Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
Professional CAD/CAM tools built on Inventor and AutoCAD
Transcript
00:02
create tool paths. To finish cut parts.
00:05
After completing this video, you'll be able to create a facing tool path,
00:09
create a two D.
00:10
Contour tool path, create chance for and two D.
00:12
Contour champ for tool paths and create a drilling and tapping tool path
00:20
Infusion 3 60. We want to carry on with our mounting block part.
00:23
You have any difficulties in the last video.
00:25
Make sure that you upload the supply dataset mounting block rough dot F. Three Z.
00:30
At this point we've already created a two D. Pocket tool path and a two D.
00:34
Adaptive tool path to make sure that we
00:36
can identify the differences between the two.
00:38
But now we want to take a look at finishing tool paths.
00:42
Remember that the order of operations is typically dictated by the part
00:45
but in general you will use a facing tool path first.
00:48
Then you'll rough apart before you finish it.
00:51
In this case now we're going to go back and take a look at a
00:54
two D facing tool path and then we'll move on to some finishing tool paths.
00:58
Under the 2D dropdown will select face
01:01
and we need to select a tool for facing
01:03
when you're facing apart.
01:05
In some cases you might use a large end mill while in
01:08
other cases you might use a shell mill or a face mill.
01:11
In this example we're going to use a large three quarter end mill
01:15
under the geometry section fusion 3 60 will automatically bring in the
01:18
border or the outside shape of the stock used in your setup.
01:22
No selection is needed but you can select a different area if
01:25
you want to focus the tool on just a specific area.
01:28
However it's important to note that with a facing tool path,
01:31
the tool will always enter and exit the outside of your selection
01:36
for the heights fusion 3 60 will automatically pick the top height as the
01:40
stock top and the bottom height as the model top in the passes section.
01:44
You want to make sure that you dictate the
01:46
number of passes based on the step over amount.
01:49
In this case our tool is three quarters of an inch
01:51
so I'm going to go 30.7 inches between each step.
01:54
Once we say okay our passes are created in order to face the part
01:59
Infusion 3 60.
01:60
We can also take this facing tool path and we can drag it
02:03
all the way up to the top of our tool path list.
02:05
This means that even though it was created after our pocket and adaptive tool paths
02:10
it can be moved up in the line and that way we can have it at the very top.
02:14
Next I'm going to take my two D.
02:16
Pocket right click and suppress when I suppress the tool path,
02:20
it will still remain inside of our setup.
02:21
However,
02:22
it's no longer going to be used to calculate stock removal or any rest machining.
02:26
Now we have our original facing tool path and then we have our adaptive tool path.
02:32
Keep in mind our adaptive tool path has left material on the walls and the floors.
02:37
We need to make sure that we go back and we remove this material.
02:40
But remember that with the small size here we've got
02:43
a little bit of stock left in the middle.
02:44
And this is going to be an important consideration when planning our tool paths.
02:49
The next thing that we want to do is take a look at a two D.
02:51
Contour and how that can be used to finish off that inside pocket.
02:55
When we go to R.
02:56
Two D drop down and select two D contour,
02:58
we need to select a tool and in this case
03:00
our quarter inch flat end mill will work just fine
03:03
from our geometry selection we need to select a chain or a face that we want to use,
03:08
notice that we have our selected contours and pocket recognition.
03:12
We're going to use the selected contours option
03:14
and select the bottom edge of our pocket.
03:17
The red arrow is going to determine which side of that edge is going to be machined.
03:21
In this case we want to make sure it stays on the inside.
03:24
In the heights section,
03:25
this will automatically be done at the selected contour bottom height
03:30
for our passes with the two D contour, it's going to create a single pass
03:34
directly on that edge.
03:37
In this case it will offset it based on our tool
03:39
diameter because we're using a compensation type of in computer.
03:43
If we turn compensation off the center of the tool
03:45
will be directly on the center of our selection.
03:48
Other options such as in control where and in verse
03:51
where will put specific codes inside of your G.
03:53
Code when you post process your tool path.
03:56
This will allow you to make adjustments to the offset of
03:58
the tool path based on parameters set inside of your machines.
04:01
Control
04:03
in this example we're going to leave this on in computer but it's a good
04:06
idea for you to review these settings and which one is best for you.
04:09
You can always hover over a dialog box and take a look at the tool tips.
04:14
Next as we go down the line, notice that there's a finished feed rate.
04:17
We can make adjustments to these parameters
04:19
and determine if we want the finishing feed
04:22
rate to be faster or slower than the default feed rate of our tool.
04:25
In this case we're going to leave it at 72
04:28
next as we go down the list,
04:30
there are some other parameters such as overlap for the finishing lead out,
04:34
distance.
04:34
In this case it's called lead and distance.
04:37
Then we also have roughing passes multiple depths and stock to leave roughing
04:42
passes will allow us to make multiple
04:44
passes horizontally from the selected contour.
04:47
Multiple depths will allow us to make multiple cuts at different Z values and
04:51
stock to leave will determine how much material we want to leave on the wall
04:55
and are linking parameters. We have a ramping option
04:58
that allows us to use our selected contour and ramp the tool down at a specified angle
05:03
in this case, two degrees is the default,
05:05
which means that the tool will follow the external contour shape,
05:09
but it will be moving down at a two degree angle the entire time.
05:12
This can help with a consistent tool load
05:14
and prevent too much tulle burial into material.
05:17
If we say okay, the tool path is going to be created with a two D,
05:20
consistent ramp going down our selected contour
05:24
in the bottom section of our window,
05:26
I'm going to turn off the tool paths and note that
05:28
we have stock left at the bottom of our pocket.
05:31
Now part of this is because we didn't create a tool path in this case
05:35
are too deep pocket to remove all the material from the bottom of our part.
05:39
The two D. Adaptive was used as a roughing tool path. Only
05:43
in some cases you might determine that you want to use a two D.
05:46
Pocket instead of a two D contour simply because you want to
05:49
machine the bottom face of that pocket as well as the walls.
05:53
I'm going to right click on my two D contour and suppress it.
05:56
Say yes, Then I'm going to go back to my
05:59
pocket, right click and un suppress it and then drag it to the very bottom.
06:04
Under my two D. Adaptive, let's go ahead and edit R. Two D.
06:07
Pocket tool path in the past this section in
06:10
this case we want to turn off multiple depths.
06:13
We're going to machine the entire pocket at the maximum depth and say okay
06:17
this will allow us to create a tool path that will machine
06:20
the entire bottom of the pocket as well as all the walls.
06:23
You can go back and turn on your tool path,
06:25
visibility and see that our tool path is created only at the bottom,
06:29
notice also that it's creating two helical entries.
06:32
This is because we've got material left in the middle of our part,
06:35
we can always make adjustments to previous tool paths such as our adaptive cut,
06:40
Go to our stock to leave and instead of using a .02 radial stock to leave,
06:45
we can leave a smaller amount such as .005 and see if we
06:49
can get the tool to go all the way through the center.
06:52
It leaves a smaller amount of material here.
06:53
But we still have a potential problem using this size tool.
06:57
These are all things that we need to consider and just using a tool path like a two d.
07:01
Pocket doesn't necessarily mean that you can avoid these issues.
07:04
The tool will still go directly through that area and
07:06
we'll have a large tool load in those corners.
07:10
The next thing that we want to talk about is d burying the inside edges.
07:13
This is typically done with a two D champ for tool path,
07:16
there are two ways in which we can do this using R two D tool paths
07:20
contour has a chance for option. If you select a tool that's applicable for two D.
07:24
Champers
07:26
champers tool path itself has some additional options,
07:29
such as collision detection with surrounding geometry.
07:33
The first thing that we need to do is select an appropriate champ for mill tool.
07:36
We don't have any in our document or in our sample library.
07:40
So we need to go down into our fusion 3 60 library and we want
07:44
to make sure that we take a look at the engraved champ for mill type
07:48
from here. We need to select a tool that we want to use.
07:51
In this case we're going to go into our milling tools,
07:53
inch section and select the second tool which is 0.4 to five
07:56
inch 45 degree champ for we'll select this and say OK,
08:01
And next we'll move on to our geometry.
08:04
We're going to select the upper edge of the pocket.
08:06
Next we'll move into our passes and here's
08:08
where we're going to determine the champ for.
08:10
With this is going to be a relatively small chance for at .01 and we're going to
08:15
use a very small chance for tip offset because
08:18
we have a relatively large champ for tool.
08:20
We need to make sure that we're not pushing it too deep into the pocket
08:23
because we do have some collision areas that we need to be aware of.
08:27
Also note that we have a chance for clearance amount.
08:29
This is going to prevent the tool from intersecting with other solid geometry.
08:33
Once we say okay,
08:34
the tool will move around and create a chance for if we zoom in note that we're
08:38
not able to cut the champ for in the center because of the geometry of the tool,
08:43
this means that we would need to use a smaller
08:45
diameter tool in order to get into all these corners.
08:48
Infusion 3 60.
08:49
We can make adjustments to the tool or we could potentially
08:52
select another tool that could be used for this application.
08:56
If we select the tool that we want to use,
08:58
make sure that we are using engraved chant for tools.
09:01
Notice that inside of our sample library, we don't have anything available.
09:05
In some cases you might choose to use an engraved tool which will
09:08
allow you to get into those corners closer for this example however,
09:12
we're going to cancel and just note that we aren't able to
09:14
get all the way into those corners with the supplied tool.
09:18
The last thing that we need to do on this side of the part is drill and tap all the holes
09:22
for this. We're going to select drilling.
09:25
We're going to select our tool from our three axis
09:27
sample library which is going to be tool number one,
09:29
our spot drill and then we're going to select our holes in the geometry selection.
09:35
We have a couple options that we can use
09:37
selected faces points or diameter range for this selection.
09:41
I'm going to use the faces option and select the inside of each hole.
09:46
We're also going to move over to the heights
09:48
instead of going all the way to the bottom of
09:50
the hole because we are using a spot drill,
09:52
we're going to go to the whole top.
09:54
Then I'm going to use the drill tip through bottom option
09:57
which will allow us to just create a small spot.
10:00
Once the tool path is generated,
10:02
we can see a preview on the screen showing that small spot drill.
10:05
Next I'm going to right click on that tool path and I
10:08
want to duplicate it because we already have our whole selected.
10:11
We can simply duplicate the tool path,
10:13
change the tool that we want to use from our three access sample library.
10:17
In this case, a tool number to a .201 drill.
10:21
We're going to move on to the geometry,
10:23
make sure that all the holes are selected and then
10:26
to our heights instead of using our whole top,
10:28
we're going to use the whole bottom and still
10:30
allow the drill tip to go through the bottom.
10:32
We can also add a breakthrough depth.
10:34
If we want the tool to go a little bit farther in this case .05
10:39
last we want to set the cycle of the drill because we are doing more than just a spot.
10:43
We're going to be using a chip breaking cycle
10:46
that allows the drill bit to go in a small amount and then come back out a
10:49
little bit to allow the chips to clear and cool it to get into those holes.
10:53
This is especially important on deeper holes.
10:56
Next I'm going to create another drilling operation this time I
10:60
want to make sure that I'm using the tap tool.
11:02
We could simply duplicate the operation one more time.
11:06
However,
11:07
the tap tool has a slightly different approach to
11:09
how the geometry is going to be accounted for.
11:12
When we move over to our cycle,
11:14
notice that it automatically is set to tapping based on our tool selection.
11:18
If you duplicate a tool path and simply change to a tapping tool,
11:22
you need to make sure that you are using the tapping cycle.
11:25
This allows the tool to go in at a small feed rate and then it'll stop at
11:29
the bottom and reverse the tool back out of the hole to prevent damage to the threats.
11:34
In this case we're going to say,
11:35
okay and now we've created our tool paths for spot drilling,
11:39
drilling and tapping those holes
11:42
at this point let's go ahead and navigate back to a
11:44
home view and make sure that we saved before moving on
Video transcript
00:02
create tool paths. To finish cut parts.
00:05
After completing this video, you'll be able to create a facing tool path,
00:09
create a two D.
00:10
Contour tool path, create chance for and two D.
00:12
Contour champ for tool paths and create a drilling and tapping tool path
00:20
Infusion 3 60. We want to carry on with our mounting block part.
00:23
You have any difficulties in the last video.
00:25
Make sure that you upload the supply dataset mounting block rough dot F. Three Z.
00:30
At this point we've already created a two D. Pocket tool path and a two D.
00:34
Adaptive tool path to make sure that we
00:36
can identify the differences between the two.
00:38
But now we want to take a look at finishing tool paths.
00:42
Remember that the order of operations is typically dictated by the part
00:45
but in general you will use a facing tool path first.
00:48
Then you'll rough apart before you finish it.
00:51
In this case now we're going to go back and take a look at a
00:54
two D facing tool path and then we'll move on to some finishing tool paths.
00:58
Under the 2D dropdown will select face
01:01
and we need to select a tool for facing
01:03
when you're facing apart.
01:05
In some cases you might use a large end mill while in
01:08
other cases you might use a shell mill or a face mill.
01:11
In this example we're going to use a large three quarter end mill
01:15
under the geometry section fusion 3 60 will automatically bring in the
01:18
border or the outside shape of the stock used in your setup.
01:22
No selection is needed but you can select a different area if
01:25
you want to focus the tool on just a specific area.
01:28
However it's important to note that with a facing tool path,
01:31
the tool will always enter and exit the outside of your selection
01:36
for the heights fusion 3 60 will automatically pick the top height as the
01:40
stock top and the bottom height as the model top in the passes section.
01:44
You want to make sure that you dictate the
01:46
number of passes based on the step over amount.
01:49
In this case our tool is three quarters of an inch
01:51
so I'm going to go 30.7 inches between each step.
01:54
Once we say okay our passes are created in order to face the part
01:59
Infusion 3 60.
01:60
We can also take this facing tool path and we can drag it
02:03
all the way up to the top of our tool path list.
02:05
This means that even though it was created after our pocket and adaptive tool paths
02:10
it can be moved up in the line and that way we can have it at the very top.
02:14
Next I'm going to take my two D.
02:16
Pocket right click and suppress when I suppress the tool path,
02:20
it will still remain inside of our setup.
02:21
However,
02:22
it's no longer going to be used to calculate stock removal or any rest machining.
02:26
Now we have our original facing tool path and then we have our adaptive tool path.
02:32
Keep in mind our adaptive tool path has left material on the walls and the floors.
02:37
We need to make sure that we go back and we remove this material.
02:40
But remember that with the small size here we've got
02:43
a little bit of stock left in the middle.
02:44
And this is going to be an important consideration when planning our tool paths.
02:49
The next thing that we want to do is take a look at a two D.
02:51
Contour and how that can be used to finish off that inside pocket.
02:55
When we go to R.
02:56
Two D drop down and select two D contour,
02:58
we need to select a tool and in this case
03:00
our quarter inch flat end mill will work just fine
03:03
from our geometry selection we need to select a chain or a face that we want to use,
03:08
notice that we have our selected contours and pocket recognition.
03:12
We're going to use the selected contours option
03:14
and select the bottom edge of our pocket.
03:17
The red arrow is going to determine which side of that edge is going to be machined.
03:21
In this case we want to make sure it stays on the inside.
03:24
In the heights section,
03:25
this will automatically be done at the selected contour bottom height
03:30
for our passes with the two D contour, it's going to create a single pass
03:34
directly on that edge.
03:37
In this case it will offset it based on our tool
03:39
diameter because we're using a compensation type of in computer.
03:43
If we turn compensation off the center of the tool
03:45
will be directly on the center of our selection.
03:48
Other options such as in control where and in verse
03:51
where will put specific codes inside of your G.
03:53
Code when you post process your tool path.
03:56
This will allow you to make adjustments to the offset of
03:58
the tool path based on parameters set inside of your machines.
04:01
Control
04:03
in this example we're going to leave this on in computer but it's a good
04:06
idea for you to review these settings and which one is best for you.
04:09
You can always hover over a dialog box and take a look at the tool tips.
04:14
Next as we go down the line, notice that there's a finished feed rate.
04:17
We can make adjustments to these parameters
04:19
and determine if we want the finishing feed
04:22
rate to be faster or slower than the default feed rate of our tool.
04:25
In this case we're going to leave it at 72
04:28
next as we go down the list,
04:30
there are some other parameters such as overlap for the finishing lead out,
04:34
distance.
04:34
In this case it's called lead and distance.
04:37
Then we also have roughing passes multiple depths and stock to leave roughing
04:42
passes will allow us to make multiple
04:44
passes horizontally from the selected contour.
04:47
Multiple depths will allow us to make multiple cuts at different Z values and
04:51
stock to leave will determine how much material we want to leave on the wall
04:55
and are linking parameters. We have a ramping option
04:58
that allows us to use our selected contour and ramp the tool down at a specified angle
05:03
in this case, two degrees is the default,
05:05
which means that the tool will follow the external contour shape,
05:09
but it will be moving down at a two degree angle the entire time.
05:12
This can help with a consistent tool load
05:14
and prevent too much tulle burial into material.
05:17
If we say okay, the tool path is going to be created with a two D,
05:20
consistent ramp going down our selected contour
05:24
in the bottom section of our window,
05:26
I'm going to turn off the tool paths and note that
05:28
we have stock left at the bottom of our pocket.
05:31
Now part of this is because we didn't create a tool path in this case
05:35
are too deep pocket to remove all the material from the bottom of our part.
05:39
The two D. Adaptive was used as a roughing tool path. Only
05:43
in some cases you might determine that you want to use a two D.
05:46
Pocket instead of a two D contour simply because you want to
05:49
machine the bottom face of that pocket as well as the walls.
05:53
I'm going to right click on my two D contour and suppress it.
05:56
Say yes, Then I'm going to go back to my
05:59
pocket, right click and un suppress it and then drag it to the very bottom.
06:04
Under my two D. Adaptive, let's go ahead and edit R. Two D.
06:07
Pocket tool path in the past this section in
06:10
this case we want to turn off multiple depths.
06:13
We're going to machine the entire pocket at the maximum depth and say okay
06:17
this will allow us to create a tool path that will machine
06:20
the entire bottom of the pocket as well as all the walls.
06:23
You can go back and turn on your tool path,
06:25
visibility and see that our tool path is created only at the bottom,
06:29
notice also that it's creating two helical entries.
06:32
This is because we've got material left in the middle of our part,
06:35
we can always make adjustments to previous tool paths such as our adaptive cut,
06:40
Go to our stock to leave and instead of using a .02 radial stock to leave,
06:45
we can leave a smaller amount such as .005 and see if we
06:49
can get the tool to go all the way through the center.
06:52
It leaves a smaller amount of material here.
06:53
But we still have a potential problem using this size tool.
06:57
These are all things that we need to consider and just using a tool path like a two d.
07:01
Pocket doesn't necessarily mean that you can avoid these issues.
07:04
The tool will still go directly through that area and
07:06
we'll have a large tool load in those corners.
07:10
The next thing that we want to talk about is d burying the inside edges.
07:13
This is typically done with a two D champ for tool path,
07:16
there are two ways in which we can do this using R two D tool paths
07:20
contour has a chance for option. If you select a tool that's applicable for two D.
07:24
Champers
07:26
champers tool path itself has some additional options,
07:29
such as collision detection with surrounding geometry.
07:33
The first thing that we need to do is select an appropriate champ for mill tool.
07:36
We don't have any in our document or in our sample library.
07:40
So we need to go down into our fusion 3 60 library and we want
07:44
to make sure that we take a look at the engraved champ for mill type
07:48
from here. We need to select a tool that we want to use.
07:51
In this case we're going to go into our milling tools,
07:53
inch section and select the second tool which is 0.4 to five
07:56
inch 45 degree champ for we'll select this and say OK,
08:01
And next we'll move on to our geometry.
08:04
We're going to select the upper edge of the pocket.
08:06
Next we'll move into our passes and here's
08:08
where we're going to determine the champ for.
08:10
With this is going to be a relatively small chance for at .01 and we're going to
08:15
use a very small chance for tip offset because
08:18
we have a relatively large champ for tool.
08:20
We need to make sure that we're not pushing it too deep into the pocket
08:23
because we do have some collision areas that we need to be aware of.
08:27
Also note that we have a chance for clearance amount.
08:29
This is going to prevent the tool from intersecting with other solid geometry.
08:33
Once we say okay,
08:34
the tool will move around and create a chance for if we zoom in note that we're
08:38
not able to cut the champ for in the center because of the geometry of the tool,
08:43
this means that we would need to use a smaller
08:45
diameter tool in order to get into all these corners.
08:48
Infusion 3 60.
08:49
We can make adjustments to the tool or we could potentially
08:52
select another tool that could be used for this application.
08:56
If we select the tool that we want to use,
08:58
make sure that we are using engraved chant for tools.
09:01
Notice that inside of our sample library, we don't have anything available.
09:05
In some cases you might choose to use an engraved tool which will
09:08
allow you to get into those corners closer for this example however,
09:12
we're going to cancel and just note that we aren't able to
09:14
get all the way into those corners with the supplied tool.
09:18
The last thing that we need to do on this side of the part is drill and tap all the holes
09:22
for this. We're going to select drilling.
09:25
We're going to select our tool from our three axis
09:27
sample library which is going to be tool number one,
09:29
our spot drill and then we're going to select our holes in the geometry selection.
09:35
We have a couple options that we can use
09:37
selected faces points or diameter range for this selection.
09:41
I'm going to use the faces option and select the inside of each hole.
09:46
We're also going to move over to the heights
09:48
instead of going all the way to the bottom of
09:50
the hole because we are using a spot drill,
09:52
we're going to go to the whole top.
09:54
Then I'm going to use the drill tip through bottom option
09:57
which will allow us to just create a small spot.
10:00
Once the tool path is generated,
10:02
we can see a preview on the screen showing that small spot drill.
10:05
Next I'm going to right click on that tool path and I
10:08
want to duplicate it because we already have our whole selected.
10:11
We can simply duplicate the tool path,
10:13
change the tool that we want to use from our three access sample library.
10:17
In this case, a tool number to a .201 drill.
10:21
We're going to move on to the geometry,
10:23
make sure that all the holes are selected and then
10:26
to our heights instead of using our whole top,
10:28
we're going to use the whole bottom and still
10:30
allow the drill tip to go through the bottom.
10:32
We can also add a breakthrough depth.
10:34
If we want the tool to go a little bit farther in this case .05
10:39
last we want to set the cycle of the drill because we are doing more than just a spot.
10:43
We're going to be using a chip breaking cycle
10:46
that allows the drill bit to go in a small amount and then come back out a
10:49
little bit to allow the chips to clear and cool it to get into those holes.
10:53
This is especially important on deeper holes.
10:56
Next I'm going to create another drilling operation this time I
10:60
want to make sure that I'm using the tap tool.
11:02
We could simply duplicate the operation one more time.
11:06
However,
11:07
the tap tool has a slightly different approach to
11:09
how the geometry is going to be accounted for.
11:12
When we move over to our cycle,
11:14
notice that it automatically is set to tapping based on our tool selection.
11:18
If you duplicate a tool path and simply change to a tapping tool,
11:22
you need to make sure that you are using the tapping cycle.
11:25
This allows the tool to go in at a small feed rate and then it'll stop at
11:29
the bottom and reverse the tool back out of the hole to prevent damage to the threats.
11:34
In this case we're going to say,
11:35
okay and now we've created our tool paths for spot drilling,
11:39
drilling and tapping those holes
11:42
at this point let's go ahead and navigate back to a
11:44
home view and make sure that we saved before moving on
After completing this video, you will 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.