Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
Professional CAD/CAM tools built on Inventor and AutoCAD
Multiple cuts and lead in/lead out.
Type:
Tutorial
Length:
7 min.
Transcript
00:03
Turning Finishing is a toolpath strategy used for finishing the Outside Diameter (OD) or Inside Diameter (ID) of the part.
00:12
You can control the step per cut, stock amounts, cut direction, starting position, and cut extensions.
00:21
This strategy removes stock to produce the required shape and surface finish of the part
00:26
and includes shallower cuts at the slower feed rate than cuts in the Profile Roughing toolpath.
00:31
From the Manufacture workspace toolbar, Turning tab, Turning group, click Turning Profile Finishing.
00:40
In the Profile Finishing dialog, on the Tool tab, click Select to choose a tool.
00:45
In the Tool Library, expand Fusion Library, select the Turning Tools (Inch) folder,
00:52
from the tool list, choose the VNMT09T302 - Right Hand tool.
00:59
Click Select.
01:01
The VNMT Insert configuration is a common insert shape for finishing.
01:06
In the Feed & Speed group of the Tool tab, select Use Constant Surface Speed to set the cut rate,
01:12
or deselect it to set an actual spindle speed and feed rate.
01:16
Most lathe programmers want to use constant surface speed,
01:19
and enter the surface speed and the cutting feed per revolution to determine their speeds and feeds.
01:25
For this example, leave the default Feed & Speed settings.
01:30
Switch to the Geometry tab to select the front and back areas to be machined.
01:35
The dialog shows that the front mode is set in reference to the Model front,
01:39
which is good, since the front of the stock was already faced off.
01:43
The back mode is set in reference to the Model back.
01:47
You want to cut past the back of the model;
01:49
and since you will require a parting operation later that will use a 1/4 inch wide cut off tool, set the Offset value to –0.3 inches.
01:59
Switch to the Radii tab.
02:02
Here, you can set clearance positions and cutting areas radially across X.
02:07
The clearance height is the fully retracted position outside the part.
02:12
It represents the safest retract for the first rapid position and the last height after the toolpath has been completed.
02:19
The From reference is set to the Stock OD and the offset is set to 0.4 inches.
02:25
There is plenty of clearance to the outside of the stock.
02:29
The outer radius represents the outer surface of the stock to be machined.
02:34
For this, the From reference is set to the Stock OD, and the offset is set to 0.
02:40
The inner radius is the final cut depth in X.
02:43
Even though the from reference is set to the Stock ID, the tool will never get to the part center line.
02:50
It cuts everything within this boundary that can be cut without violating the part model.
02:55
There is nothing to change here.
02:58
Switch to the Passes tab.
03:00
To prevent dipping into the open groove areas, set the Grooving parameter to Don't allow grooving.
03:06
The Stepover amount per cut is set to .0393, but since the Number of Stepovers is set to 1, it will simply take a single finish pass.
03:16
The settings on the Linking tab control what will happen between cuts when the tool needs to retract and reposition.
03:23
For this example, there is nothing to change right now, so click OK to generate the profile finishing toolpath.
03:30
Zoom in to the back of the part.
03:33
In the Browser, notice the warning for the toolpath.
03:37
Click the warning symbol to show more information.
03:40
In this case, Fusion had to modify the toolpath to make it safe.
03:45
The lead out has been modified due to a gouge with the remaining stock.
03:50
Close the warning message.
03:52
Right-click the toolpath operation and select Edit.
03:57
In the Profile Finishing dialog, switch to the Linking tab.
04:01
Here, in the Leads & Transitions group, you see that the Linear Lead-In Angle is set to 45° from where the toolpath ends.
04:10
If it moves at 45°, it will collide with the stock.
04:14
There are two ways to fix this.
04:17
Option 1: If you absolutely cannot violate the stock area, uncheck Same As Lead-In and change the Linear Lead-Out Angle to 90°.
04:27
Option 2: If it is OK to cut the remaining stock, the simpler way is to check Allow Lead to Cut Stock.
04:34
Then, Fusion will permit the lead out move to enter the stock area.
04:39
For this example, check Allow Lead to Cut Stock, and then click OK.
04:44
The profile finishing toolpath is re-generated and there is no longer a warning.
04:49
Save your model if you want to continue working on it.
Video transcript
00:03
Turning Finishing is a toolpath strategy used for finishing the Outside Diameter (OD) or Inside Diameter (ID) of the part.
00:12
You can control the step per cut, stock amounts, cut direction, starting position, and cut extensions.
00:21
This strategy removes stock to produce the required shape and surface finish of the part
00:26
and includes shallower cuts at the slower feed rate than cuts in the Profile Roughing toolpath.
00:31
From the Manufacture workspace toolbar, Turning tab, Turning group, click Turning Profile Finishing.
00:40
In the Profile Finishing dialog, on the Tool tab, click Select to choose a tool.
00:45
In the Tool Library, expand Fusion Library, select the Turning Tools (Inch) folder,
00:52
from the tool list, choose the VNMT09T302 - Right Hand tool.
00:59
Click Select.
01:01
The VNMT Insert configuration is a common insert shape for finishing.
01:06
In the Feed & Speed group of the Tool tab, select Use Constant Surface Speed to set the cut rate,
01:12
or deselect it to set an actual spindle speed and feed rate.
01:16
Most lathe programmers want to use constant surface speed,
01:19
and enter the surface speed and the cutting feed per revolution to determine their speeds and feeds.
01:25
For this example, leave the default Feed & Speed settings.
01:30
Switch to the Geometry tab to select the front and back areas to be machined.
01:35
The dialog shows that the front mode is set in reference to the Model front,
01:39
which is good, since the front of the stock was already faced off.
01:43
The back mode is set in reference to the Model back.
01:47
You want to cut past the back of the model;
01:49
and since you will require a parting operation later that will use a 1/4 inch wide cut off tool, set the Offset value to –0.3 inches.
01:59
Switch to the Radii tab.
02:02
Here, you can set clearance positions and cutting areas radially across X.
02:07
The clearance height is the fully retracted position outside the part.
02:12
It represents the safest retract for the first rapid position and the last height after the toolpath has been completed.
02:19
The From reference is set to the Stock OD and the offset is set to 0.4 inches.
02:25
There is plenty of clearance to the outside of the stock.
02:29
The outer radius represents the outer surface of the stock to be machined.
02:34
For this, the From reference is set to the Stock OD, and the offset is set to 0.
02:40
The inner radius is the final cut depth in X.
02:43
Even though the from reference is set to the Stock ID, the tool will never get to the part center line.
02:50
It cuts everything within this boundary that can be cut without violating the part model.
02:55
There is nothing to change here.
02:58
Switch to the Passes tab.
03:00
To prevent dipping into the open groove areas, set the Grooving parameter to Don't allow grooving.
03:06
The Stepover amount per cut is set to .0393, but since the Number of Stepovers is set to 1, it will simply take a single finish pass.
03:16
The settings on the Linking tab control what will happen between cuts when the tool needs to retract and reposition.
03:23
For this example, there is nothing to change right now, so click OK to generate the profile finishing toolpath.
03:30
Zoom in to the back of the part.
03:33
In the Browser, notice the warning for the toolpath.
03:37
Click the warning symbol to show more information.
03:40
In this case, Fusion had to modify the toolpath to make it safe.
03:45
The lead out has been modified due to a gouge with the remaining stock.
03:50
Close the warning message.
03:52
Right-click the toolpath operation and select Edit.
03:57
In the Profile Finishing dialog, switch to the Linking tab.
04:01
Here, in the Leads & Transitions group, you see that the Linear Lead-In Angle is set to 45° from where the toolpath ends.
04:10
If it moves at 45°, it will collide with the stock.
04:14
There are two ways to fix this.
04:17
Option 1: If you absolutely cannot violate the stock area, uncheck Same As Lead-In and change the Linear Lead-Out Angle to 90°.
04:27
Option 2: If it is OK to cut the remaining stock, the simpler way is to check Allow Lead to Cut Stock.
04:34
Then, Fusion will permit the lead out move to enter the stock area.
04:39
For this example, check Allow Lead to Cut Stock, and then click OK.
04:44
The profile finishing toolpath is re-generated and there is no longer a warning.
04:49
Save your model if you want to continue working on it.
Manufacture > Turning (tab) > Turning > Turning Finishing 
Turning Finishing is a toolpath strategy used for finishing the Outside Diameter (OD) or Inside Diameter (ID) of the part. You can control the cut direction, tool orientation and limit the toolpath area by using containment boundaries.
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 for the best experience
Save your progress
Get access to courses
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.