& 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
In this lesson, we'll learn about external threading.
00:06
After completing this lesson, you'll be able to: Create an external threading toolpath and analyze a toolpath simulation.
00:14
In Fusion 360, we want to carry on with external threads.f3d.
00:18
At this point, we've created the chamfer toolpath on the leading edge of where our threads are going to be.
00:23
And now we want to create threads on the outside of the smaller and larger diameters.
00:28
This is going to be a 0.5/13 and this is going to be a 9/16 by 12.
00:33
We're going to do this by first going into Turning and selecting Turning Thread.
00:39
There is a threading tool inside of this document and we're going to take a look at tool number 5.
00:46
We will be changing this a little bit later.
00:47
But we're going to start with this tool to highlight a potential problem.
00:52
Once we've selected this, make sure that we are in outside or OD threading and we want to move on to our geometry.
00:58
We're going to select the outside face and automatically we'll get a preview on the screen where the tool’s coming from.
01:04
Notice right now that the tool is starting pretty far out and it's actually cutting a bit deeper than we want.
01:10
So there are few things that we want to do with this confinement.
01:13
First I'm going to set this back down to 0 and notice where the tool is coming into.
01:18
We need to have it at least start outside of this chamfer so we're going to set it at 0.08, which will allow us enough room to come into the cut.
01:27
On the back side, we want to extend past the end of our selection.
01:32
So you'll notice I'm going to take that out to 0.08 as well.
01:36
This will allow us to come into this groove which was cut specifically for threading,
01:41
and then we can pull away from the cut and hopefully not hit this taper.
01:45
We'll be able to see that in simulation if we have any problems.
01:49
The next thing that we want to do is we want to modify our OD.
01:53
And we're going to set this to a diameter and we're going to set it to 0.5.
01:58
We're going to set this exactly to our outside diameter and I like to do this to make sure that the tool knows exactly where we're working.
02:06
Next in the Passes section we have a few things that we need to adjust.
02:09
First is our thread depth.
02:11
This is going to be taken from some sort of threading charts.
02:15
Since we're doing external threading, we’ll be taking the major and the minor diameters for external threading.
02:22
In our case, that ends up being a value of 0.0472 if you take 0.5” and you subtract the minor or the effective diameter of external threading.
02:34
Then we need to adjust our thread pitch.
02:37
Since we're dealing with a 0.5/13, that is one inch divided by 13 and that's going to give us a value of 0.0769.
02:46
Once we have those set, I'm also going to adjust the Infeed Angle.
02:51
Notice that by default when it's set to 0 degrees, it's going to come in and then just work its way over.
02:58
When we modify this value, notice that it has an example of 60 degrees divided by 2 minus 0.5 will give us a 29.5 Infeed Angle.
03:07
So I'm going to adjust this to 29.5 and then I'm going to say OK.
03:14
Notice how it changes the exits as well.
03:18
Now that we have this, let's go ahead and simulate.
03:22
When we simulate threading tools, because we have our model set to the outside diameter, we’ll need to hide the model so we can see the threads.
03:31
And at a first glance this might look okay, but notice that the peaks of the threads are actually cut.
03:37
And this is telling me that the tool that I'm using is not actually large enough.
03:41
It doesn't have enough reach to cut the large threads that I'm dealing with.
03:45
So I need to change the tool that's used in this operation.
03:49
So I'm going to edit the operation.
03:50
And instead of using that tool, I'm going to go into my samples library and I'm going to filter by Turning, I'm going to filter by Turning Threading.
03:58
There are two tools in here and of course, we can make our own if we have a specific tool that we're using.
04:03
But I'm going to use the overall length of 30 millimeters, I'm going to select this.
04:08
Notice that this gives us a little bit more depth and then I'm going to regenerate this toolpath.
04:13
I’m going to go back into Simulate and jump all the way to the end.
04:16
Now you can see that there is a portion that's left at that major outside diameter.
04:21
So we're no longer cutting down the threads with the portion of the tool that we're not expecting to cut with.
04:27
Now that we have this set up, let's go ahead and re-show our model and create another turning thread toolpath.
04:35
Again, we want to go in and make sure that we are using that larger tool because now we're dealing with a 9/16-12.
04:42
Then in the Geometry, we're going to select the face that we're interested in.
04:45
But notice that by default the front side stock offset is way too large.
04:50
We need to reduce this value and I'm going to take it down to 0.1, which should allow us to come into this groove.
04:57
We might have to reduce this after a simulation, but it allows us to come into the area where there's no thread and then move into the cut.
05:06
We also want to extend this on the back side and again, I'm going to go 0.8.
05:10
I want to make sure that it's at least more than my thread pitch so that the tool does come completely out of the cut.
05:16
Next I need to set the OD.
05:18
And we can do this again based on our specifics.
05:21
But I can also select the geometry and then set my offset value to 0 after I've made that selection.
05:29
So if we know the outside diameter that we're using, for example, if we have a specific fit or a class of thread that we're cutting,
05:37
and we know that it's a little bit smaller than half inch or 9/16, then we can use those values as well.
05:44
Now that we have that set, we need to adjust the thread depth as well as the thread pitch.
05:49
Since we are dealing with a 9/16, then we're going to be dealing with a slightly different number again.
05:55
Based on the class of thread and specifics about what you're cutting, this can range anywhere from about 0.049 to 0.0511.
06:04
I'm going to go ahead and use that larger value.
06:07
And I'm going to set my thread pitch again based on one inch divided by 12,
06:12
because the number of threads that we’re using per inch is based off of that number.
06:16
This is going to be 0833.
06:19
I am going to change that Infeed Angle again to 29.5 and I'll say OK.
06:25
Notice that when the tool comes in, it's clipping the backside of this front thread.
06:30
So that's obviously problematic and we can see that directly in in-process stock.
06:35
However, if we didn't have that turned on, it might be a little bit harder to recognize that the tool is actually gouging,
06:40
and we don't want that to happen.
06:42
So we'll go back into our toolpath, we'll go back into our containment and on the front side, we're going to set this a little bit lower.
06:50
I'm going to set it to 0.05 which should give me plenty of room.
06:55
We'll say OK, and then we'll simulate this toolpath as well.
06:59
Once again, hiding the model, we can play through or we can jump all the way to the end and see if the results that we have are what we're expecting.
07:07
Now, likely what we would want to do on the backside of this part is probably begin to cut a relief before we started cutting these threads,
07:14
and then we can part it off after the threading operation.
07:18
Let's go ahead and select the entire setup and run through simulation.
07:22
I'm going to jump ahead all the way to the end and just take a look at the results.
07:27
So this looks a bit better. It looks like what I would expect to see.
07:31
And again, we would need to make sure that the tool that we're using is right for the application.
07:37
We don't want to just grab a tool from the library and try to make it work.
07:40
We want to make sure that we have a specific threading tool and custom tailor the tool inside of our library to match what we have.
07:47
If the tool in your machine doesn't match the tool that's being used in the simulation or the calculations of where that tool needs to go,
07:54
then the results are going to be hopefully just drastically different and not catastrophic.
08:01
But from here now that we've created our threading toolpaths, let's make sure that we save this before moving on.
Video transcript
00:02
In this lesson, we'll learn about external threading.
00:06
After completing this lesson, you'll be able to: Create an external threading toolpath and analyze a toolpath simulation.
00:14
In Fusion 360, we want to carry on with external threads.f3d.
00:18
At this point, we've created the chamfer toolpath on the leading edge of where our threads are going to be.
00:23
And now we want to create threads on the outside of the smaller and larger diameters.
00:28
This is going to be a 0.5/13 and this is going to be a 9/16 by 12.
00:33
We're going to do this by first going into Turning and selecting Turning Thread.
00:39
There is a threading tool inside of this document and we're going to take a look at tool number 5.
00:46
We will be changing this a little bit later.
00:47
But we're going to start with this tool to highlight a potential problem.
00:52
Once we've selected this, make sure that we are in outside or OD threading and we want to move on to our geometry.
00:58
We're going to select the outside face and automatically we'll get a preview on the screen where the tool’s coming from.
01:04
Notice right now that the tool is starting pretty far out and it's actually cutting a bit deeper than we want.
01:10
So there are few things that we want to do with this confinement.
01:13
First I'm going to set this back down to 0 and notice where the tool is coming into.
01:18
We need to have it at least start outside of this chamfer so we're going to set it at 0.08, which will allow us enough room to come into the cut.
01:27
On the back side, we want to extend past the end of our selection.
01:32
So you'll notice I'm going to take that out to 0.08 as well.
01:36
This will allow us to come into this groove which was cut specifically for threading,
01:41
and then we can pull away from the cut and hopefully not hit this taper.
01:45
We'll be able to see that in simulation if we have any problems.
01:49
The next thing that we want to do is we want to modify our OD.
01:53
And we're going to set this to a diameter and we're going to set it to 0.5.
01:58
We're going to set this exactly to our outside diameter and I like to do this to make sure that the tool knows exactly where we're working.
02:06
Next in the Passes section we have a few things that we need to adjust.
02:09
First is our thread depth.
02:11
This is going to be taken from some sort of threading charts.
02:15
Since we're doing external threading, we’ll be taking the major and the minor diameters for external threading.
02:22
In our case, that ends up being a value of 0.0472 if you take 0.5” and you subtract the minor or the effective diameter of external threading.
02:34
Then we need to adjust our thread pitch.
02:37
Since we're dealing with a 0.5/13, that is one inch divided by 13 and that's going to give us a value of 0.0769.
02:46
Once we have those set, I'm also going to adjust the Infeed Angle.
02:51
Notice that by default when it's set to 0 degrees, it's going to come in and then just work its way over.
02:58
When we modify this value, notice that it has an example of 60 degrees divided by 2 minus 0.5 will give us a 29.5 Infeed Angle.
03:07
So I'm going to adjust this to 29.5 and then I'm going to say OK.
03:14
Notice how it changes the exits as well.
03:18
Now that we have this, let's go ahead and simulate.
03:22
When we simulate threading tools, because we have our model set to the outside diameter, we’ll need to hide the model so we can see the threads.
03:31
And at a first glance this might look okay, but notice that the peaks of the threads are actually cut.
03:37
And this is telling me that the tool that I'm using is not actually large enough.
03:41
It doesn't have enough reach to cut the large threads that I'm dealing with.
03:45
So I need to change the tool that's used in this operation.
03:49
So I'm going to edit the operation.
03:50
And instead of using that tool, I'm going to go into my samples library and I'm going to filter by Turning, I'm going to filter by Turning Threading.
03:58
There are two tools in here and of course, we can make our own if we have a specific tool that we're using.
04:03
But I'm going to use the overall length of 30 millimeters, I'm going to select this.
04:08
Notice that this gives us a little bit more depth and then I'm going to regenerate this toolpath.
04:13
I’m going to go back into Simulate and jump all the way to the end.
04:16
Now you can see that there is a portion that's left at that major outside diameter.
04:21
So we're no longer cutting down the threads with the portion of the tool that we're not expecting to cut with.
04:27
Now that we have this set up, let's go ahead and re-show our model and create another turning thread toolpath.
04:35
Again, we want to go in and make sure that we are using that larger tool because now we're dealing with a 9/16-12.
04:42
Then in the Geometry, we're going to select the face that we're interested in.
04:45
But notice that by default the front side stock offset is way too large.
04:50
We need to reduce this value and I'm going to take it down to 0.1, which should allow us to come into this groove.
04:57
We might have to reduce this after a simulation, but it allows us to come into the area where there's no thread and then move into the cut.
05:06
We also want to extend this on the back side and again, I'm going to go 0.8.
05:10
I want to make sure that it's at least more than my thread pitch so that the tool does come completely out of the cut.
05:16
Next I need to set the OD.
05:18
And we can do this again based on our specifics.
05:21
But I can also select the geometry and then set my offset value to 0 after I've made that selection.
05:29
So if we know the outside diameter that we're using, for example, if we have a specific fit or a class of thread that we're cutting,
05:37
and we know that it's a little bit smaller than half inch or 9/16, then we can use those values as well.
05:44
Now that we have that set, we need to adjust the thread depth as well as the thread pitch.
05:49
Since we are dealing with a 9/16, then we're going to be dealing with a slightly different number again.
05:55
Based on the class of thread and specifics about what you're cutting, this can range anywhere from about 0.049 to 0.0511.
06:04
I'm going to go ahead and use that larger value.
06:07
And I'm going to set my thread pitch again based on one inch divided by 12,
06:12
because the number of threads that we’re using per inch is based off of that number.
06:16
This is going to be 0833.
06:19
I am going to change that Infeed Angle again to 29.5 and I'll say OK.
06:25
Notice that when the tool comes in, it's clipping the backside of this front thread.
06:30
So that's obviously problematic and we can see that directly in in-process stock.
06:35
However, if we didn't have that turned on, it might be a little bit harder to recognize that the tool is actually gouging,
06:40
and we don't want that to happen.
06:42
So we'll go back into our toolpath, we'll go back into our containment and on the front side, we're going to set this a little bit lower.
06:50
I'm going to set it to 0.05 which should give me plenty of room.
06:55
We'll say OK, and then we'll simulate this toolpath as well.
06:59
Once again, hiding the model, we can play through or we can jump all the way to the end and see if the results that we have are what we're expecting.
07:07
Now, likely what we would want to do on the backside of this part is probably begin to cut a relief before we started cutting these threads,
07:14
and then we can part it off after the threading operation.
07:18
Let's go ahead and select the entire setup and run through simulation.
07:22
I'm going to jump ahead all the way to the end and just take a look at the results.
07:27
So this looks a bit better. It looks like what I would expect to see.
07:31
And again, we would need to make sure that the tool that we're using is right for the application.
07:37
We don't want to just grab a tool from the library and try to make it work.
07:40
We want to make sure that we have a specific threading tool and custom tailor the tool inside of our library to match what we have.
07:47
If the tool in your machine doesn't match the tool that's being used in the simulation or the calculations of where that tool needs to go,
07:54
then the results are going to be hopefully just drastically different and not catastrophic.
08:01
But from here now that we've created our threading toolpaths, let's make sure that we save this before moving on.
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.