& 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 use drill and tap for turning.
00:06
After completing this lesson, you'll be able to: Create a drilling cycle and create a rigid tapping cycle.
00:14
In Fusion 360, we want to get started with the data set drill and tap.f3d.
00:18
We should be in the Manufacture workspace with the unit set to inch.
00:23
Notice that we already have a setup with stock and we need to simply create some operations to drill and tap this part.
00:30
I'm going to get started by doing some standard operations such as turning face.
00:35
We need to select a tool and I'm going to go into my Fusion 360 Library.
00:40
I’m going to take a look at turning general and I'm going to grab the second tool in the list, making sure that the orientation is correct.
00:49
I'm going to say OK allowing it to face the end and then I'm going to use that same tool for a profile roughing operation.
00:57
I’m going to use all of the default settings and say OK, allowing it to create my toolpath.
01:04
I'm not going to finish the outside, but now we're a little bit closer to the final shape,
01:08
and what we can see here is that we're ready to drill and tap the end.
01:13
What I want to talk about is ways in which we can use drilling and tapping that can be used on a turning machine.
01:20
So in this instance, what we're going to do is we're going to select Drill,
01:24
and rather than create pre drill toolpaths, I'm going to just go ahead and go right to the correct diameter of this hole.
01:30
Now, obviously depending on the material and the type of drill that you're using,
01:34
you would likely want to come in and clear out a little bit of material first.
01:38
But again, in this example, we're just going to take a look at how we're going to create this.
01:43
We're going to be using a 27/64 drill which is already inside of our document.
01:49
But I want to make sure that we use the edit tool operation and take a look at post processor.
01:57
This has what we call a live tool.
01:60
When it has the live tool option, what this means is that it can be used in a CNC lathe that has live tooling.
02:08
Now, in this case the chuck on this is wrong.
02:11
But what we're really interested in is creating this drilling operation coming from the Z axis.
02:18
So you'll notice that the tool orientation is already correct.
02:21
It's already based on the rotation axis of our machine.
02:25
So all we really need to do is we need to tell it where it's drilling, specifically the heights.
02:31
We can use the geometry to select the inside of the hole and in this part, it actually goes all the way through.
02:37
The next thing that we want to do is we want to set our heights, which looks very similar to how it would when we're dealing with milling.
02:44
We can turn on drill tip through bottom and based on the drill parameters, it'll come all the way through.
02:50
We might also want a positive breakthrough depth and in this case, I'm going to set it to positive 0.1.
02:56
Because we do have stock on the back side and we will be using a parting tool to get this off the rest of the stock,
03:02
I want to make sure that the square portion of the drill, not the tapered end, is coming through at least the thickness of my parting tool.
03:11
So I'm adding that 0.1.
03:12
We can add as much as we need,
03:14
but that ensures that I'm making a nice clean cut all the way to the center and we're not leaving a small remnant there.
03:21
The next thing that we want to take a look at is the drilling cycle.
03:24
Since we are dealing with a large drill going into a bore, I'm going to use the full retract option,
03:32
which means that it's going to be pecking a specific amount, in this case 0.105 and then it's going to come completely back out of the hole.
03:41
So I'm going to say OK, and I'm going to take a look at this in simulation.
03:44
I'm going to drag the cursor along the bottom, notice it's making those pecks and it's coming completely back out of the hole.
03:50
This allows the chips to be ejected, especially since we are spinning and likely using some coolant.
03:56
This will help make sure that we get a nice clean hole.
04:00
And again, in reality we would probably pre drill this based on the specific tools that you're using.
04:05
But I want to just do this with a single operation so now we can take a look at creating a tapping operation.
04:12
Once again I'm going to go to drill, I'm going to select my tap, which is a 0.5/13.
04:17
This is automatically going to change the cycle to tapping.
04:21
We need to select the geometry.
04:23
Now, if we want to tap the entire hole, let's go ahead and select that.
04:27
And then we're going to move on to our heights.
04:29
And again we're going to allow it to go through the bottom.
04:32
When we use drill tip through the bottom on a tap, it doesn't really change anything because the end of the tap is not tapered.
04:39
So what we need to do is we need to use the offset but it's going to be a negative value.
04:44
So I'm going to set it to negative 0.1”, that allows me to extend through the bottom at least a single thread and then it'll retract from there.
04:55
Now if we want to change the tapping cycle or the dwelling,
04:58
we can make those modifications just like a standard drilling or tapping cycle that we would use on a mill.
05:04
Now that we have this tap created, we can simulate it but remember that the hole size is going to be the minor diameter.
05:11
So as we run the tap through, all it's going to do is make a larger hole than we would expect.
05:16
Tapping this deep on a part is often going to be problematic.
05:20
So again we will have to make sure that we set our tapping cycle and our drilling cycles based on the geometry,
05:28
and the size of the tools that we're working with.
05:30
From here, now that we have both of these operations set, let's go ahead and save this before moving on.
Video transcript
00:02
In this lesson, we'll use drill and tap for turning.
00:06
After completing this lesson, you'll be able to: Create a drilling cycle and create a rigid tapping cycle.
00:14
In Fusion 360, we want to get started with the data set drill and tap.f3d.
00:18
We should be in the Manufacture workspace with the unit set to inch.
00:23
Notice that we already have a setup with stock and we need to simply create some operations to drill and tap this part.
00:30
I'm going to get started by doing some standard operations such as turning face.
00:35
We need to select a tool and I'm going to go into my Fusion 360 Library.
00:40
I’m going to take a look at turning general and I'm going to grab the second tool in the list, making sure that the orientation is correct.
00:49
I'm going to say OK allowing it to face the end and then I'm going to use that same tool for a profile roughing operation.
00:57
I’m going to use all of the default settings and say OK, allowing it to create my toolpath.
01:04
I'm not going to finish the outside, but now we're a little bit closer to the final shape,
01:08
and what we can see here is that we're ready to drill and tap the end.
01:13
What I want to talk about is ways in which we can use drilling and tapping that can be used on a turning machine.
01:20
So in this instance, what we're going to do is we're going to select Drill,
01:24
and rather than create pre drill toolpaths, I'm going to just go ahead and go right to the correct diameter of this hole.
01:30
Now, obviously depending on the material and the type of drill that you're using,
01:34
you would likely want to come in and clear out a little bit of material first.
01:38
But again, in this example, we're just going to take a look at how we're going to create this.
01:43
We're going to be using a 27/64 drill which is already inside of our document.
01:49
But I want to make sure that we use the edit tool operation and take a look at post processor.
01:57
This has what we call a live tool.
01:60
When it has the live tool option, what this means is that it can be used in a CNC lathe that has live tooling.
02:08
Now, in this case the chuck on this is wrong.
02:11
But what we're really interested in is creating this drilling operation coming from the Z axis.
02:18
So you'll notice that the tool orientation is already correct.
02:21
It's already based on the rotation axis of our machine.
02:25
So all we really need to do is we need to tell it where it's drilling, specifically the heights.
02:31
We can use the geometry to select the inside of the hole and in this part, it actually goes all the way through.
02:37
The next thing that we want to do is we want to set our heights, which looks very similar to how it would when we're dealing with milling.
02:44
We can turn on drill tip through bottom and based on the drill parameters, it'll come all the way through.
02:50
We might also want a positive breakthrough depth and in this case, I'm going to set it to positive 0.1.
02:56
Because we do have stock on the back side and we will be using a parting tool to get this off the rest of the stock,
03:02
I want to make sure that the square portion of the drill, not the tapered end, is coming through at least the thickness of my parting tool.
03:11
So I'm adding that 0.1.
03:12
We can add as much as we need,
03:14
but that ensures that I'm making a nice clean cut all the way to the center and we're not leaving a small remnant there.
03:21
The next thing that we want to take a look at is the drilling cycle.
03:24
Since we are dealing with a large drill going into a bore, I'm going to use the full retract option,
03:32
which means that it's going to be pecking a specific amount, in this case 0.105 and then it's going to come completely back out of the hole.
03:41
So I'm going to say OK, and I'm going to take a look at this in simulation.
03:44
I'm going to drag the cursor along the bottom, notice it's making those pecks and it's coming completely back out of the hole.
03:50
This allows the chips to be ejected, especially since we are spinning and likely using some coolant.
03:56
This will help make sure that we get a nice clean hole.
04:00
And again, in reality we would probably pre drill this based on the specific tools that you're using.
04:05
But I want to just do this with a single operation so now we can take a look at creating a tapping operation.
04:12
Once again I'm going to go to drill, I'm going to select my tap, which is a 0.5/13.
04:17
This is automatically going to change the cycle to tapping.
04:21
We need to select the geometry.
04:23
Now, if we want to tap the entire hole, let's go ahead and select that.
04:27
And then we're going to move on to our heights.
04:29
And again we're going to allow it to go through the bottom.
04:32
When we use drill tip through the bottom on a tap, it doesn't really change anything because the end of the tap is not tapered.
04:39
So what we need to do is we need to use the offset but it's going to be a negative value.
04:44
So I'm going to set it to negative 0.1”, that allows me to extend through the bottom at least a single thread and then it'll retract from there.
04:55
Now if we want to change the tapping cycle or the dwelling,
04:58
we can make those modifications just like a standard drilling or tapping cycle that we would use on a mill.
05:04
Now that we have this tap created, we can simulate it but remember that the hole size is going to be the minor diameter.
05:11
So as we run the tap through, all it's going to do is make a larger hole than we would expect.
05:16
Tapping this deep on a part is often going to be problematic.
05:20
So again we will have to make sure that we set our tapping cycle and our drilling cycles based on the geometry,
05:28
and the size of the tools that we're working with.
05:30
From here, now that we have both of these operations set, let's go ahead and 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.