& 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
Transcript
00:02
Machine Operation three of apart
00:06
in this video we'll review a blueprint and we use two D. Adaptive too rough apart
00:13
Infusion 3 60. We're going to carry on with our engine case Rh ready to program
00:18
at this point we've created op one where
00:21
we've machined everything from the top side,
00:24
taking care of the top face,
00:25
the drilled and tapped holes the entire outside
00:28
profile as well as delivering the top edge
00:30
in op two. We machined the rest of the what's called the hat off the bottom of the part.
00:36
So now we have all the external faces finished on
00:40
the part and it's time to move on to op three
00:43
for op three. Let's go ahead and create a new setup.
00:46
And for this new setup we want to make sure that we are showing the op three vice.
00:51
So inside of our generic vice we want to hide up to and show up three.
00:55
And based on our synchronization settings,
00:58
we do need to go in and we need to show the individual parts.
01:01
We need to go into our bodies and make sure that we
01:05
do have all of the appropriate bodies shown or hidden as well.
01:08
So for example on the rear jaw we have a lot of different parallels
01:12
In this case we're gonna be using the 1.625 parallels.
01:16
So we want to make sure just to show those
01:19
then I'm going to minimize the model and I'm going to
01:22
rotate this around so we can take a look at our part
01:25
at this stage.
01:26
We do want to make sure that our stock is coming
01:28
from the preceding set up and we are continuing to rest machine
01:32
continuing to rest machine will mean that the stock from the previous setups
01:36
that's already been removed will be accounted for in our new setups.
01:40
However, the stock display on the screen will still look a little different.
01:44
The next thing that we want to do is we want
01:46
to make use of the machined corner of our part.
01:49
So if we rotate this part around, let's go ahead and take a look at it from a front view.
01:54
This side has already been machined as well as this side and the top
01:58
face which means that we can use it as our coordinate system reference.
02:02
So we're going to rotate this model around and
02:04
we're gonna make sure that first off our Z.
02:06
Is pointing in the correct orientation.
02:08
So we need to change the model orientation to select Z. Axis plane and X. Axis.
02:14
In this case X. Is going to be our new Z. And then we also need to flip our X.
02:20
Direction so that it is appropriate relative to our vice.
02:23
Then we're going to change our origin to a model box point.
02:27
And we want to select that box point on this
02:29
corner notice when we do this that nothing is displayed.
02:33
And that's because we haven't actually selected which model we want to machine yet.
02:36
So let's go ahead and select the model.
02:39
And now if we go back to our model box point,
02:41
you can see the corner is able to be selected.
02:43
We do also want to make sure that we include fixtures and we are going to go
02:47
into our models and we want to make sure that we select the generic vice op three.
02:53
This is going to make sure to account for the vice in our simulations
02:56
as well as make sure that we don't collide with it with the tool.
02:59
It is important to note that collision checking is mainly
03:02
used against things like stock that's left behind and the
03:06
part that we're machining but it is always important for
03:09
us to consider the fixtures and the work holdings.
03:11
Whenever we're creating our setups
03:14
now that we have our stock and our wCS or work coordinate system set up,
03:19
we need to move on to post process,
03:21
we're going to set this up as program number 1003
03:25
and this is going to be O P three engine case
03:29
and we're going to be using the wCS offset of three.
03:32
Again,
03:33
we're taking a look at a generic host controller
03:35
or a next gen controller and the wCS offset
03:39
of one or zero is going to be G 54 to for our second op will be G 55
03:47
This wCS offset will get reused for op four as well.
03:51
So we're going to say, okay,
03:52
and now we've created this new op before we go any further,
03:56
let's rename set up 32 B O P three.
03:59
And we also want to right click and create associated named view.
04:04
Remember when we do this and we check another operation,
04:07
it's going to automatically reset our view and all
04:09
of the different bodies and components that were visible.
04:12
This is going to help us make sure that we can associate
04:15
various fixtures and work holdings with the part and its orientation.
04:20
We also have those named views appear.
04:22
We can select them without changing what's visible on the screen but
04:26
it is important that activating these operations can take care of that.
04:30
I do also want to rename up to,
04:32
it looks like I have a lower case P and we can fix that at any point in time.
04:35
Just note that the named view name is not going to change and that's okay
04:40
now that we have op three set up and active, let's go ahead and start machining.
04:45
This is probably going to be the most
04:48
intricate and probably most critical aspect of this program
04:52
now in reality because all of the critical features are inside of this part,
04:57
it would have been best for us to be able to machine this first.
05:00
However,
05:01
the complexities of holding the part in a Standard Vice
05:04
with parallels means that this ends up being our third operation
05:08
but it's a great time for us to take another look
05:10
at the detailed drawing before we create any tool paths.
05:14
So taking a look at the detailed drawing,
05:17
note that we are going to be machining the inside board and
05:20
this is going to be the crankshaft location for the engine assembly.
05:24
We also need to make sure that we have the bolt hole locations that hold both cases
05:28
together as well as the holes that are used for dowel pins to help for location.
05:33
Now we've already machined everything from the top and all of
05:36
the external sides with the exception of the counter board.
05:39
So when we look at these features note that these are
05:43
circled here and this is again representing an inspection dimension.
05:47
This is something that we need to check after.
05:49
The fact also note that the dimensions are referencing this side edge also datum.
05:54
See so date um see we have a quarter inch over for these holes.
05:58
The center hole is at 1.188 and the far right hole is at 2.13.
06:04
There are no additional tolerances listed with
06:06
these dimensions which means that we need to
06:08
take a look at the detailed drawing and see what the tolerances are associated with.
06:12
Two decimal places and three
06:15
and down here we have 30.5 for two decimal places and 20.10 for three decimal places.
06:23
This means the location of the boar is critical and the location
06:27
of the holes is slightly less critical at two decimal places.
06:31
We can see that the tolerance value is a little bit looser.
06:34
So this is something that we should keep in mind when we're machining,
06:37
meaning that we should pay more attention when
06:40
we are going into machine that boar and
06:43
we can still make sure that we are
06:45
on tolerance when we're creating these other holes.
06:48
It is also important to note that the datum reference of C and B. R.
06:54
Machine and these are using R, Y and R. X. Locations.
06:59
Data A is rz location in this orientation.
07:02
So for this critical aspect of our program,
07:05
we are referencing the three critical data that
07:08
are called out in the detailed drawing.
07:10
So let's hop back into fusion and let's begin programming are part.
07:14
So now that we're taking a look at the part,
07:16
let's go ahead and begin creating some operations.
07:19
I'm going to minimize op one and op two,
07:23
we're going to come back to those later rename some of
07:25
those tool paths just for a little bit more clarity.
07:27
But now inside of op three you can see that the green stock is
07:31
showing what's been removed and we still need to remove material from the inside.
07:35
So I'm going to get started focusing on the critical aspect of the design.
07:40
We already know that this face has been machined.
07:42
So I want to begin clearing out material from the inside.
07:45
I'm going to do this with a two d adaptive clearing tool path.
07:49
We want to make sure that we select tool number one which is a half inch flat end mill,
07:54
I'm going to select aluminum roughing
07:57
And I also am going to adjust my cutting feed rate.
07:60
I want to make sure that this stays at that 100" a minute.
08:03
Remember we can always customize those properties inside of our tool library,
08:07
but for these examples,
08:09
I'm just going to manually update it because it's always good for us to double check,
08:13
make sure that we are using the correct preset.
08:15
Next let's move into our geometry.
08:18
Now with this tool path it is going to require us to select some geometry.
08:23
So what I want to do is I want to select this edge right here but I have
08:28
to be careful because I don't want a machine all the way down to this bottom face.
08:32
It doesn't know that this boss is here unless I select a face.
08:36
If I do select a face, however, it's going to omit that boss all the way down.
08:41
So we need to make a decision here about how we want to machine this.
08:44
So I'm going to select that bottom chain,
08:46
I am going to turn on stock contours and this is important
08:49
because it will know exactly how far outside of this pocket.
08:52
It needs to go
08:53
then from our heights,
08:55
we want to make sure that we don't go all the way down to the selected contour but
08:59
instead we're going to go down to a selection which is the top face of that boss.
09:04
Now as we're machining this out,
09:06
we need to think about how much engagement we want with the tool.
09:09
So in the past this section we want to make sure that we look at our tolerance value,
09:14
note that it's at .004.
09:16
Now, instead of three zeros ahead of this, that's going to be an okay amount.
09:21
But my optimal load needs to be reduced a little bit and again,
09:25
when you look at these value,
09:26
optimal load and you're planning out your feeds and speeds.
09:29
This really is going to come from the tool,
09:32
manufacturer data first and then you're going to have to do
09:35
some test cuts and figure out what works for your tools,
09:37
speeding them up and slowing them down,
09:39
figuring out where the sweet spot is for your operation.
09:43
The next thing that we need to think about with the optimal load is
09:46
how much engagement do we want by default because this is a roughing operation,
09:51
stock to leave is already turned on but as of right now
09:55
it's going to make a single depth cut all the way down.
09:58
We do want to make sure that we use multiple depths
10:00
and we're going to go down a distance of .3.
10:04
Now that's a little bit more than half of the tool.
10:06
So the radius of our tool is .25,
10:10
this is going to be a decent amount of engagement and
10:12
again we're not even focusing on the boss just yet.
10:15
That is the critical location feature.
10:17
We're going to have to come back and take
10:19
a couple passes at making sure that's within tolerance.
10:22
But for right now we have everything we need.
10:24
We're going to go ahead and select OK and take a look at the results.
10:29
Let's view this from the top and note that the
10:32
tool is starting pretty far outside of our stock contour.
10:36
We can make some adjustments to the tool path,
10:38
but sometimes it's good at least when you're getting started to
10:42
have a little bit more safety built into the operation,
10:45
it thinks that there's a little bit more stock left than
10:47
there actually is because we haven't turned on rest machining.
10:51
So if we go back and edit this operation and go to geometry and turn on rest machining.
10:56
Note that it's looking for a tool diameter.
10:59
When we have a tool diameter,
11:01
it's looking at how much material was removed beforehand.
11:04
This is not a model aware type of tool path.
11:07
It's only based on our contour selections.
11:09
So the rest machining is not going to bring that in for us in a case like this.
11:14
The only option that we have is we can adjust
11:17
the pocket chain by giving it to a closest boundary
11:22
or we can make adjustments for things like lead in and lead out.
11:25
We can also turn off stock contours.
11:28
Turning off the stock contours will mean that it's no longer going
11:32
to take into account the stock contours again for this operation,
11:35
I'm going to go ahead and leave it with this
11:38
long entry and just allow it to cut that material.
11:40
But just note that this is where you're going to
11:42
spend most of your time making adjustments to tool paths
11:47
with this operation roughed out. Let's go ahead and navigate back to R. O. P.
11:51
Three named View and make sure that we save this before
11:54
we move on to add a few more tool paths.
Video transcript
00:02
Machine Operation three of apart
00:06
in this video we'll review a blueprint and we use two D. Adaptive too rough apart
00:13
Infusion 3 60. We're going to carry on with our engine case Rh ready to program
00:18
at this point we've created op one where
00:21
we've machined everything from the top side,
00:24
taking care of the top face,
00:25
the drilled and tapped holes the entire outside
00:28
profile as well as delivering the top edge
00:30
in op two. We machined the rest of the what's called the hat off the bottom of the part.
00:36
So now we have all the external faces finished on
00:40
the part and it's time to move on to op three
00:43
for op three. Let's go ahead and create a new setup.
00:46
And for this new setup we want to make sure that we are showing the op three vice.
00:51
So inside of our generic vice we want to hide up to and show up three.
00:55
And based on our synchronization settings,
00:58
we do need to go in and we need to show the individual parts.
01:01
We need to go into our bodies and make sure that we
01:05
do have all of the appropriate bodies shown or hidden as well.
01:08
So for example on the rear jaw we have a lot of different parallels
01:12
In this case we're gonna be using the 1.625 parallels.
01:16
So we want to make sure just to show those
01:19
then I'm going to minimize the model and I'm going to
01:22
rotate this around so we can take a look at our part
01:25
at this stage.
01:26
We do want to make sure that our stock is coming
01:28
from the preceding set up and we are continuing to rest machine
01:32
continuing to rest machine will mean that the stock from the previous setups
01:36
that's already been removed will be accounted for in our new setups.
01:40
However, the stock display on the screen will still look a little different.
01:44
The next thing that we want to do is we want
01:46
to make use of the machined corner of our part.
01:49
So if we rotate this part around, let's go ahead and take a look at it from a front view.
01:54
This side has already been machined as well as this side and the top
01:58
face which means that we can use it as our coordinate system reference.
02:02
So we're going to rotate this model around and
02:04
we're gonna make sure that first off our Z.
02:06
Is pointing in the correct orientation.
02:08
So we need to change the model orientation to select Z. Axis plane and X. Axis.
02:14
In this case X. Is going to be our new Z. And then we also need to flip our X.
02:20
Direction so that it is appropriate relative to our vice.
02:23
Then we're going to change our origin to a model box point.
02:27
And we want to select that box point on this
02:29
corner notice when we do this that nothing is displayed.
02:33
And that's because we haven't actually selected which model we want to machine yet.
02:36
So let's go ahead and select the model.
02:39
And now if we go back to our model box point,
02:41
you can see the corner is able to be selected.
02:43
We do also want to make sure that we include fixtures and we are going to go
02:47
into our models and we want to make sure that we select the generic vice op three.
02:53
This is going to make sure to account for the vice in our simulations
02:56
as well as make sure that we don't collide with it with the tool.
02:59
It is important to note that collision checking is mainly
03:02
used against things like stock that's left behind and the
03:06
part that we're machining but it is always important for
03:09
us to consider the fixtures and the work holdings.
03:11
Whenever we're creating our setups
03:14
now that we have our stock and our wCS or work coordinate system set up,
03:19
we need to move on to post process,
03:21
we're going to set this up as program number 1003
03:25
and this is going to be O P three engine case
03:29
and we're going to be using the wCS offset of three.
03:32
Again,
03:33
we're taking a look at a generic host controller
03:35
or a next gen controller and the wCS offset
03:39
of one or zero is going to be G 54 to for our second op will be G 55
03:47
This wCS offset will get reused for op four as well.
03:51
So we're going to say, okay,
03:52
and now we've created this new op before we go any further,
03:56
let's rename set up 32 B O P three.
03:59
And we also want to right click and create associated named view.
04:04
Remember when we do this and we check another operation,
04:07
it's going to automatically reset our view and all
04:09
of the different bodies and components that were visible.
04:12
This is going to help us make sure that we can associate
04:15
various fixtures and work holdings with the part and its orientation.
04:20
We also have those named views appear.
04:22
We can select them without changing what's visible on the screen but
04:26
it is important that activating these operations can take care of that.
04:30
I do also want to rename up to,
04:32
it looks like I have a lower case P and we can fix that at any point in time.
04:35
Just note that the named view name is not going to change and that's okay
04:40
now that we have op three set up and active, let's go ahead and start machining.
04:45
This is probably going to be the most
04:48
intricate and probably most critical aspect of this program
04:52
now in reality because all of the critical features are inside of this part,
04:57
it would have been best for us to be able to machine this first.
05:00
However,
05:01
the complexities of holding the part in a Standard Vice
05:04
with parallels means that this ends up being our third operation
05:08
but it's a great time for us to take another look
05:10
at the detailed drawing before we create any tool paths.
05:14
So taking a look at the detailed drawing,
05:17
note that we are going to be machining the inside board and
05:20
this is going to be the crankshaft location for the engine assembly.
05:24
We also need to make sure that we have the bolt hole locations that hold both cases
05:28
together as well as the holes that are used for dowel pins to help for location.
05:33
Now we've already machined everything from the top and all of
05:36
the external sides with the exception of the counter board.
05:39
So when we look at these features note that these are
05:43
circled here and this is again representing an inspection dimension.
05:47
This is something that we need to check after.
05:49
The fact also note that the dimensions are referencing this side edge also datum.
05:54
See so date um see we have a quarter inch over for these holes.
05:58
The center hole is at 1.188 and the far right hole is at 2.13.
06:04
There are no additional tolerances listed with
06:06
these dimensions which means that we need to
06:08
take a look at the detailed drawing and see what the tolerances are associated with.
06:12
Two decimal places and three
06:15
and down here we have 30.5 for two decimal places and 20.10 for three decimal places.
06:23
This means the location of the boar is critical and the location
06:27
of the holes is slightly less critical at two decimal places.
06:31
We can see that the tolerance value is a little bit looser.
06:34
So this is something that we should keep in mind when we're machining,
06:37
meaning that we should pay more attention when
06:40
we are going into machine that boar and
06:43
we can still make sure that we are
06:45
on tolerance when we're creating these other holes.
06:48
It is also important to note that the datum reference of C and B. R.
06:54
Machine and these are using R, Y and R. X. Locations.
06:59
Data A is rz location in this orientation.
07:02
So for this critical aspect of our program,
07:05
we are referencing the three critical data that
07:08
are called out in the detailed drawing.
07:10
So let's hop back into fusion and let's begin programming are part.
07:14
So now that we're taking a look at the part,
07:16
let's go ahead and begin creating some operations.
07:19
I'm going to minimize op one and op two,
07:23
we're going to come back to those later rename some of
07:25
those tool paths just for a little bit more clarity.
07:27
But now inside of op three you can see that the green stock is
07:31
showing what's been removed and we still need to remove material from the inside.
07:35
So I'm going to get started focusing on the critical aspect of the design.
07:40
We already know that this face has been machined.
07:42
So I want to begin clearing out material from the inside.
07:45
I'm going to do this with a two d adaptive clearing tool path.
07:49
We want to make sure that we select tool number one which is a half inch flat end mill,
07:54
I'm going to select aluminum roughing
07:57
And I also am going to adjust my cutting feed rate.
07:60
I want to make sure that this stays at that 100" a minute.
08:03
Remember we can always customize those properties inside of our tool library,
08:07
but for these examples,
08:09
I'm just going to manually update it because it's always good for us to double check,
08:13
make sure that we are using the correct preset.
08:15
Next let's move into our geometry.
08:18
Now with this tool path it is going to require us to select some geometry.
08:23
So what I want to do is I want to select this edge right here but I have
08:28
to be careful because I don't want a machine all the way down to this bottom face.
08:32
It doesn't know that this boss is here unless I select a face.
08:36
If I do select a face, however, it's going to omit that boss all the way down.
08:41
So we need to make a decision here about how we want to machine this.
08:44
So I'm going to select that bottom chain,
08:46
I am going to turn on stock contours and this is important
08:49
because it will know exactly how far outside of this pocket.
08:52
It needs to go
08:53
then from our heights,
08:55
we want to make sure that we don't go all the way down to the selected contour but
08:59
instead we're going to go down to a selection which is the top face of that boss.
09:04
Now as we're machining this out,
09:06
we need to think about how much engagement we want with the tool.
09:09
So in the past this section we want to make sure that we look at our tolerance value,
09:14
note that it's at .004.
09:16
Now, instead of three zeros ahead of this, that's going to be an okay amount.
09:21
But my optimal load needs to be reduced a little bit and again,
09:25
when you look at these value,
09:26
optimal load and you're planning out your feeds and speeds.
09:29
This really is going to come from the tool,
09:32
manufacturer data first and then you're going to have to do
09:35
some test cuts and figure out what works for your tools,
09:37
speeding them up and slowing them down,
09:39
figuring out where the sweet spot is for your operation.
09:43
The next thing that we need to think about with the optimal load is
09:46
how much engagement do we want by default because this is a roughing operation,
09:51
stock to leave is already turned on but as of right now
09:55
it's going to make a single depth cut all the way down.
09:58
We do want to make sure that we use multiple depths
10:00
and we're going to go down a distance of .3.
10:04
Now that's a little bit more than half of the tool.
10:06
So the radius of our tool is .25,
10:10
this is going to be a decent amount of engagement and
10:12
again we're not even focusing on the boss just yet.
10:15
That is the critical location feature.
10:17
We're going to have to come back and take
10:19
a couple passes at making sure that's within tolerance.
10:22
But for right now we have everything we need.
10:24
We're going to go ahead and select OK and take a look at the results.
10:29
Let's view this from the top and note that the
10:32
tool is starting pretty far outside of our stock contour.
10:36
We can make some adjustments to the tool path,
10:38
but sometimes it's good at least when you're getting started to
10:42
have a little bit more safety built into the operation,
10:45
it thinks that there's a little bit more stock left than
10:47
there actually is because we haven't turned on rest machining.
10:51
So if we go back and edit this operation and go to geometry and turn on rest machining.
10:56
Note that it's looking for a tool diameter.
10:59
When we have a tool diameter,
11:01
it's looking at how much material was removed beforehand.
11:04
This is not a model aware type of tool path.
11:07
It's only based on our contour selections.
11:09
So the rest machining is not going to bring that in for us in a case like this.
11:14
The only option that we have is we can adjust
11:17
the pocket chain by giving it to a closest boundary
11:22
or we can make adjustments for things like lead in and lead out.
11:25
We can also turn off stock contours.
11:28
Turning off the stock contours will mean that it's no longer going
11:32
to take into account the stock contours again for this operation,
11:35
I'm going to go ahead and leave it with this
11:38
long entry and just allow it to cut that material.
11:40
But just note that this is where you're going to
11:42
spend most of your time making adjustments to tool paths
11:47
with this operation roughed out. Let's go ahead and navigate back to R. O. P.
11:51
Three named View and make sure that we save this before
11:54
we move on to add a few more tool paths.
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.