17

we can now see that the stock is cut down to the top of our part.

05:21

This is done showing us in process stock and

05:24

the visibility can be changed by going down to this

05:26

bottom section in fusion and turning on or off the

05:29

in process stock or by going to our tool,

05:32

visibility

05:32

going on and off for the tool.

05:35

And we can also turn on and off our tool paths.

05:39

This can help especially once we get into more complex

05:41

tool paths that have much more movements on the screen.

05:44

But for right now, we're gonna leave them as is.

05:46

So anytime we click on our facing tool path, we'll get a preview

05:50

now that we face the top of our part,

05:52

we're going to move on to doing some roughing operations

05:55

in the two D tools.

05:56

We've got a two D adaptive clearing,

05:58

which is a wonderful option for nearly all types of parts.

06:02

There are other options such as two D pocket for clearing.

06:05

But the two D adaptive is going to allow us to cut

06:07

a little bit deeper and keep a consistent load on our tool.

06:10

We're going to select two D adaptive clearing.

06:13

We're gonna be using the same tool moving on to our geometry selection

06:17

and we're going to select the bottom outside edge of our part.

06:20

There'll be a blue preview on the screen and this is gonna

06:23

let us know which side of the part is gonna be cut.

06:26

You also note that this goes out to the size of our stock,

06:29

so no other selections are needed.

06:31

Next, we're gonna go to our height section at

06:34

this point.

06:35

All of the heights are going to be ok because

06:37

the bottom height is based on our selected contour.

06:39

However, a two D adaptive tool path is a roughing tool path,

06:44

which means it's intended to leave stock behind.

06:47

And that's gonna not allow us to cut all the way down to the bottom of our part.

06:50

So if we view this from a front view again,

06:52

and we go down to our bottom height and the selected contours

06:55

and we add, say two millimeters

06:58

that's going to allow the tool to go two

06:59

millimeters relative to the bottom of our part.

07:02

However, the positive value is in the positive Z direction.

07:06

Because of the coordinate system, we need to use a negative value.

07:09

If we make this change, all we need to do is edit our tool path,

07:13

go to our height section

07:14

and change the offset value to minus two millimeters and say, OK.

07:19

Now the preview on the screen shows the tool path

07:21

cutting two millimeters below the bottom of our part.

07:24

Let's go ahead and take one quick look at the rest of the settings.

07:27

Before we move on to the next tool path.

07:30

In the passive section,

07:31

we have some values in here such as optimal load that are going to determine

07:35

how much engagement we have between our tool and the material that it's cutting.

07:39

We have a default stock to leave.

07:41

In this case,

07:42

it's half a millimeter in the radial direction and the axial direction.

07:46

This means on the side of the tool and on the bottom of the tool.

07:49

Next, we also have a multiple depths option.

07:52

In this case, our tool can make this cut with a single depth.

07:55

But if we had to cut extremely deep into a part, we may need to toggle that on.

08:00

The next option here is multi

08:02

axis which we're not taking a look at. And the last one is linking

08:05

by default, it'll do a helo

08:07

entry and we're gonna leave all of these values as default and say, OK,

08:12

back in a home view,

08:13

we can now see that we've cleared the material around the outside

08:15

of our part all the way to two millimeters below the part

08:19

minus that extra half a millimeter that it's leaving for a stock to leave.

08:23

Now, we want to remove the material from this phase.

08:26

We can do this in a single operation,

08:28

but it's good practice to go back and do this a couple of different times.

08:31

So we're going to use the same process using a two D adaptive clearing.

08:35

Note that when we're using two D adaptive clearing,

08:38

there is a rest machining option.

08:40

However, with two D tool pass,

08:41

rest machining is really taking a look at a previously

08:45

sized tool and the material that would be left behind

08:48

when we get into 3D tool pass,

08:49

those are model aware and they make better use of

08:52

the material that was left behind from previous operations.

08:55

So for us,

08:56

we're gonna use a closed chain selection and not worry about rest machining

09:01

next.

09:01

In the height section,

09:02

we need to be careful here because we are gonna

09:05

be leaving stock and we can't have a bottom height offset

09:08

because the bottom of the tool is hitting stock,

09:11

we need to make sure that it's stopping at that area.

09:14

And in our passive section, we're leaving a half a millimeter of stock.

09:18

So for this tool path, we're gonna say, OK,

09:21

now that we've got our roughed material,

09:23

we need to go back and finish it and this can

09:25

generally be done with a couple of different tool paths.

09:28

For our part. It's gonna make the most amount of sense to use a two D contour.

09:32

Once again, we're gonna do this in two separate operations.

09:36

We're gonna select our tool.

09:37

We're gonna move to our geometry and select this bottom edge for our contour.

09:41

We're gonna move to our passes, make sure that we're not leaving any stock.

09:45

And we're gonna say, OK,

09:47

because of the size of our tool and the size of material that we need to remove,

09:51

we can do this in a single pass.

09:53

The reason we didn't do the bottom edge at the same time is

09:56

because the bottom edge needs to be cut a little bit lower.

09:59

So we're gonna do a two D contour one more time

10:02

this time selecting our bottom edge.

10:04

But inside of our passes section, we need to make sure that we are not leaving stock.

10:08

And in our height section, we need to make sure that we're using a negative offset.

10:13

When we did our two D adaptive, we had negative two millimeters.

10:16

However, that left half a millimeter of stock behind.

10:20

If we do this, it's going to engage too much stock at the bottom of our cut.

10:24

So we're gonna use minus 1.5 millimeters and say, OK,

10:28

this should get us down to the exact same height as our two D adaptive clearing.

10:33

Now that all of the outside of our part has been machined.

10:36

The last thing that we need to do is take care of the holes,

10:38

the holes are taken care of with drilling operations.

10:42

We're gonna start the drilling operations by using a spot drill.

10:45

This is gonna be tool number two in our tool library.

10:48

And we're gonna select aluminum drilling.

10:51

Then for our geometry, we're gonna select the insides of each of these holes.

10:56

By default. Fusion wants to drill all the way to the bottom of the hole.

10:59

This is a problem because we're using a spot drill and we

11:02

only need to start the hole so that it centers our drill.

11:05

So from our height section,

11:07

the very bottom, we're gonna change the from

11:09

to be the top of our hole.

11:12

And we're going to use the drill tip through bottom and say, OK,

11:15

this is gonna leave a small indent at the center of

11:18

each hole that allows the larger drill bit to be centered.

11:22

Next.

11:22

We're gonna do another drilling operation once again,

11:25

selecting each of these center holes.

11:26

However, this time we're gonna use the final size drill bit.

11:29

It's gonna be tool number three, a six millimeter drill.

11:32

And we'll select aluminum drilling for our preset.

11:35

We're going to go to our geometry selection, select each hole

11:39

and in our height section from our front view,

11:42

we want to make sure that we're drilling through the bottom.

11:45

And in this case, we've got two values,

11:47

we've got an offset value and a breakthrough depth,

11:50

the offset value is going to be based on our Z coordinate orientation.

11:54

This means that we need a negative value to go

11:56

further down and a positive value to go further up.

11:59

However, with the breakthrough depth,

12:01

if we use a positive value of two millimeters,

12:03

this is going to extend beyond the bottom of our part.

12:06

There is one more thing that we need to change and that's gonna be the drilling cycle.

12:11

This is gonna be a canned cycle that gets called inside of our coat.

12:14

Typically, when we're doing a spot drill,

12:17

the drill bit can come down spot the hole relatively quick and retract away.

12:21

However, when we're actually drilling in the material,

12:24

we want to use something like a chip breaking cycle.

12:27

This allows the drill bit to go in a small amount and

12:29

either pause or retract to allow the hole to clear the chips

12:33

and allow coolant to get into that hole.

12:35

This is especially important when we're drilling deep holes to ensure

12:38

that the quality and the diameter of the hole are consistent.

12:42

We're gonna say, OK, and we'll go back to our home view

12:46

at this point, everything looks ok.

12:48

However, the drill bit size is too small for the size of our hole.

12:52

If we use our inspect measure tool and we measure this hole,

12:55

we can see that it's currently at a diameter of eight millimeters.

12:59

We've already created our tool path with a six millimeter drill.

13:03

And if we expand this, you can see that tool number three is a six millimeter drill.

13:07

If we right click, we are able to edit the tool.

13:10

This means that we can go in and modify its parameters.

13:13

You should only do this if you have direct control

13:16

over which tools you have available on your machine.

13:18

In

13:19

this case, I'm gonna just simply change the diameter to eight millimeters

13:22

except

13:23

and now it tells me that this tool path is out of date

13:26

to fix this. All we need to do is go to actions and select generate.

13:31

It's gonna redo the tool path with the updated tool diameter,

13:34

our eight millimeter drill.

13:36

And now we can see the preview on the screen shows

13:38

that the holes are being drilled to the correct size.

13:41

Now, at this point, we've created our facing tool path,

13:44

our two D adaptive tool path to rough the stock

13:47

and our two D contours to finish the outside shape.

13:50

Then we went back with a spot drill to start

13:52

the holes and a drill bit to finish the holes.

13:55

So at this point,

13:56

let's go ahead and make sure that we save everything

13:58

we've done before we move on to the next step.

After completing this video, you’ll be able to:

  • Create a drilling operation.
  • Create 2.5 axis roughing toolpaths.
  • Create 2.5 axis finishing toolpaths.

Video quiz

What does the orange border displayed during geometry selection for a facing toolpath represent?

(Select one)
Select an answer

1/1 questions left unanswered

Step-by-step guide

It appears you don't have a PDF plugin for this browser.

Was this information helpful?