& Construction
![architecture engineering and construction collection logo](https://damassets.autodesk.net/content/dam/autodesk/www/universal-header/flyout/architecture-engineering-construction-collection-uhblack-banner-lockup-364x40.png)
Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
& Manufacturing
![product design manufacturing collection logo](https://damassets.autodesk.net/content/dam/autodesk/www/universal-header/flyout/product-design-manufacturing-collection-uhblack-banner-lockup-364x40.png)
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
00:03
In this video, you’ll: Apply toolpaths.
00:08
Open the file ToolContainment.f3d
00:12
There are different ways to contain toolpaths based on boundaries, height, slopes,
00:18
and whether they must touch or avoid surfaces.
00:22
These methods can also be combined.
00:26
In the Manufacturing workspace, in the Milling tab, from the ViewCube, click Home to orient the view properly.
00:34
Then, from the Browser, select Setup1.
00:39
This displays the setup stock and the Work Coordinate System,
00:44
as well as some of the surfacing toolpaths that have been already applied.
00:49
To begin, create a 3D Parallel toolpath.
00:54
Parallel toolpaths create finishing cuts in equally spaced rows.
00:60
From the Toolbar, expand 3D and select Parallel.
01:06
The Parallel dialog displays.
01:09
In the Tool tab, under Tool, next to Tool, click the selection tool.
01:15
This displays the Tool Library.
01:18
From the list of available libraries, under the Fusion 360 Library, select Sample Tools – Inch.
01:26
Then, under Filters, set the Tool category to Milling and the Type to Ball end mill.
01:35
From the updated list of Sample Tools, select 1/4 inch Ball Endmill.
01:42
Next, from the Cutting data presets list, select Aluminum – Finishing.
01:48
Click Select.
01:50
Back in the Parallel dialog, click OK.
01:53
Notice that the displayed toolpath covers the entire part and is not contained.
02:00
To contain the toolpath, from the Browser, right-click the toolpath Parallel1,
02:06
and then from the shortcut menu, select Edit.
02:11
First, contain the toolpath based on a boundary.
02:15
From the Parallel dialog, open the Geometry tab,
02:19
and then, under Geometry, expand the Machining Boundary drop-down.
02:25
Click Selection.
02:27
Now, on the model, pick the base edge of the first feature.
02:32
The toolpath will now be contained to the region within this selected boundary.
02:38
To configure the toolpath so it runs from front to back, open the Passes tab,
02:45
and under Passes, in the Pass Direction field, enter 90.
02:50
Next, specify the horizontal stepover between passes.
02:55
In the Stepover field, enter .02.
02:60
Click OK.
03:02
The toolpath updates and is contained to the region within the boundary selection.
03:07
Zoom into the region and orbit the view so you can review the toolpath.
03:14
Notice that there is excellent coverage in some areas, while other areas are lacking.
03:21
Copy the current toolpath to use it to derive a second toolpath.
03:27
From the Browser, right-click the toolpath, and from the shortcut menu,
03:32
select Create Derived Operation > 3D Milling > Contour.
03:38
Notice that Parallel is not selected.
03:42
The Contour dialog displays.
03:45
Open the Geometry tab and notice that the Machining Boundary Selection
03:50
has been inherited from the previous toolpath.
03:54
Open the Passes tab next.
03:57
The Maximum Stepdown, which specifies the maximum stepdown distance between Z-levels,
04:03
needs to be edited.
04:05
Under Passes, in the Maximum Stepdown field, enter .02.
04:11
Finally, open the Linking tab.
04:15
Here, you can configure how the tool moves.
04:19
Under Ramp, you can specify how the cutter moves down for each depth cut.
04:24
Currently, this is set to Helix, which would enter the stock in a helical motion.
04:31
Expand the Ramp Type drop-down and select Plunge.
04:35
This sets the toolpath to be a direct descent. Click OK.
04:40
The toolpath displays.
04:43
Notice that the steep areas have good coverage, but the flat areas are now lacking.
04:50
Toggle between the Parallel and the Contour toolpaths.
04:54
Because the Parallel toolpath has a stepover, it grants more coverage to flat surfaces.
05:01
Likewise, because the Contour toolpath has a stepdown, it grants more coverage to vertical surfaces.
05:09
To clear this up, you can contain the toolpaths to a slope angle.
05:14
From the Browser, edit the Parallel toolpath.
05:19
From the Parallel dialog, open the Geometry tab.
05:23
Enable Slope to access the Slope options.
05:28
Since the Parallel toolpath is best at machining flat surfaces,
05:33
contain the toolpath to areas that slope from 0 to 45 degrees.
05:39
To do this, leave the From Slope Angle set to 0 degrees,
05:45
but in the To Slope Angle field, enter 45.
05:49
Click OK.
05:51
In the canvas, the toolpath updates so that it is now contained by the defined slope range.
05:59
Next, edit the 3D Contour toolpath.
06:03
In the Contour dialog, open the Geometry tab, enable Slope,
06:08
and adjust the slope range to 40 to 90 degrees, which will allow some overlap of the toolpaths.
06:17
In the From Slope Angle field, enter 40.
06:21
Keep the To Slope Angle set to 90 degrees.
06:25
Click OK.
06:27
In the canvas, the updated toolpath displays.
06:31
To view both toolpaths simultaneously, from your keyboard, press CTRL and then,
06:39
in the Browser, select the Parallel toolpath.
06:43
Both toolpaths appear.
06:45
The entire part is covered using two different toolpaths.
06:50
Save the file.
06:52
Now, open the file Toolpath Containment2.f3d.
06:58
On the ViewCube, click Home to make sure the view is oriented properly.
07:03
From the Browser, click Setup1 to view the CAM setup.
07:08
Now, pick an edge of the concaved area of the model.
07:12
When you do, in the canvas, the measurement of the radius of the concave is reported to be 0.0625 inches.
07:24
To machine this, a 1/8 inch end mill is necessary.
07:30
From the Toolbar, expand the 3D drop-down, and select Parallel.
07:36
The Parallel dialog displays again.
07:39
From the Tool tab, click the selection tool to open the Tool Library.
07:45
Again, from the list of available libraries, under the Fusion 360 Library,
07:51
select Sample Tools – Inch.
07:55
In the Filters panel, set the Tool category to Milling, and the Type to Ball end mill.
08:03
From the updated Sample Tools list, select 1/8 inch Ball Endmill.
08:10
From the Cutting data presets list, select Aluminum – Finishing.
08:14
Now, click Select.
08:17
Back in the Parallel dialog, open the Geometry tab.
08:22
Leave the configurations as they are for now.
08:26
Next, open the Heights tab.
08:28
Again, leave the settings as is.
08:32
Open the Passes tab.
08:34
Under Passes, in the Pass Direction field, enter 90.
08:40
This will set the pass direction to 90 degrees.
08:44
Next, in the Stepover field, enter .02.
08:49
Now, open the Linking tab to configure how the tool moves.
08:54
Expand the Retraction Policy drop-down and select Minimum Retraction.
08:59
When set to Minimum Retraction, the tool moves directly to the safest, lowest height where the tool clears the workpiece.
09:08
Click OK.
09:10
Again, this toolpath has not yet been contained.
09:14
To contain it based on height, edit the Parallel toolpath.
09:20
In the Parallel dialog, open the Heights tab.
09:24
Under Top Height, you can set the height for the top of the cut,
09:28
which should always be set above the Bottom height.
09:33
Top height is used with the subsequent offset to establish the height.
09:38
Expand the From drop-down and choose Selection.
09:43
Then in the canvas, pick an edge at the base of the top fillet.
09:48
Under Bottom Height, expand the From drop-down and click Selection.
09:55
Now, in the canvas, pick an edge on a bottom fillet.
09:59
Click OK.
10:01
The toolpath updates and is contained to where the tool can fit.
10:06
To further refine the toolpath, from the Browser, edit it again.
10:11
In the Parallel dialog, open the Heights tab again, and this time, under Bottom Height, set From to Model bottom.
10:22
Click OK.
10:25
Notice that the toolpath extends down the model.
10:29
Edit the toolpath .
10:31
In the Parallel dialog, open the Geometry tab and enable Avoid/Touch Surfaces.
10:39
When this option is enabled, toolpaths ignore selected surfaces.
10:44
However, you can also configure it to only touch certain surfaces.
10:50
Next to Avoid/Touch Surfaces, click the selection tool
10:55
and then select the faces of the model you want it to avoid.
11:01
In this instance, select the top of the model, the fillets, and the steep walls.
11:08
Click OK.
11:10
The toolpath updates.
11:13
To add more faces to avoid, edit the toolpath again.
11:18
Once more from the Geometry tab, click the Avoid/Touch Surfaces tool selection, and then select any additional faces.
11:29
Click OK.
11:31
Now the toolpath is entirely contained.
11:34
Save the file.
11:36
Toolpaths can be contained in a variety of ways,
11:40
using the model boundaries, height, slopes, and whether they must touch or avoid surfaces.
Video transcript
00:03
In this video, you’ll: Apply toolpaths.
00:08
Open the file ToolContainment.f3d
00:12
There are different ways to contain toolpaths based on boundaries, height, slopes,
00:18
and whether they must touch or avoid surfaces.
00:22
These methods can also be combined.
00:26
In the Manufacturing workspace, in the Milling tab, from the ViewCube, click Home to orient the view properly.
00:34
Then, from the Browser, select Setup1.
00:39
This displays the setup stock and the Work Coordinate System,
00:44
as well as some of the surfacing toolpaths that have been already applied.
00:49
To begin, create a 3D Parallel toolpath.
00:54
Parallel toolpaths create finishing cuts in equally spaced rows.
00:60
From the Toolbar, expand 3D and select Parallel.
01:06
The Parallel dialog displays.
01:09
In the Tool tab, under Tool, next to Tool, click the selection tool.
01:15
This displays the Tool Library.
01:18
From the list of available libraries, under the Fusion 360 Library, select Sample Tools – Inch.
01:26
Then, under Filters, set the Tool category to Milling and the Type to Ball end mill.
01:35
From the updated list of Sample Tools, select 1/4 inch Ball Endmill.
01:42
Next, from the Cutting data presets list, select Aluminum – Finishing.
01:48
Click Select.
01:50
Back in the Parallel dialog, click OK.
01:53
Notice that the displayed toolpath covers the entire part and is not contained.
02:00
To contain the toolpath, from the Browser, right-click the toolpath Parallel1,
02:06
and then from the shortcut menu, select Edit.
02:11
First, contain the toolpath based on a boundary.
02:15
From the Parallel dialog, open the Geometry tab,
02:19
and then, under Geometry, expand the Machining Boundary drop-down.
02:25
Click Selection.
02:27
Now, on the model, pick the base edge of the first feature.
02:32
The toolpath will now be contained to the region within this selected boundary.
02:38
To configure the toolpath so it runs from front to back, open the Passes tab,
02:45
and under Passes, in the Pass Direction field, enter 90.
02:50
Next, specify the horizontal stepover between passes.
02:55
In the Stepover field, enter .02.
02:60
Click OK.
03:02
The toolpath updates and is contained to the region within the boundary selection.
03:07
Zoom into the region and orbit the view so you can review the toolpath.
03:14
Notice that there is excellent coverage in some areas, while other areas are lacking.
03:21
Copy the current toolpath to use it to derive a second toolpath.
03:27
From the Browser, right-click the toolpath, and from the shortcut menu,
03:32
select Create Derived Operation > 3D Milling > Contour.
03:38
Notice that Parallel is not selected.
03:42
The Contour dialog displays.
03:45
Open the Geometry tab and notice that the Machining Boundary Selection
03:50
has been inherited from the previous toolpath.
03:54
Open the Passes tab next.
03:57
The Maximum Stepdown, which specifies the maximum stepdown distance between Z-levels,
04:03
needs to be edited.
04:05
Under Passes, in the Maximum Stepdown field, enter .02.
04:11
Finally, open the Linking tab.
04:15
Here, you can configure how the tool moves.
04:19
Under Ramp, you can specify how the cutter moves down for each depth cut.
04:24
Currently, this is set to Helix, which would enter the stock in a helical motion.
04:31
Expand the Ramp Type drop-down and select Plunge.
04:35
This sets the toolpath to be a direct descent. Click OK.
04:40
The toolpath displays.
04:43
Notice that the steep areas have good coverage, but the flat areas are now lacking.
04:50
Toggle between the Parallel and the Contour toolpaths.
04:54
Because the Parallel toolpath has a stepover, it grants more coverage to flat surfaces.
05:01
Likewise, because the Contour toolpath has a stepdown, it grants more coverage to vertical surfaces.
05:09
To clear this up, you can contain the toolpaths to a slope angle.
05:14
From the Browser, edit the Parallel toolpath.
05:19
From the Parallel dialog, open the Geometry tab.
05:23
Enable Slope to access the Slope options.
05:28
Since the Parallel toolpath is best at machining flat surfaces,
05:33
contain the toolpath to areas that slope from 0 to 45 degrees.
05:39
To do this, leave the From Slope Angle set to 0 degrees,
05:45
but in the To Slope Angle field, enter 45.
05:49
Click OK.
05:51
In the canvas, the toolpath updates so that it is now contained by the defined slope range.
05:59
Next, edit the 3D Contour toolpath.
06:03
In the Contour dialog, open the Geometry tab, enable Slope,
06:08
and adjust the slope range to 40 to 90 degrees, which will allow some overlap of the toolpaths.
06:17
In the From Slope Angle field, enter 40.
06:21
Keep the To Slope Angle set to 90 degrees.
06:25
Click OK.
06:27
In the canvas, the updated toolpath displays.
06:31
To view both toolpaths simultaneously, from your keyboard, press CTRL and then,
06:39
in the Browser, select the Parallel toolpath.
06:43
Both toolpaths appear.
06:45
The entire part is covered using two different toolpaths.
06:50
Save the file.
06:52
Now, open the file Toolpath Containment2.f3d.
06:58
On the ViewCube, click Home to make sure the view is oriented properly.
07:03
From the Browser, click Setup1 to view the CAM setup.
07:08
Now, pick an edge of the concaved area of the model.
07:12
When you do, in the canvas, the measurement of the radius of the concave is reported to be 0.0625 inches.
07:24
To machine this, a 1/8 inch end mill is necessary.
07:30
From the Toolbar, expand the 3D drop-down, and select Parallel.
07:36
The Parallel dialog displays again.
07:39
From the Tool tab, click the selection tool to open the Tool Library.
07:45
Again, from the list of available libraries, under the Fusion 360 Library,
07:51
select Sample Tools – Inch.
07:55
In the Filters panel, set the Tool category to Milling, and the Type to Ball end mill.
08:03
From the updated Sample Tools list, select 1/8 inch Ball Endmill.
08:10
From the Cutting data presets list, select Aluminum – Finishing.
08:14
Now, click Select.
08:17
Back in the Parallel dialog, open the Geometry tab.
08:22
Leave the configurations as they are for now.
08:26
Next, open the Heights tab.
08:28
Again, leave the settings as is.
08:32
Open the Passes tab.
08:34
Under Passes, in the Pass Direction field, enter 90.
08:40
This will set the pass direction to 90 degrees.
08:44
Next, in the Stepover field, enter .02.
08:49
Now, open the Linking tab to configure how the tool moves.
08:54
Expand the Retraction Policy drop-down and select Minimum Retraction.
08:59
When set to Minimum Retraction, the tool moves directly to the safest, lowest height where the tool clears the workpiece.
09:08
Click OK.
09:10
Again, this toolpath has not yet been contained.
09:14
To contain it based on height, edit the Parallel toolpath.
09:20
In the Parallel dialog, open the Heights tab.
09:24
Under Top Height, you can set the height for the top of the cut,
09:28
which should always be set above the Bottom height.
09:33
Top height is used with the subsequent offset to establish the height.
09:38
Expand the From drop-down and choose Selection.
09:43
Then in the canvas, pick an edge at the base of the top fillet.
09:48
Under Bottom Height, expand the From drop-down and click Selection.
09:55
Now, in the canvas, pick an edge on a bottom fillet.
09:59
Click OK.
10:01
The toolpath updates and is contained to where the tool can fit.
10:06
To further refine the toolpath, from the Browser, edit it again.
10:11
In the Parallel dialog, open the Heights tab again, and this time, under Bottom Height, set From to Model bottom.
10:22
Click OK.
10:25
Notice that the toolpath extends down the model.
10:29
Edit the toolpath .
10:31
In the Parallel dialog, open the Geometry tab and enable Avoid/Touch Surfaces.
10:39
When this option is enabled, toolpaths ignore selected surfaces.
10:44
However, you can also configure it to only touch certain surfaces.
10:50
Next to Avoid/Touch Surfaces, click the selection tool
10:55
and then select the faces of the model you want it to avoid.
11:01
In this instance, select the top of the model, the fillets, and the steep walls.
11:08
Click OK.
11:10
The toolpath updates.
11:13
To add more faces to avoid, edit the toolpath again.
11:18
Once more from the Geometry tab, click the Avoid/Touch Surfaces tool selection, and then select any additional faces.
11:29
Click OK.
11:31
Now the toolpath is entirely contained.
11:34
Save the file.
11:36
Toolpaths can be contained in a variety of ways,
11:40
using the model boundaries, height, slopes, and whether they must touch or avoid surfaces.
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.