& Construction

Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
& Manufacturing

Professional CAD/CAM tools built on Inventor and AutoCAD
Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
Professional CAD/CAM tools built on Inventor and AutoCAD
In this practice, you’ll create all the operations needed to machine one side of a bracket.
Learning objectives:
Exercise
Any referenced datasets can be downloaded from "Module downloads" in the module overview.
Transcript
00:01
This is the practice exercise video solution
00:04
for this practice exercise.
00:05
Let's begin with the supply data set caliper bracket dash cams setup dot F 3D.
00:10
This already contains a setup
00:12
one with stock and we're gonna be machining this
00:14
without worrying about how it's held in a vice.
00:17
It's always important for us to understand how our parts
00:20
are held because it will affect the tool path,
00:22
the clearance and the way in which we approach the different operations.
00:26
But for this example, let's focus just on the tool path and not how the part is held
00:31
to get started. We can use a two D or a 3D adaptive clearing.
00:35
Once again, the 3D adaptive clearing is going to be model aware,
00:39
which means that we don't really have to make any selections on our part.
00:42
We're gonna start by going into our precision
00:44
machining tool library and selecting tool number seven,
00:47
which is our half inch flat end mill
00:49
in the geometry section fusion 3 60 automatically grabs our stock contour and
00:54
it's going to be looking in that area for areas to machine,
00:57
we can toggle off rest machining since this is our first tool path
01:01
in the height section, we do wanna make sure that we are going below the part
01:05
and in this case, I'm gonna set this at 0.05.
01:09
Then in our passes section,
01:12
we want to make sure that we identify stock to leave is currently set at 0.02 or 20.
01:16
Th
01:17
this means that even though we're going 0.05 below our part,
01:22
the actual stock that's gonna be remaining is 0.03.
01:25
The difference between those two values
01:27
we're gonna say, OK, and allow it to generate,
01:30
we can see that we've roughed out the entire part.
01:33
And now we're gonna move on to finishing the outside profile.
01:36
Once again, consideration on how the part is held is always important.
01:40
But for these practice examples, we're only gonna be focusing on the tool paths.
01:43
So from our two D menu, we're gonna select two D contour,
01:48
we're gonna carry on using the same tool number seven.
01:51
And the geometry will simply be this bottom edge,
01:54
the height by default is going to be based on that selected contour,
01:57
but we need it to come down a little bit further.
02:00
Remember that the Z values are based on the coordinate system.
02:04
In this case with everything except for drill tip
02:06
through bottom when we're using a drilling operation.
02:09
So
02:10
Z up and away from the part is positive and Z down is negative.
02:14
If this is tricky, we can always change the bottom height to model bottom,
02:18
which will bring back our plane
02:20
and we can take a look at entering a positive value
02:23
noting that it's coming up on the part or
02:25
a negative value noting that it's going below.
02:28
Remember in the two D or 3D adaptive tool pass that we use to rough
02:32
our part stock to leave is gonna come into play with the bottom height.
02:36
We wanna make sure that we don't take our two D
02:38
contour tool and bury it into the stock at the bottom.
02:41
So for this reason, we're gonna have 0.03
02:45
in the passes section.
02:47
We want to make sure that we're not using stock to leave and we can
02:49
carry on adding things like repeating the finishing
02:52
pass if needed or adding roughing passes.
02:54
If we want to make sure that we add additional passes,
02:57
I'm gonna set this at 0.2 inches and say, OK,
03:01
this allows us to create a roughing pass and then come back with our finishing pass
03:06
once again, the 3d Adaptive cleared out most of this material.
03:09
So the roughing pass is really not needed. In this case,
03:14
any changes can be done by right clicking and editing our tool path,
03:17
going to our passes section and toggling off roughing passes and saying, OK,
03:22
now that we have the outside of the part finished,
03:24
let's go back and focus on finishing off the various areas and faces.
03:29
We're gonna be using our two D drop down and selecting two D pocket
03:32
again with the same tool number seven.
03:34
And for our geometry, we want to select the various faces that we want to finish.
03:39
Fusion 3 60 will be able to identify areas
03:41
where there are contours that need to be created.
03:44
So for example, around the outside of this box, we see a darker blue line
03:48
note that on the top, we're not seeing a blue line around the opening or the hole.
03:53
This is perfectly fine and this will allow us to finish off the entire top of that box
03:58
in the passes section. Make sure that we disable stock to leave. And we'll say, OK,
04:03
this will create our finishing tool path to finish both the faces of the different
04:07
parts of the caliper bracket as well as the side faces around the boss.
04:12
If you want to,
04:13
you can always use F seven to toggle on and off the tool path to get
04:16
a better idea of what areas have been machined and what have been left behind.
04:21
Now that we've finished off the outside and the inside,
04:24
we need to go back and drill the holes to do this.
04:27
We're gonna be using a drilling tool path with tool number one,
04:30
which is our spot drill.
04:32
So make sure that we go into our library,
04:33
select tool number one and then select the holes that we want to drill.
04:37
Remember that when selecting holes, there are multiple methods.
04:40
In this case, I'm selecting the inside faces.
04:43
And then when we move on to our height section,
04:45
we're going to be using the whole top instead of the
04:48
whole bottom because we are using a spot drilling operation.
04:52
When we're using a spot drill,
04:53
we also have the option to simply click drill tip through bottom.
04:56
If the holes are larger than the diameter of the spot drill,
04:59
this generally will be fine.
05:01
However,
05:01
we're gonna be tapping this hole here and we wanna
05:04
make sure that the spot drill is not too large.
05:07
Everything does look, OK.
05:08
So I'm gonna simply use that drill tip through bottom and say, ok,
05:13
next, we need to drill the holes.
05:14
And for this, I want to double check and measure the whole sizes.
05:18
In this case, you can see the diameter is 0.313.
05:21
And if I measure the diameter of this hole,
05:24
let's go ahead and see what this one comes in at 0.38.
05:28
So in order for us to drill and tap this, we need to have the appropriate drill size.
05:33
If we go back to drilling and we make our selections here.
05:37
Let's go back to our tool and see if we have that drill in our library.
05:41
We can see that we have a 2 57 which is not gonna be the appropriate size.
05:46
If we don't have the proper size drill bit,
05:48
we can always use N mills to get it to the proper size.
05:51
Or add additional tools to our tool library.
05:54
For this example, I am gonna be using the larger drill bit that I have available,
05:58
making sure I'm using aluminum drilling
06:01
and I wanna go ahead and add all the holes to this,
06:04
making sure that on the heights we do drill tip through bottom,
06:07
we're gonna add a small offset of 0.05
06:11
and set our drill cycle to be a chip breaking, which is going to be a partial retract,
06:17
we'll say, OK, and allow it to drill each of those.
06:21
Now,
06:21
we want to finish off those holes and as explored
06:23
before we can do this with various different tool paths.
06:26
For example, we could use a bore a two D pocket or even a two D contour.
06:31
For this example,
06:32
I'm gonna be using a two D contour with the quarter inch flat
06:35
end mill that we have in our tool library as tool number five
06:39
for the geometry. Let's go ahead and select the bottom of each of these holes.
06:46
And then we want to take a look at the way in which we're machining. This,
06:50
the heights are gonna go all the way down to the bottom of the selected contour,
06:53
but we want to go down just a little bit further.
06:56
Remember that we can use the model bottom, which will show the plane
06:60
and then we can have a negative value allowing us to go down just a little bit
07:03
further to make sure that we're not leaving a sharp corner on the bottom of our part
07:08
for our passes section.
07:09
We are going to be doing a finishing pass, but we wanna make sure that we use a ramp.
07:14
This will allow us to do a helical ramp in.
07:17
We can do pre drill positions if we want the tool to
07:20
go all the way down to the bottom of the hole.
07:22
If we've drilled it large enough.
07:23
In this case,
07:24
the difference between a quarter inch ML and the 0.257 drill is
07:28
a little too tight for me to feel comfortable doing that.
07:31
So I'm gonna allow it to ramp into the hole and
07:33
that's gonna be the way in which we make our cut
07:36
notice when we have this ramping motion
07:38
that we are starting the ramp relatively high
07:42
because these holes are at different heights,
07:44
the ramp height is gonna be based on the tallest one.
07:47
So in order to change that we can right click and edit our heights,
07:51
we can bring our height down just a little bit,
07:54
which will allow us to start the feed a little bit later.
07:57
Uh Keep in mind that this is going to be something
07:59
we need to be very careful with whenever we're creating tool paths
08:02
because we wanna make sure that it does start
08:05
high enough above the part that we don't begin
08:07
too late and just simply engage with a tool
08:09
that's not spinning or moving at the appropriate speed.
08:13
This tool path does produce a problem.
08:15
It's telling us that our lead in and lead outs were dropped due to constraints.
08:18
It simply means that there's not enough room for the lead in and lead out.
08:22
So we're using the helical entry and the tool is
08:24
getting pulled straight back out of the hole perfectly fine.
08:27
Again, in this instance,
08:28
because we are using that ramp down at two degrees to cut the geometry.
08:33
Next, we need to tap those holes.
08:35
And once again, if we have the appropriate size, it should be in our library.
08:38
If we go to our practical machining library, note that we have a quarter 20
08:43
this is not gonna be the appropriate size.
08:45
So we would need to go into the fusion 3 60 library and pick out the right tap.
08:50
We're gonna be using a right handed tap and notice
08:52
that quarter 20 is the only one listed here.
08:55
But once we go into our library and we take a look at the right handed taps,
08:59
we can see here that we've got the appropriate sizes.
09:03
You need to know what the tap is that you need to use. In this case, it's a 5 16, it's 18.
09:09
We're gonna select this,
09:10
this will automatically enable the tapping cycle. And we can say, OK,
09:14
now, in this case, it says that we didn't select any holes,
09:17
make sure that we do select the holes that we
09:18
want to tap and allow it to create that operation.
09:22
The last thing that we want to do is deeper the top edges and to do this,
09:26
we use a two D chan for tool path.
09:29
We need to have an appropriate tool.
09:30
So once again, back into our tool library, we're gonna select tool number two,
09:34
which is a chan for mill.
09:36
And then we simply need to select our geometry.
09:39
Now keep in mind when we make our selections
09:42
that the tool is going to be going around all
09:44
of these various edges that don't currently have a Chamfer.
09:48
This means that we need to come through and manually give
09:51
it a value that we want the champ with to be.
09:54
I'm gonna go ahead and leave all the other options
09:56
as default allowed to go through and create that deep
09:59
or that two D chamber
10:01
at this point, we have all of the various operations created.
10:05
Once again,
10:05
there is a warning because of lead in and lead out
10:08
if you want to clear that you can always go in and
10:10
manually remove the lead in and lead outs by disabling that check
10:14
box and that will remove the warning from the tool path.
10:17
The warnings don't necessarily mean that the operation is going to fail.
10:21
It just is letting us know a change
10:23
that was made based on our selections and parameters
10:26
at this point. Let's make sure that we simulate all these tool paths
10:29
just to make sure that we validate all the stock is being removed.
10:33
I'm gonna jump ahead one operation at a time, taking a look at our roughing finishing
10:39
and the holes
10:40
making sure that we are tapping the holes properly
10:43
coming through and doing our final.
10:46
If there are any problems with any of the tool paths now would
10:49
be a good time to check it and change it before creating any documentation
10:54
at this point. Let's go ahead and make sure that we do save this before moving on.
Video transcript
00:01
This is the practice exercise video solution
00:04
for this practice exercise.
00:05
Let's begin with the supply data set caliper bracket dash cams setup dot F 3D.
00:10
This already contains a setup
00:12
one with stock and we're gonna be machining this
00:14
without worrying about how it's held in a vice.
00:17
It's always important for us to understand how our parts
00:20
are held because it will affect the tool path,
00:22
the clearance and the way in which we approach the different operations.
00:26
But for this example, let's focus just on the tool path and not how the part is held
00:31
to get started. We can use a two D or a 3D adaptive clearing.
00:35
Once again, the 3D adaptive clearing is going to be model aware,
00:39
which means that we don't really have to make any selections on our part.
00:42
We're gonna start by going into our precision
00:44
machining tool library and selecting tool number seven,
00:47
which is our half inch flat end mill
00:49
in the geometry section fusion 3 60 automatically grabs our stock contour and
00:54
it's going to be looking in that area for areas to machine,
00:57
we can toggle off rest machining since this is our first tool path
01:01
in the height section, we do wanna make sure that we are going below the part
01:05
and in this case, I'm gonna set this at 0.05.
01:09
Then in our passes section,
01:12
we want to make sure that we identify stock to leave is currently set at 0.02 or 20.
01:16
Th
01:17
this means that even though we're going 0.05 below our part,
01:22
the actual stock that's gonna be remaining is 0.03.
01:25
The difference between those two values
01:27
we're gonna say, OK, and allow it to generate,
01:30
we can see that we've roughed out the entire part.
01:33
And now we're gonna move on to finishing the outside profile.
01:36
Once again, consideration on how the part is held is always important.
01:40
But for these practice examples, we're only gonna be focusing on the tool paths.
01:43
So from our two D menu, we're gonna select two D contour,
01:48
we're gonna carry on using the same tool number seven.
01:51
And the geometry will simply be this bottom edge,
01:54
the height by default is going to be based on that selected contour,
01:57
but we need it to come down a little bit further.
02:00
Remember that the Z values are based on the coordinate system.
02:04
In this case with everything except for drill tip
02:06
through bottom when we're using a drilling operation.
02:09
So
02:10
Z up and away from the part is positive and Z down is negative.
02:14
If this is tricky, we can always change the bottom height to model bottom,
02:18
which will bring back our plane
02:20
and we can take a look at entering a positive value
02:23
noting that it's coming up on the part or
02:25
a negative value noting that it's going below.
02:28
Remember in the two D or 3D adaptive tool pass that we use to rough
02:32
our part stock to leave is gonna come into play with the bottom height.
02:36
We wanna make sure that we don't take our two D
02:38
contour tool and bury it into the stock at the bottom.
02:41
So for this reason, we're gonna have 0.03
02:45
in the passes section.
02:47
We want to make sure that we're not using stock to leave and we can
02:49
carry on adding things like repeating the finishing
02:52
pass if needed or adding roughing passes.
02:54
If we want to make sure that we add additional passes,
02:57
I'm gonna set this at 0.2 inches and say, OK,
03:01
this allows us to create a roughing pass and then come back with our finishing pass
03:06
once again, the 3d Adaptive cleared out most of this material.
03:09
So the roughing pass is really not needed. In this case,
03:14
any changes can be done by right clicking and editing our tool path,
03:17
going to our passes section and toggling off roughing passes and saying, OK,
03:22
now that we have the outside of the part finished,
03:24
let's go back and focus on finishing off the various areas and faces.
03:29
We're gonna be using our two D drop down and selecting two D pocket
03:32
again with the same tool number seven.
03:34
And for our geometry, we want to select the various faces that we want to finish.
03:39
Fusion 3 60 will be able to identify areas
03:41
where there are contours that need to be created.
03:44
So for example, around the outside of this box, we see a darker blue line
03:48
note that on the top, we're not seeing a blue line around the opening or the hole.
03:53
This is perfectly fine and this will allow us to finish off the entire top of that box
03:58
in the passes section. Make sure that we disable stock to leave. And we'll say, OK,
04:03
this will create our finishing tool path to finish both the faces of the different
04:07
parts of the caliper bracket as well as the side faces around the boss.
04:12
If you want to,
04:13
you can always use F seven to toggle on and off the tool path to get
04:16
a better idea of what areas have been machined and what have been left behind.
04:21
Now that we've finished off the outside and the inside,
04:24
we need to go back and drill the holes to do this.
04:27
We're gonna be using a drilling tool path with tool number one,
04:30
which is our spot drill.
04:32
So make sure that we go into our library,
04:33
select tool number one and then select the holes that we want to drill.
04:37
Remember that when selecting holes, there are multiple methods.
04:40
In this case, I'm selecting the inside faces.
04:43
And then when we move on to our height section,
04:45
we're going to be using the whole top instead of the
04:48
whole bottom because we are using a spot drilling operation.
04:52
When we're using a spot drill,
04:53
we also have the option to simply click drill tip through bottom.
04:56
If the holes are larger than the diameter of the spot drill,
04:59
this generally will be fine.
05:01
However,
05:01
we're gonna be tapping this hole here and we wanna
05:04
make sure that the spot drill is not too large.
05:07
Everything does look, OK.
05:08
So I'm gonna simply use that drill tip through bottom and say, ok,
05:13
next, we need to drill the holes.
05:14
And for this, I want to double check and measure the whole sizes.
05:18
In this case, you can see the diameter is 0.313.
05:21
And if I measure the diameter of this hole,
05:24
let's go ahead and see what this one comes in at 0.38.
05:28
So in order for us to drill and tap this, we need to have the appropriate drill size.
05:33
If we go back to drilling and we make our selections here.
05:37
Let's go back to our tool and see if we have that drill in our library.
05:41
We can see that we have a 2 57 which is not gonna be the appropriate size.
05:46
If we don't have the proper size drill bit,
05:48
we can always use N mills to get it to the proper size.
05:51
Or add additional tools to our tool library.
05:54
For this example, I am gonna be using the larger drill bit that I have available,
05:58
making sure I'm using aluminum drilling
06:01
and I wanna go ahead and add all the holes to this,
06:04
making sure that on the heights we do drill tip through bottom,
06:07
we're gonna add a small offset of 0.05
06:11
and set our drill cycle to be a chip breaking, which is going to be a partial retract,
06:17
we'll say, OK, and allow it to drill each of those.
06:21
Now,
06:21
we want to finish off those holes and as explored
06:23
before we can do this with various different tool paths.
06:26
For example, we could use a bore a two D pocket or even a two D contour.
06:31
For this example,
06:32
I'm gonna be using a two D contour with the quarter inch flat
06:35
end mill that we have in our tool library as tool number five
06:39
for the geometry. Let's go ahead and select the bottom of each of these holes.
06:46
And then we want to take a look at the way in which we're machining. This,
06:50
the heights are gonna go all the way down to the bottom of the selected contour,
06:53
but we want to go down just a little bit further.
06:56
Remember that we can use the model bottom, which will show the plane
06:60
and then we can have a negative value allowing us to go down just a little bit
07:03
further to make sure that we're not leaving a sharp corner on the bottom of our part
07:08
for our passes section.
07:09
We are going to be doing a finishing pass, but we wanna make sure that we use a ramp.
07:14
This will allow us to do a helical ramp in.
07:17
We can do pre drill positions if we want the tool to
07:20
go all the way down to the bottom of the hole.
07:22
If we've drilled it large enough.
07:23
In this case,
07:24
the difference between a quarter inch ML and the 0.257 drill is
07:28
a little too tight for me to feel comfortable doing that.
07:31
So I'm gonna allow it to ramp into the hole and
07:33
that's gonna be the way in which we make our cut
07:36
notice when we have this ramping motion
07:38
that we are starting the ramp relatively high
07:42
because these holes are at different heights,
07:44
the ramp height is gonna be based on the tallest one.
07:47
So in order to change that we can right click and edit our heights,
07:51
we can bring our height down just a little bit,
07:54
which will allow us to start the feed a little bit later.
07:57
Uh Keep in mind that this is going to be something
07:59
we need to be very careful with whenever we're creating tool paths
08:02
because we wanna make sure that it does start
08:05
high enough above the part that we don't begin
08:07
too late and just simply engage with a tool
08:09
that's not spinning or moving at the appropriate speed.
08:13
This tool path does produce a problem.
08:15
It's telling us that our lead in and lead outs were dropped due to constraints.
08:18
It simply means that there's not enough room for the lead in and lead out.
08:22
So we're using the helical entry and the tool is
08:24
getting pulled straight back out of the hole perfectly fine.
08:27
Again, in this instance,
08:28
because we are using that ramp down at two degrees to cut the geometry.
08:33
Next, we need to tap those holes.
08:35
And once again, if we have the appropriate size, it should be in our library.
08:38
If we go to our practical machining library, note that we have a quarter 20
08:43
this is not gonna be the appropriate size.
08:45
So we would need to go into the fusion 3 60 library and pick out the right tap.
08:50
We're gonna be using a right handed tap and notice
08:52
that quarter 20 is the only one listed here.
08:55
But once we go into our library and we take a look at the right handed taps,
08:59
we can see here that we've got the appropriate sizes.
09:03
You need to know what the tap is that you need to use. In this case, it's a 5 16, it's 18.
09:09
We're gonna select this,
09:10
this will automatically enable the tapping cycle. And we can say, OK,
09:14
now, in this case, it says that we didn't select any holes,
09:17
make sure that we do select the holes that we
09:18
want to tap and allow it to create that operation.
09:22
The last thing that we want to do is deeper the top edges and to do this,
09:26
we use a two D chan for tool path.
09:29
We need to have an appropriate tool.
09:30
So once again, back into our tool library, we're gonna select tool number two,
09:34
which is a chan for mill.
09:36
And then we simply need to select our geometry.
09:39
Now keep in mind when we make our selections
09:42
that the tool is going to be going around all
09:44
of these various edges that don't currently have a Chamfer.
09:48
This means that we need to come through and manually give
09:51
it a value that we want the champ with to be.
09:54
I'm gonna go ahead and leave all the other options
09:56
as default allowed to go through and create that deep
09:59
or that two D chamber
10:01
at this point, we have all of the various operations created.
10:05
Once again,
10:05
there is a warning because of lead in and lead out
10:08
if you want to clear that you can always go in and
10:10
manually remove the lead in and lead outs by disabling that check
10:14
box and that will remove the warning from the tool path.
10:17
The warnings don't necessarily mean that the operation is going to fail.
10:21
It just is letting us know a change
10:23
that was made based on our selections and parameters
10:26
at this point. Let's make sure that we simulate all these tool paths
10:29
just to make sure that we validate all the stock is being removed.
10:33
I'm gonna jump ahead one operation at a time, taking a look at our roughing finishing
10:39
and the holes
10:40
making sure that we are tapping the holes properly
10:43
coming through and doing our final.
10:46
If there are any problems with any of the tool paths now would
10:49
be a good time to check it and change it before creating any documentation
10:54
at this point. Let's go ahead and make sure that we do save this before moving on.
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.