Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
Professional CAD/CAM tools built on Inventor and AutoCAD
In this exercise, you'll practice how to strategize toolpaths, configure toolpath parameters, and prepare toolpaths for a part.
Exercise
Transcript
00:00
Creating and optimizing toolpaths is critical for the success of turning.
00:09
With the file Turning Practice.f3d open, ensure that the setup has been created.
00:16
Now, you must select the appropriate toolpath strategy, adjust the toolpath parameters,
00:23
and then determine specific strategies to optimize various toolpaths.
00:29
First, choose the tool that you want to use for the facing operation.
00:34
With the Manufacture workspace active, start the Turning Face tool.
00:40
A dialog for Face3 opens.
00:44
Click the selection prompt to open the Select Tool dialog.
00:49
On the left panel, a selection tree displays with all the available locations from which to select a tool.
00:57
For this example, open the Cloud library to access the Practice library, which contains the tools for this exercise.
01:06
In the right panel, a list of tools displays.
01:11
Select the first tool.
01:13
Now, in the canvas, pan and zoom the part.
01:18
Notice that the stock profile does not go far enough out,
01:22
and that you can see things like the counterbore for the hole that is going through the part, which should not be visible.
01:31
You need to make adjustments to resolve these issues.
01:34
Select the part in the Browser and enable the Spun profile option.
01:40
Then, repeat the same Turning Face toolpath with spun profile enabled.
01:47
This time, in the Select Tool dialog, you can see in the left panel that the tool you previously selected is now under Documents.
01:57
Select it.
01:59
Now, in the canvas, with spun profile enabled, you can see the proper outside profile of the part.
02:07
Notice also that a facing toolpath appears on the front of the part.
02:13
Now, it is time to add the profile roughing toolpath.
02:18
From the Toolbar, this time when you expand the Turning drop-down, click Turning Profile Roughing.
02:25
A dialog for Profile Roughing2 opens.
02:30
Open the Geometry tab.
02:33
Under Back, in the Offset field, type “-.375”.
02:40
Then, open the rest of the tabs and review the information in each to ensure that the profile roughing operation is configured correctly.
02:50
Click OK.
02:53
In the canvas, the profile roughing toolpath appears on the part.
02:58
Pan and zoom to examine the toolpath.
03:02
Note that it dives down between the two faces and behind the part, so you need to make adjustments.
03:10
In the Browser, under Setup1, edit the profile roughing operation.
03:16
The Profile Roughing dialog displays again.
03:20
Open the Passes tab, and, under Cycle and direction, expand the drop-down next to Grooving and select Don’t allow grooving.
03:32
Click OK.
03:34
In the canvas, notice that the toolpath has been corrected.
03:39
Now it is time to profile finish the part.
03:43
Instead of starting from scratch, you can derive the finishing toolpath from the roughing toolpath.
03:50
Right-click the profile roughing operation and select Create Derived Operation > Turning > Turning Profile Finishing.
04:01
A dialog opens for Profile Finishing2.
04:06
Now you can select the finishing tools for this new toolpath.
04:11
In the Select Tool dialog, in the left panel, expand Cloud and click the Practice library.
04:19
Then, in the right panel, click Tool #6.
04:24
Click Select.
04:27
Back in the Profile Finishing dialog, open each tab to review the toolpath parameters.
04:34
Click OK.
04:36
In the canvas, the finishing toolpath displays on the part.
04:40
In the Browser, next to the profile finishing operation, a warning appears.
04:47
Click it, and the warning dialog informs that the “Lead-Out has been modified due to a gouge with the remaining stock”.
04:56
This indicates that Fusion has changed the lead-out value so that you do not have to continue into the stock.
05:04
You could shorten that if you wanted to, or change the layout, but, for this example, leave the settings as they are.
05:13
Now it is time to groove out the material between the flanges.
05:17
On the Toolbar, expand the Turning drop-down and click Turning Groove.
05:23
A dialog for Groove2 opens.
05:27
Again, open the Practice library, and this time, select Tool #3, which is a grooving tool.
05:34
Click Select.
05:37
In the Groove dialog, click OK.
05:40
In the canvas, the toolpath displays on the part.
05:45
Notice that the toolpath grooves the part entirely from front to back when it should be grooving out only between the flanges,
05:53
so you need to make some adjustments.
05:56
In the Browser, edit the grooving toolpath to open the Groove2 dialog again.
06:03
Choose a confinement for the grooving operation by selecting the faces of the flanges
06:08
to indicate the front and back of the grooving toolpath.
06:13
On the Geometry tab, under Front, expand the Front Mode drop-down and click Selection to activate the selection tool.
06:24
In the canvas, select the inside of the flange in the front.
06:29
In the dialog, the selection tool changes to indicate that a Face has been selected.
06:35
Repeat the process and select the back flange.
06:40
Under Back, expand the Back Mode drop-down and click Selection to activate the selection tool.
06:48
In the canvas, select the other side of the flange face.
06:54
In the dialog, the selection tool changes to indicate that a Face has been selected.
07:00
Click OK.
07:03
In the canvas, zoom in on the toolpath.
07:07
Notice how the adjustments have yielded a better result.
07:11
However, the tool is still going beyond the bounds a little, and it is starting higher than is preferable,
07:18
so you need to make another adjustment.
07:21
Again, in the Browser, edit the grooving operation.
07:25
In the Groove dialog, on the Geometry tab, enable the checkbox next to Rest Machining.
07:33
This machines the rest of the leftover stock after the previous operations.
07:38
Now, in the canvas, you can see that the toolpath is much better contained between the two faces.
07:46
Since you are still using the grooving tool, this is a good time to add the chamfers that were called out on the model.
07:54
In the Chamfer1 dialog, on the Geometry tab, next to Chamfers, you can see that Nothing has been selected.
08:05
Click the selection prompt.
08:08
In the canvas, click the outside edges where you want the chamfers to go.
08:13
In the dialog, the selection prompt changes to indicate that 3 Edges have been selected.
08:21
Open the Passes tab.
08:24
In the Chamfer Width field, type “.015”.
08:29
Click OK.
08:31
Now, you have the proper chamfer values to deburr the part as called out on the print.
08:37
Next, you need to drill the part.
08:41
On the Toolbar, in the Drilling panel, click Drill.
08:47
In the Drill1 dialog, click the selection prompt to add a drilling tool.
08:53
In the Select Tool dialog, click the Fusion 360 Library.
08:58
In the right panel, under Tool category, select Hole making, and under Type, enable the Drill option.
09:08
In the center panel, look for drill that is three-quarters of an inch in diameter.
09:14
To make the search easier, in the right panel, expand Diameter and, in the text field, type “.75 in”.
09:24
In the center panel, a tool is listed that meets these criteria.
09:29
Click the tool, then click Select.
09:34
Open the Geometry tab.
09:36
In the canvas, click the hole face.
09:40
Next to Hole faces, the selection prompt changes to indicate that a Face has been selected.
09:47
Open the Heights tab.
09:50
Set the Top Height to From > Model top, and then set the Bottom Height to Drill Tip Through Bottom.
09:60
In the Break-Through Depth field that appears below, type “.1”.
10:05
Open the Cycle tab.
10:08
Set the Cycle Type to Chip breaking – partial retract, and then click OK.
10:16
Next, add a boring operation to the front of the drilled inner diameter.
10:21
Start the Turning profile roughing tool again, and then in the Profile Roughing dialog, click the selection prompt.
10:30
In the Select Tool dialog, click the Practice library, select Tool #2, and then click Select.
10:40
Open the Geometry tab.
10:43
Indicate the boring operation to start at the front of the model and extend back only to the inside face in the bore.
10:52
In the dialog, open the Radii tab.
10:56
Use model selections to indicate the desired clearance diameter, then offset it by -.05.
11:05
Also select geometry to indicate the inner radius and outer radius.
11:11
In the canvas, pan and zoom the part and observe that the boring toolpath has been added.
11:22
The last thing to do is to add the parting toolpath.
11:27
Select Turning Part, and in the Part1 dialog, click the selection prompt, choose the Practice library again, and then choose Tool #4.
11:40
Click Select.
11:43
Back in the dialog, open each tab to review the parameters for the toolpath.
11:49
Click OK.
11:51
Now, all the toolpaths needed to make this part have been added.
Video transcript
00:00
Creating and optimizing toolpaths is critical for the success of turning.
00:09
With the file Turning Practice.f3d open, ensure that the setup has been created.
00:16
Now, you must select the appropriate toolpath strategy, adjust the toolpath parameters,
00:23
and then determine specific strategies to optimize various toolpaths.
00:29
First, choose the tool that you want to use for the facing operation.
00:34
With the Manufacture workspace active, start the Turning Face tool.
00:40
A dialog for Face3 opens.
00:44
Click the selection prompt to open the Select Tool dialog.
00:49
On the left panel, a selection tree displays with all the available locations from which to select a tool.
00:57
For this example, open the Cloud library to access the Practice library, which contains the tools for this exercise.
01:06
In the right panel, a list of tools displays.
01:11
Select the first tool.
01:13
Now, in the canvas, pan and zoom the part.
01:18
Notice that the stock profile does not go far enough out,
01:22
and that you can see things like the counterbore for the hole that is going through the part, which should not be visible.
01:31
You need to make adjustments to resolve these issues.
01:34
Select the part in the Browser and enable the Spun profile option.
01:40
Then, repeat the same Turning Face toolpath with spun profile enabled.
01:47
This time, in the Select Tool dialog, you can see in the left panel that the tool you previously selected is now under Documents.
01:57
Select it.
01:59
Now, in the canvas, with spun profile enabled, you can see the proper outside profile of the part.
02:07
Notice also that a facing toolpath appears on the front of the part.
02:13
Now, it is time to add the profile roughing toolpath.
02:18
From the Toolbar, this time when you expand the Turning drop-down, click Turning Profile Roughing.
02:25
A dialog for Profile Roughing2 opens.
02:30
Open the Geometry tab.
02:33
Under Back, in the Offset field, type “-.375”.
02:40
Then, open the rest of the tabs and review the information in each to ensure that the profile roughing operation is configured correctly.
02:50
Click OK.
02:53
In the canvas, the profile roughing toolpath appears on the part.
02:58
Pan and zoom to examine the toolpath.
03:02
Note that it dives down between the two faces and behind the part, so you need to make adjustments.
03:10
In the Browser, under Setup1, edit the profile roughing operation.
03:16
The Profile Roughing dialog displays again.
03:20
Open the Passes tab, and, under Cycle and direction, expand the drop-down next to Grooving and select Don’t allow grooving.
03:32
Click OK.
03:34
In the canvas, notice that the toolpath has been corrected.
03:39
Now it is time to profile finish the part.
03:43
Instead of starting from scratch, you can derive the finishing toolpath from the roughing toolpath.
03:50
Right-click the profile roughing operation and select Create Derived Operation > Turning > Turning Profile Finishing.
04:01
A dialog opens for Profile Finishing2.
04:06
Now you can select the finishing tools for this new toolpath.
04:11
In the Select Tool dialog, in the left panel, expand Cloud and click the Practice library.
04:19
Then, in the right panel, click Tool #6.
04:24
Click Select.
04:27
Back in the Profile Finishing dialog, open each tab to review the toolpath parameters.
04:34
Click OK.
04:36
In the canvas, the finishing toolpath displays on the part.
04:40
In the Browser, next to the profile finishing operation, a warning appears.
04:47
Click it, and the warning dialog informs that the “Lead-Out has been modified due to a gouge with the remaining stock”.
04:56
This indicates that Fusion has changed the lead-out value so that you do not have to continue into the stock.
05:04
You could shorten that if you wanted to, or change the layout, but, for this example, leave the settings as they are.
05:13
Now it is time to groove out the material between the flanges.
05:17
On the Toolbar, expand the Turning drop-down and click Turning Groove.
05:23
A dialog for Groove2 opens.
05:27
Again, open the Practice library, and this time, select Tool #3, which is a grooving tool.
05:34
Click Select.
05:37
In the Groove dialog, click OK.
05:40
In the canvas, the toolpath displays on the part.
05:45
Notice that the toolpath grooves the part entirely from front to back when it should be grooving out only between the flanges,
05:53
so you need to make some adjustments.
05:56
In the Browser, edit the grooving toolpath to open the Groove2 dialog again.
06:03
Choose a confinement for the grooving operation by selecting the faces of the flanges
06:08
to indicate the front and back of the grooving toolpath.
06:13
On the Geometry tab, under Front, expand the Front Mode drop-down and click Selection to activate the selection tool.
06:24
In the canvas, select the inside of the flange in the front.
06:29
In the dialog, the selection tool changes to indicate that a Face has been selected.
06:35
Repeat the process and select the back flange.
06:40
Under Back, expand the Back Mode drop-down and click Selection to activate the selection tool.
06:48
In the canvas, select the other side of the flange face.
06:54
In the dialog, the selection tool changes to indicate that a Face has been selected.
07:00
Click OK.
07:03
In the canvas, zoom in on the toolpath.
07:07
Notice how the adjustments have yielded a better result.
07:11
However, the tool is still going beyond the bounds a little, and it is starting higher than is preferable,
07:18
so you need to make another adjustment.
07:21
Again, in the Browser, edit the grooving operation.
07:25
In the Groove dialog, on the Geometry tab, enable the checkbox next to Rest Machining.
07:33
This machines the rest of the leftover stock after the previous operations.
07:38
Now, in the canvas, you can see that the toolpath is much better contained between the two faces.
07:46
Since you are still using the grooving tool, this is a good time to add the chamfers that were called out on the model.
07:54
In the Chamfer1 dialog, on the Geometry tab, next to Chamfers, you can see that Nothing has been selected.
08:05
Click the selection prompt.
08:08
In the canvas, click the outside edges where you want the chamfers to go.
08:13
In the dialog, the selection prompt changes to indicate that 3 Edges have been selected.
08:21
Open the Passes tab.
08:24
In the Chamfer Width field, type “.015”.
08:29
Click OK.
08:31
Now, you have the proper chamfer values to deburr the part as called out on the print.
08:37
Next, you need to drill the part.
08:41
On the Toolbar, in the Drilling panel, click Drill.
08:47
In the Drill1 dialog, click the selection prompt to add a drilling tool.
08:53
In the Select Tool dialog, click the Fusion 360 Library.
08:58
In the right panel, under Tool category, select Hole making, and under Type, enable the Drill option.
09:08
In the center panel, look for drill that is three-quarters of an inch in diameter.
09:14
To make the search easier, in the right panel, expand Diameter and, in the text field, type “.75 in”.
09:24
In the center panel, a tool is listed that meets these criteria.
09:29
Click the tool, then click Select.
09:34
Open the Geometry tab.
09:36
In the canvas, click the hole face.
09:40
Next to Hole faces, the selection prompt changes to indicate that a Face has been selected.
09:47
Open the Heights tab.
09:50
Set the Top Height to From > Model top, and then set the Bottom Height to Drill Tip Through Bottom.
09:60
In the Break-Through Depth field that appears below, type “.1”.
10:05
Open the Cycle tab.
10:08
Set the Cycle Type to Chip breaking – partial retract, and then click OK.
10:16
Next, add a boring operation to the front of the drilled inner diameter.
10:21
Start the Turning profile roughing tool again, and then in the Profile Roughing dialog, click the selection prompt.
10:30
In the Select Tool dialog, click the Practice library, select Tool #2, and then click Select.
10:40
Open the Geometry tab.
10:43
Indicate the boring operation to start at the front of the model and extend back only to the inside face in the bore.
10:52
In the dialog, open the Radii tab.
10:56
Use model selections to indicate the desired clearance diameter, then offset it by -.05.
11:05
Also select geometry to indicate the inner radius and outer radius.
11:11
In the canvas, pan and zoom the part and observe that the boring toolpath has been added.
11:22
The last thing to do is to add the parting toolpath.
11:27
Select Turning Part, and in the Part1 dialog, click the selection prompt, choose the Practice library again, and then choose Tool #4.
11:40
Click Select.
11:43
Back in the dialog, open each tab to review the parameters for the toolpath.
11:49
Click OK.
11:51
Now, all the toolpaths needed to make this part have been added.
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.