Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
Professional CAD/CAM tools built on Inventor and AutoCAD
Any referenced datasets can be downloaded from "Module downloads" in the module overview.
Transcript
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.
Video transcript
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.
After completing this video, you’ll be able to:
Step-by-step guide
How to buy
Privacy | Do not sell or share my personal information | Cookie preferences | Report noncompliance | Terms of use | Legal | © 2025 Autodesk Inc. All rights reserved
Sign in to start learning
Sign in for unlimited free access to all learning content.Save your progress
Take assessments
Receive personalized recommendations
May we collect and use your data?
Learn more about the Third Party Services we use and our Privacy Statement. May we collect and use your data to tailor your experience?
Explore the benefits of a customized experience by managing your privacy settings for this site or visit our Privacy Statement to learn more about your options.