Create a lathe toolpaths

00:02

Create lathe tool paths.

00:05

After completing this video, you'll be able to

00:08

create profile, roughing and finishing tool, pas create groove tool, pas,

00:11

threading tool path and a parting tool

00:14

pa

00:16

In Fusion 3 60 we want to get started with the supply data set. C

00:20

A

00:20

lathe

00:20

tool

00:21

pa dot F 3D.

00:22

We're going to be taking a look at the

00:23

general process to create a handful of tool paths,

00:26

but we're not going to be covering all tool paths available.

00:29

We first want to begin with the turning face tool path.

00:32

This will allow us to prepare the end of our stock,

00:35

making sure that we have a nice clean surface for

00:37

anything like drilling or boring the center of a part.

00:40

We first need to select a tool.

00:43

In this case,

00:43

we're gonna be going into our document and we want

00:46

to select the general tool number two and hit select.

00:51

We don't need to make any selections because Fusion 3 60 already knows

00:55

where the end of stock is as well as the end of part,

00:57

we just need to verify some of the motions.

00:60

And in this case, we're going to go into geometry.

01:02

Noting that it's automatically grabbing the front of our model

01:05

in the radii section.

01:07

We wanna make sure that the different values are going to give

01:10

us enough clearance and enough safety before we begin entering the part.

01:15

Each time we talk about things like the retract and the outer limits of our part,

01:19

these are going to determine where the tool rapids or feeds to.

01:23

So keep in mind that making them too large

01:25

or too small could potentially cause a collision,

01:28

especially if your tool can't slow down quick enough.

01:31

We're going to move over to the passes section

01:33

note that we're gonna be going outside to inside

01:37

and also note that the values that we're gonna be using for the passes

01:41

are going to allow for the standard numbers that come directly from our tool.

01:46

Last linking allows us to go to and from the safe Z distance.

01:52

And that's gonna be the distance that's out here as defined in our setup.

01:56

We're gonna say, OK, leaving all the rest of the defaults

01:59

and note. Now, we can see that the tool comes in,

02:01

moves in and creates our cut

02:04

and we can verify this later on when we begin talking about simulation.

02:08

But note that with lathe,

02:09

we're actually looking at a cross section of the part you can see shown in darker blue

02:15

and we've got the yellow section representing the stock that remains,

02:19

we can use the stock visibility to turn on or off the stock preview,

02:23

but this will still leave this yellow section showing us where stock still remains.

02:28

The next thing that we wanna do is talk about external profile,

02:32

roughing and finishing

02:33

the turning profile, roughing will allow us to rough out the part

02:38

and then we can go back with a finishing tool path.

02:41

Once again, we're gonna use the same tool note.

02:43

Now we see slightly different settings.

02:46

We're gonna be going outside. We're not doing profiling inside of our part.

02:50

And we're gonna leave the tool orientation as default.

02:53

Some machines will allow you to adjust the angle of the tool.

02:57

But in this case, we're going to assume that our tool is fixed,

03:00

we're gonna move over to the second section

03:03

and we're gonna take our back plane.

03:05

Remembering that we actually have some obstruction here with the jaw.

03:09

And what we're gonna be doing is making sure that we're clear of that Chuck plane

03:14

and we're gonna be starting all the way at the front.

03:17

We don't need to worry about any additional offsets or extensions.

03:20

We're gonna simply say, OK, leaving all of the default settings

03:24

we can see here now that the tool is moving

03:27

from left to right or right to left,

03:29

depending on our settings and it's moving in the X direction,

03:32

removing that material.

03:34

Once again, if we zoom in,

03:35

we can see the material that's left behind and we

03:37

can see that the tool slightly dropped into that groove

03:41

there are options for groove suppression if we go back to our passes

03:45

and we can allow it to skip over any grooves

03:48

or we can allow it to drop into those.

03:51

If we go back into our tool path under our geometry section,

03:54

we can toggle on groove suppression and we can allow it to skip those areas.

03:59

This will allow us to avoid specific areas of a tool path.

04:03

But in this case, because this back wall is shared,

04:06

it's not going to allow us to suppress just that area.

04:09

But that's OK because this tool can't go very deep into that groove.

04:13

It will allow us to come back and do a clean up pass.

04:17

The next thing that we want to do is repeat this process.

04:19

But this time we're gonna be using profile finishing,

04:22

we're gonna use the same tool in this instance.

04:25

But in some cases,

04:26

you might find that you'll use a different tool between roughing and finishing

04:30

for our geometry. Once again that back plane, we're gonna be moving forward

04:35

and under our passes section,

04:37

we want to make sure that we are making sharp corners,

04:40

a spring pass will allow us to go back.

04:43

No dragging. This will allow us to avoid dragging the tool up a face.

04:49

But we're going to leave these options as default and say, OK,

04:52

this goes back and it cuts the rest of the material

04:54

that was left behind with the exception of that one groove

04:58

Now, let's go to our turning options and let's take a look at doing a groove tool path.

05:03

We've got groove finishing.

05:05

We've also got turning groove and turning single groove,

05:08

depending on the layout of your model.

05:10

This will determine which one of these options you'll be using.

05:13

I'm gonna select turning single groove.

05:15

Then from our tool selection, we're gonna go in and select our OD grooving tool.

05:20

If we take a quick look,

05:21

we can see the width of the tool is 0.125 and there is a small corner radius.

05:26

We're gonna select it.

05:27

Then we need to move on to our geometry selection,

05:31

gonna rotate the model just slightly

05:33

and I'll be selecting that inside edge.

05:35

When we go back to a top view,

05:38

you can see here.

05:38

Now the tool comes in, moves into that position and it'll pull back out.

05:43

We have groove side alignment as middle and tip and we'll say, OK,

05:47

and just take a look at the preview.

05:49

When we look at the preview, you can see that the tool is actually offset forward.

05:54

It's centered on our selection. So we need to go back into our settings

05:58

back into the geometry.

06:01

And this time instead of middle, we can do a back or a front alignment.

06:06

When we do a front alignment,

06:07

it moves the tool all the way forward and we do a back alignment,

06:10

it moves the tool all the way back.

06:12

We're gonna say OK, and allow it to regenerate that tool path.

06:16

We can see now that we were able to remove all the material.

06:20

But there are other tool paths that we do want to talk about.

06:23

We do have a tool path for turning champ for.

06:25

Now, the profiling tool path will allow us to take care of large model champers.

06:30

But an actual champ for tool path will allow us

06:33

to come back and just simply break those edges.

06:36

We want to make sure that we do go back to our general turning tool.

06:41

Then we want to select our geometry. And for this, I'm gonna select the front edge,

06:46

this back edge and I'll select this front edge as well.

06:49

And then we need to specify the size. I'm

06:52

gonna go with a relatively small champer of 0.04 at 45 degrees and say, OK,

06:58

now we have a warning telling us it failed to generate.

07:00

Now,

07:01

one thing we always have to be careful with is the

07:03

orientation of our tool relative to what we're trying to cut.

07:07

If we go back into the two D

07:09

Cher

07:09

tool path, and we

07:10

deselect this edge here and say, OK,

07:12

it's able to generate.

07:14

So part of the problem that we have is this specific tool isn't able to cut that champ

07:20

at 45 degrees here.

07:21

So if we wanted to clean that corner up,

07:23

we would have to come back with a different tool in order to do it.

07:27

Keeping in mind that this is a relatively small champ for close to a wall.

07:31

So it would need a very specific tool.

07:34

Now that we've processed most of the model,

07:36

let's come back and let's do a threading tool path here

07:40

under the turning section. We're gonna select turning thread

07:44

and then we need to select a specific turning threading tool.

07:48

We're gonna select OK, and take a quick note of the thread pitch being 0.05

07:53

we're gonna select our geometry.

07:57

And then on the radii, we're going to leave all these settings as default

08:01

for passes.

08:02

We have a thread depth of 0.04 by default and a

08:05

thread pitch of 0.05 which comes directly from our tool.

08:09

We're going to say OK and allow it to generate that tool path.

08:13

When we look here,

08:14

we can see that it's starting from the front of our part and moving through,

08:18

but it doesn't extend past the end

08:21

in order to adjust that we need to go back into our settings.

08:24

And in our geometry, we need to include a small backside offset

08:28

because that's an eighth of an inch gap.

08:30

We're gonna say 0.06 allowing it to extend just barely and say OK,

08:36

validating the tool path that was created here will need to be done with simulation.

08:41

As this preview we see on the screen is not gonna

08:43

be able to let us know what that thread looks like

08:46

we can turn in process stock back on.

08:49

But once again,

08:50

it's not gonna be able to verify or validate that threading tool path.

08:54

I'm gonna toggle this back off for now.

08:56

And the last tool path that we do want

08:58

to identify is something called a parting tool path

09:01

in general.

09:02

When you're creating a lathe part, at the very end,

09:05

you'll likely be using a parting tool path to

09:07

remove the part from the rest of the stock.

09:09

In

09:09

this specific case,

09:11

what we actually did was we have the chuck on this portion of our part,

09:15

which means that we can't actually select the back

09:17

edge to remove it from the rest of stock.

09:20

But we are gonna select turning part,

09:22

we need to use an appropriate tool.

09:24

And in most cases, a grooving tool or a very specific parting tool will be used.

09:29

We'll select this

09:31

and note that by default, it's going off of the back of the part.

09:35

We can move that in a specific amount if we wish and part it off sooner.

09:40

But in general, it will be the back of your digital model.

09:44

I gonna say, OK, and allow it to generate,

09:46

noting that we have now gone through and removed this

09:49

portion of our design from the rest of the stock

09:53

at this point.

09:53

Let's make sure that we do save our design before we move

09:56

on and start talking about simulating tool paths and generating our documents.