& 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 video, we'll talk about Lathe threading toolpaths.
00:07
After completing this step, you'll be able to create a threading toolpath.
00:12
In Fusion 360, we want to carry on with our CAD CAM Lathe dataset.
00:16
Now it's time for us to take a look at threading the outside of our part.
00:20
To get started, we're going to go to turning and select turning threat.
00:25
We first need to select an appropriate tool and we'll go to introduction to CAD CAM Lathe and select tool number 5 or OD threading.
00:33
Once we select this tool we can move on to selecting our geometry.
00:37
We're going to start with the smaller portion and take a look at this from the top.
00:42
Can see where the tool is coming in, moving through and pulling away right at the end.
00:47
There are some confinement options we have in terms of the front and the back side.
00:52
The front doesn't need a full 10 but the back side needs a little bit more.
00:57
I'm going to give it 2.2 mm which should take us fairly close to this wall.
01:03
In the next section we're going to go to passes and we're going to take a look at our options.
01:08
Right now, the default thread depth value is set to and thread chart.
01:16
In our case it's going to be 2.6 mm and the thread pitch is 2. This outside thread is an M50 x 4.0 now the inside thread was an M25 x 2.0,
01:29
but we had a tap for that internal geometry.
01:32
What we want to do from here is we want to make sure that we are removing enough material and that the thread depth is enough for what we're doing.
01:40
We're going to set our thread pitch to four and we're going to use the default value of constant in feed for right now.
01:48
We have fade thread end and you'll notice that it's starting to taper away.
01:52
We also have spring pass. If we want to repeat the last pass.
01:56
From here, let's select "OK". And let's see the results.
02:00
You'll note that we're not seeing any of the results, but if we go to simulate and we hide the model,
02:06
we can play through and see it begin to cut these threads.
02:10
One thing that you want to be aware of whenever you're cutting threads,
02:13
is the tool that you're using to make sure that it's actually applicable for the thread size.
02:18
You'll know what this tool as it comes back through.
02:21
The tool itself is starting to cut the tops of the threads flat because it doesn't have enough thread depth to cut the geometry we need.
02:31
This tells me that I'm not using the correct tool for the job once again using Fusion 360 and simulating, we're able to find these problems.
02:40
So let's go into tool number 5. And let's edit the tool.
02:44
With a threading tool, we can take a look at the insert and note that the geometry of the insert right now
02:50
is based on the thickness and overall length a width and a thread pitch.
02:55
The threat pitch in our case is going to be four and this is going to change the depth that this can actually cut.
03:03
I'm going to increase the width to 6 mm and we're going to use all the rest of those values and accept the change.
03:11
We need to regenerate this toolpath and then we'll simulate it one more time.
03:16
This time I'm gonna roll through and notice that as we're coming through when we get to the final cut through,
03:24
the insert is no longer cutting off the tops or the ends of those threads.
03:28
We're sticking to that major outside diameter.
03:31
So once again it's important that our tool is able to cut the geometry needed, it might not be visible,
03:38
but you need to make sure that you double check all of these settings.
03:41
When you're looking at simulate and make sure you identify areas of possible concerns.
03:46
When we're looking at these results. We can also see areas where we might want to explore additional toolpaths as needed.
03:53
The last thing that will need for this part is to remove it from the rest of the stock.
03:58
In order to do that, we're going to go to turning and select turning part.
04:02
We need an appropriate parting tool and in our case our library doesn't contain one
04:08
but we can use this OD grooving tool depending on the geometry and the orientation of the holder.
04:14
We might have enough to remove our part but we might have to grab another tool.
04:19
So let's give it a shot with this tool that's already preloaded
04:22
and note that it automatically goes to the correct area and begins the toolpath without any selection.
04:28
It does this based on model back and knows exactly where the john tree is.
04:33
So we don't have to make any adjustments.
04:36
But when we're using this toolpath we have an option called edge break
04:39
that allows us to add a chamfer on the back edge at the same time as a parting operation,
04:45
let's go ahead and use that and let's review the geometry.
04:49
We're going to go in to simulate one more time and I'm going to hide the model.
04:53
At the bottom, I'm going to manually play through noting that it starts a pecking operation and it begins to cut.
04:59
But because of the holder geometry we can't actually get in, in part.
05:04
This tells me that I need to use a different tool. So I'm going to modify and select another tool.
05:12
In my Fusion 360 library, let's take a look at some of the OD grooving tools that we have.
05:18
We have some round tools and we have a square tool.
05:21
Either of these will be fine. It just simply depends on the geometry.
05:26
I'm going to select the rounded OD grooving tool and then we're going to make some changes to the tool afterwards.
05:33
I do want to take a look at my passes, I'm going to turn on packing
05:38
and I'm going to double check my settings for the chamfer.
05:42
Noting that the chamfer option using edge break is not actually cutting the chamfer on our part. The tool is coming in a bit further away.
05:51
We also have an option to use fill it.
05:52
But in this case let's turn the edge break off and just see if we can part this without intersecting with the stock.
05:60
Once again, you'll note that we have an issue so we need to redefine the tool itself.
06:06
Depending on the tools you have available,
06:08
once again, you need to make sure that your specific tools will actually make the geometry or make the cut that's needed.
06:15
We have an overall length and the thickness value. We have a width value and a groove width.
06:21
And these values are based on the insert and then we have a holder value which has our head length,
06:26
it has the overall length and has the shank width and the shank height.
06:31
We're going to increase the head length of 50 mm.
06:35
We're going to accept this change and we're going to allow it to regenerate that toolpath.
06:41
Lastly we'll simulate it one more time.
06:45
Make sure that we have the clearance to remove the part completely.
06:51
And then we can finish the simulation. Go back to home view and bring back the view of our part.
06:58
Let's make a quick save and let's discuss briefly what we've done.
07:03
At this point, we face the outside of the part and we've done our external roughing and finishing toolpaths.
07:09
We did a single groove on the outside and then we used an insert drill on the inside to remove material before taking a smaller boring bar in.
07:18
We had a single groove tool which needs a little bit of adjustment. You'll notice that it's going a little bit too far back.
07:24
Then we drilled the inside which was our tapping operation. We did our external chamfers.
07:30
We worked with our boring bar to create our internal chamfer, we did our external thread and then we did our parting toolpath.
07:38
Once again I can't stress enough how important it is to make sure that you have the right tools for the job
07:43
and that your digital representation of those tools matches what the physical tool has.
07:49
Without having the consistency between your digital tool library and the real tool.
07:54
The collision checking and errors that you find in Fusion 360 are not going to help you produce your parts.
08:01
At this point, if you made any other changes, make sure that you say before moving on.
Video transcript
00:02
In this video, we'll talk about Lathe threading toolpaths.
00:07
After completing this step, you'll be able to create a threading toolpath.
00:12
In Fusion 360, we want to carry on with our CAD CAM Lathe dataset.
00:16
Now it's time for us to take a look at threading the outside of our part.
00:20
To get started, we're going to go to turning and select turning threat.
00:25
We first need to select an appropriate tool and we'll go to introduction to CAD CAM Lathe and select tool number 5 or OD threading.
00:33
Once we select this tool we can move on to selecting our geometry.
00:37
We're going to start with the smaller portion and take a look at this from the top.
00:42
Can see where the tool is coming in, moving through and pulling away right at the end.
00:47
There are some confinement options we have in terms of the front and the back side.
00:52
The front doesn't need a full 10 but the back side needs a little bit more.
00:57
I'm going to give it 2.2 mm which should take us fairly close to this wall.
01:03
In the next section we're going to go to passes and we're going to take a look at our options.
01:08
Right now, the default thread depth value is set to and thread chart.
01:16
In our case it's going to be 2.6 mm and the thread pitch is 2. This outside thread is an M50 x 4.0 now the inside thread was an M25 x 2.0,
01:29
but we had a tap for that internal geometry.
01:32
What we want to do from here is we want to make sure that we are removing enough material and that the thread depth is enough for what we're doing.
01:40
We're going to set our thread pitch to four and we're going to use the default value of constant in feed for right now.
01:48
We have fade thread end and you'll notice that it's starting to taper away.
01:52
We also have spring pass. If we want to repeat the last pass.
01:56
From here, let's select "OK". And let's see the results.
02:00
You'll note that we're not seeing any of the results, but if we go to simulate and we hide the model,
02:06
we can play through and see it begin to cut these threads.
02:10
One thing that you want to be aware of whenever you're cutting threads,
02:13
is the tool that you're using to make sure that it's actually applicable for the thread size.
02:18
You'll know what this tool as it comes back through.
02:21
The tool itself is starting to cut the tops of the threads flat because it doesn't have enough thread depth to cut the geometry we need.
02:31
This tells me that I'm not using the correct tool for the job once again using Fusion 360 and simulating, we're able to find these problems.
02:40
So let's go into tool number 5. And let's edit the tool.
02:44
With a threading tool, we can take a look at the insert and note that the geometry of the insert right now
02:50
is based on the thickness and overall length a width and a thread pitch.
02:55
The threat pitch in our case is going to be four and this is going to change the depth that this can actually cut.
03:03
I'm going to increase the width to 6 mm and we're going to use all the rest of those values and accept the change.
03:11
We need to regenerate this toolpath and then we'll simulate it one more time.
03:16
This time I'm gonna roll through and notice that as we're coming through when we get to the final cut through,
03:24
the insert is no longer cutting off the tops or the ends of those threads.
03:28
We're sticking to that major outside diameter.
03:31
So once again it's important that our tool is able to cut the geometry needed, it might not be visible,
03:38
but you need to make sure that you double check all of these settings.
03:41
When you're looking at simulate and make sure you identify areas of possible concerns.
03:46
When we're looking at these results. We can also see areas where we might want to explore additional toolpaths as needed.
03:53
The last thing that will need for this part is to remove it from the rest of the stock.
03:58
In order to do that, we're going to go to turning and select turning part.
04:02
We need an appropriate parting tool and in our case our library doesn't contain one
04:08
but we can use this OD grooving tool depending on the geometry and the orientation of the holder.
04:14
We might have enough to remove our part but we might have to grab another tool.
04:19
So let's give it a shot with this tool that's already preloaded
04:22
and note that it automatically goes to the correct area and begins the toolpath without any selection.
04:28
It does this based on model back and knows exactly where the john tree is.
04:33
So we don't have to make any adjustments.
04:36
But when we're using this toolpath we have an option called edge break
04:39
that allows us to add a chamfer on the back edge at the same time as a parting operation,
04:45
let's go ahead and use that and let's review the geometry.
04:49
We're going to go in to simulate one more time and I'm going to hide the model.
04:53
At the bottom, I'm going to manually play through noting that it starts a pecking operation and it begins to cut.
04:59
But because of the holder geometry we can't actually get in, in part.
05:04
This tells me that I need to use a different tool. So I'm going to modify and select another tool.
05:12
In my Fusion 360 library, let's take a look at some of the OD grooving tools that we have.
05:18
We have some round tools and we have a square tool.
05:21
Either of these will be fine. It just simply depends on the geometry.
05:26
I'm going to select the rounded OD grooving tool and then we're going to make some changes to the tool afterwards.
05:33
I do want to take a look at my passes, I'm going to turn on packing
05:38
and I'm going to double check my settings for the chamfer.
05:42
Noting that the chamfer option using edge break is not actually cutting the chamfer on our part. The tool is coming in a bit further away.
05:51
We also have an option to use fill it.
05:52
But in this case let's turn the edge break off and just see if we can part this without intersecting with the stock.
05:60
Once again, you'll note that we have an issue so we need to redefine the tool itself.
06:06
Depending on the tools you have available,
06:08
once again, you need to make sure that your specific tools will actually make the geometry or make the cut that's needed.
06:15
We have an overall length and the thickness value. We have a width value and a groove width.
06:21
And these values are based on the insert and then we have a holder value which has our head length,
06:26
it has the overall length and has the shank width and the shank height.
06:31
We're going to increase the head length of 50 mm.
06:35
We're going to accept this change and we're going to allow it to regenerate that toolpath.
06:41
Lastly we'll simulate it one more time.
06:45
Make sure that we have the clearance to remove the part completely.
06:51
And then we can finish the simulation. Go back to home view and bring back the view of our part.
06:58
Let's make a quick save and let's discuss briefly what we've done.
07:03
At this point, we face the outside of the part and we've done our external roughing and finishing toolpaths.
07:09
We did a single groove on the outside and then we used an insert drill on the inside to remove material before taking a smaller boring bar in.
07:18
We had a single groove tool which needs a little bit of adjustment. You'll notice that it's going a little bit too far back.
07:24
Then we drilled the inside which was our tapping operation. We did our external chamfers.
07:30
We worked with our boring bar to create our internal chamfer, we did our external thread and then we did our parting toolpath.
07:38
Once again I can't stress enough how important it is to make sure that you have the right tools for the job
07:43
and that your digital representation of those tools matches what the physical tool has.
07:49
Without having the consistency between your digital tool library and the real tool.
07:54
The collision checking and errors that you find in Fusion 360 are not going to help you produce your parts.
08:01
At this point, if you made any other changes, make sure that you say 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.