Adaptive Clear Stock

00:02

Adaptive clear stock.

00:05

After completing this video, you'll be able to

00:07

use a 3D adaptive tool path and adjust tool path parameters.

00:13

In fusion 3 60 we want to carry on with the data set. From our previous example.

00:17

At this stage,

00:18

we have our caliper in a vise and we have our new setup off one

00:22

created with the coordinate system in the right location and our stock is defined.

00:26

Now, we need to start creating tool paths that will remove the material.

00:29

So we can end up with a final part.

00:31

This course is gonna focus mainly on two D or 2.5 axis tool paths

00:36

where the Z movement happens independent of the X and Y.

00:40

Well,

00:40

that's not universally true for tool paths like

00:42

two D contour with helical entries or ramps.

00:45

It is generally true that 2.5 access tool paths

00:48

are going to move independently in Z and X and Y.

00:52

We are also going to use a 3D tool path. In this case, adaptive clearing.

00:57

There are times when 3D or three axis tool

00:59

paths that can move simultaneously in XY and Z

01:02

are going to make the most sense.

01:04

And in this case,

01:05

it makes sense for us to start this process by using a 3D adaptive clearing.

01:09

For one main reason

01:14

They're taking a look at the geometry specifically this caliper

01:18

because we have a lot of geometry at different heights.

01:21

It's gonna be the easiest tool path for us to rough out the part.

01:24

If we go to a two D adaptive clearing,

01:27

this has a similar tool motion in the X and Y direction

01:31

using a constant chip load or a troi

01:34

coal

01:34

motion.

01:35

But this is going to be based on pocket selections chains or faces.

01:39

This is not going to be necessarily model aware,

01:42

which means that we have to do a little bit more to set it up.

01:46

So to get started, let's go to our 3D tool path and use adaptive clearing.

01:51

The first thing that we need to do when setting up our

01:53

new tool path is to select the tool that we want to use

01:56

for this.

01:57

We're gonna go into the tool library that we

01:59

have set up called the precision machining caliber dash

02:03

S

02:03

inside of here,

02:04

we have all the tools that we created in this tool library and we

02:07

also want to make sure that we don't have any tool category filters turned on

02:11

if you have a filter, make sure that you clear it in the upper right.

02:15

One of the main reasons why you see filters on by default is

02:19

because some tool paths will dictate what types of tools can be used.

02:22

For example, when de

02:24

burring using a two D chan

02:25

tool path, it needs to have a specific champ or an engraving tool.

02:30

And this means for tool paths like adaptive,

02:32

it's not gonna be using certain tools like drill bits.

02:35

So those will automatically get filtered out.

02:38

But to make sure that all the tools are in your library,

02:40

go ahead and clear that filter just to make sure that everything is here.

02:44

The tool that we want to use is going to be tool number seven,

02:46

which is our half inch flat

02:48

note. When we set this up, we don't have other cutting data presets.

02:52

But if you did, you would want to make sure to preselect which one you want to use. Now,

02:57

on the right hand side, we've got product info.

02:59

In this case, we've got information about the vendor,

03:02

the product ID,

03:03

if there's a hyperlink to that tool and then information about the geometry,

03:08

we're gonna select this tool to be used in this 3d adaptive tool path.

03:12

The next thing that we want to do is double check

03:14

and verify the feeds and speeds that have come in.

03:17

You can see here that we've got a spindle speed of 8100 R PM.

03:21

It's important that we understand the machine that we're using this

03:24

on and what that R PM limit is going to be

03:27

in our case, a

03:28

SVF two has a limit of 8100 R PM.

03:31

If we're going to a different machine,

03:33

it might be possible to run the tool faster and potentially more efficiently.

03:38

In this case, we're gonna leave it at 8100. But this is important that we understand

03:42

the machine that this is going to be run on because these values are critical

03:46

as we move over to the second tab. This is going to be our geometry selection

03:51

as mentioned fusion 3 60 3d tool paths are model aware.

03:55

So all it really needs to know is the stock size.

03:58

In this case, the orange box shown on the screen

04:01

and it's going to look in that area to machine and remove geometry.

04:05

So we don't have to make any selections at all for this tool path.

04:09

But note that by default, rest machining will be turned on.

04:12

We're gonna disable that because there's no prior tool path.

04:15

And there's no reason that we need to calculate that

04:18

the next tab is going to be our heights.

04:20

And this is gonna dictate the various heights where the

04:22

tool changes from things like rapid to feed rates.

04:26

As we look at this, it helps often to go to a side view.

04:29

So we can understand where these planes are located.

04:32

For example, at the very top,

04:34

we've got our clearance height any time the tool needs to go to a clearance move,

04:38

for example, potentially rapiding between movements or at the end of a tool path.

04:42

This is how far above the part it's going to go.

04:45

The second height down is going to represent our retract height.

04:48

Now, if we're retracting between independent moves,

04:51

we might see the tool go up to this plane.

04:54

The next height is our top offset.

04:55

And if we take a look at this,

04:57

this is based on the top of stock and it's currently set to zero.

05:01

And the dark blue plane at the very bottom is our bottom offset,

05:04

which is currently set to model bottom.

05:06

This is potentially a problem especially for this initial roughing tool path.

05:10

Because if we move over to the next tab for just a moment, we can see that by default,

05:15

this is a roughing tool path with stock to leave.

05:18

This means at the very bottom because the height is based on the bottom of our part,

05:23

we're gonna end up leaving 20 thou of stock that's

05:26

going to be roughly the size of that champ.

05:29

So we wanna make sure that we do account for that whenever we're modeling

05:33

and whenever we're programming our tool paths,

05:35

the part is entirely above the vice,

05:38

but we do have stock below the jaws of the vice down to this, in this case, a parallel.

05:43

So we can machine a little bit lower and get slightly closer to the vice.

05:47

This is critical that we understand that this number is going

05:51

to be based off of the stock that we put in

05:53

digitally. This makes sense.

05:55

But if you end up putting a piece of stock that's taller or smaller than this,

05:59

you're gonna end up putting your tool closer or further away from the vice.

06:03

So it's critical that we make sure we understand that these are all

06:06

based off of a number that we selected based on our stock.

06:10

So we're gonna move back over to our heights.

06:12

And instead of using the bottom of our model, we're gonna use a selection.

06:16

I'm gonna select the top of my vice and then I'm gonna enter an offset value.

06:22

Z is currently located at the top of our stock.

06:24

So anything above that is a positive value and anything below that is negative,

06:29

this means that when we create code,

06:31

we can look at the code and see that any

06:33

negative Z values are going to be removing material or machining

06:37

any positive Z values will be above our part or in this case above our raw stock.

06:42

When we're talking about adding or removing values in this case,

06:46

an offset from our bottom

06:48

because we wanted to go up in Z. This is going to be a positive number.

06:52

We're gonna add 50 thou 0.05.

06:55

This should give us enough clearance above the bottom of the

06:57

vice and we're currently below the bottom of our part.

07:01

This means that we move over to our passes section.

07:04

I'm also going to make a slate adjustment to

07:07

the axial stock to leave and set that 2.01.

07:11

This means that 50 thou off the bottom of the vice is actually going

07:14

to be 60 thou because now we're leaving a little bit more stock.

07:18

There

07:18

should still get to the bottom of our part, especially where that champ or that

07:22

is gonna be on the corner.

07:23

But in this case,

07:24

these are things that we need to be aware of

07:26

mainly because when we do a finishing tool path,

07:29

we want to make sure that we're not going to the

07:30

bottom of the cut and engaging a bunch of material.

07:33

We didn't expect to be there.

07:35

There are some other values that we want to identify inside of

07:38

here and we're gonna take a look starting from the top.

07:41

So we've got tolerance values, we've got optimal load values,

07:45

we've got cutting radius values, cavities and so on.

07:48

It's a good idea to hover your cursor over these dialog boxes and you'll

07:52

get a tool tip that tells you exactly what each of these are.

07:55

We're not gonna be going through each of these throughout this,

07:58

but we're gonna identify a couple of critical ones.

08:01

In this case, the optimal load,

08:03

this is going to be the amount of stock or material that the tool is engaging

08:07

because we're doing an efficient cut and adaptive clearing movement.

08:11

This is going to keep that load consistent on the tool

08:14

and it's going to update the way that that tool moves.

08:17

So we wanna make sure that the number that we're using is representative of the tool.

08:22

So make sure that you do double check the tools you're using,

08:24

especially if you're not using the same tools or machine that we have.

08:27

Here.

08:28

In this case,

08:28

we're gonna use a fairly conservative value of 0.05

08:32

knowing that this tool could be run a lot harder

08:35

as we go down. We also want to note the maximum roughing step down.

08:39

This is how deep of a cut the tool is going to take

08:42

while this tool could take a cut that deep. We're gonna reduce this to 0.75.

08:47

So what this means is the tool is gonna go down three quarters

08:50

of an inch and engage 0.05 all the way around our part.

08:55

This automatically sets our fine step down based on that value.

08:59

There's also a flat area detection,

09:01

which is important for us because we do have a lot of flats in this part.

09:04

So we're gonna leave that checked

09:06

and then there is also a minimum step down value.

09:09

Note that this is currently based on 3.9 times 10 to the negative six.

09:14

This is an extremely small value.

09:16

I'm gonna just leave it as default, but note that we can also modify that.

09:20

And the last tab that we have here is going to be our linking parameters.

09:24

This is going to allow us to see how the tool engages or enters the stock,

09:29

how it moves through various movements

09:31

and what kinds of settings will keep it down

09:33

rather than doing a rapid movement above the part.

09:36

So let's take a look at these settings and then we're gonna OK,

09:39

the tool path and we're going to get a preview

09:42

so we can see that our leads in transitions right now.

09:44

We're using a horizontal lead in and lead out radius value of

09:52

Those are gonna be our default numbers and we're gonna leave those as is

09:55

this is also going to be entering the stock with a helo ramp.

09:59

So it'll do that down to its three quarter of

10:01

an inch depth before it starts moving in XY.

10:04

We also have pre drill positions which we're

10:06

not using because this is our first operation.

10:09

So we're gonna say, OK, and we'll take a look at those in future videos

10:12

from the side.

10:13

We can see here that the tool goes down three quarters of an inch,

10:16

it goes down another three quarters of an inch.

10:19

But because we have flat area detection,

10:20

it's able to make intermediate steps based on the geometry

10:25

as we rotate this around, we can also see that it did a helical ramp going into the bore

10:30

and that was able to efficiently remove or rough that material.

10:34

The green that we see on the screen is going to be our in process stock.

10:38

If this is a little too hard to see,

10:40

we can also toggle on and off the tool path visibility or we can toggle

10:44

on and off the stock visibility using F seven and F eight on this keyboard.

10:50

So we can see the material that's been removed and this looks pretty good for a first

10:54

pass without having to make any selections or

10:56

really very minor adjustments to the tool path.

10:59

It is important that we do validate this and make adjustments when necessary.

11:04

For example, we can see a lot of rapid movements going up and over the part.

11:08

Now, while the rapid movements

11:10

are moving at a really high rate,

11:13

it can be inefficient for us to make that many jumps and steps around the part.

11:18

We also want to double check and verify that we're not actually going all the

11:21

way down to the vice and it looks like we're leaving a small amount here.

11:25

So we're gonna leave some process refinement tips for

11:28

future videos where we talk about different tool paths.

11:30

But note that when we first see a tool path on the screen,

11:33

it's important that we do identify things such as the red movements,

11:36

which is going to be the helical entry.

11:38

Our

11:39

yellow movements which are rapid,

11:40

the greens which are lead in and lead out

11:43

and the blue movements which are are cutting movements.

11:46

Let's go ahead and activate or click on the activate button

11:49

next to our set up to go back to our name view

11:52

and then we can save this before moving on to our next step.