& 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're going to drill and tap.
00:06
After completing this step, you'll be able to create a spot drill operation, create a peck drill operation and create a tapping operation.
00:15
In Fusion 360, we want to carry on with our CAD/CAM Milling dataset.
00:19
At this point, we've gone all the way through the model, to rough and finish the major geometry and we've roughed and finish the slots.
00:27
Now we need to drill and tap all the holes in the design.
00:30
To do this, we're going to start by going to drilling and select the drill operation.
00:35
We need to select the proper tool so we'll go into our introduction library.
00:39
A note that we have a drill, a spot drill and then we have a tap.
00:43
For this operation, we're going to select the 5 mm spot drill.
00:47
One thing to note is none of the tools so far have had tool numbers which means that Fusion 360 is automatically going to increment them for us.
00:56
If you're starting fresh and don't have predefined tools inside of your machine, this can work.
01:01
However, it's always a good idea to define those tool numbers.
01:05
So once we're done programming the part we're going to go back and make some adjustments to these tool numbers.
01:10
Now that we have our tool selected, we need to move on to our geometry.
01:14
There are a few different ways that we can select holes in Fusion 360. We can manually select them based on faces.
01:21
We can use some other options such as selected points which allows us to select an edge
01:26
and it will automatically grab the center point or we can use the option to give it a diameter range.
01:33
We know that we're drilling a hole for an M5.
01:36
So if we set the lower end at 4 mm, noticed that it automatically grabbed all the holes for us and it knows exactly what the depth is.
01:45
We're going to move on to the heights section but note that we're using a spot drill.
01:49
So instead of using the whole bottom, I'm going to use the whole top and check the drill tip through bottom,
01:56
which allows the end of the spot drill to go through all the way up to the end of its taper.
02:01
This works for a smaller spot drill but if you have a larger spot drill, you want to be careful that you're not exceeding the diameter of the hole.
02:09
And lastly we needed to find the cycle. For us, drilling rapid out is going to work fine because we're barely taking the drill tip into the material.
02:17
So we're going to say, okay.
02:19
Now it starts at the red arrow and it moves its way all the way around until it gets to the green arrow.
02:26
Now we want to drill the holes so I'm going to right click on this drilling operation and duplicate it.
02:33
I'm going to select the duplicate right click and edit.
02:37
Now we're going to change our tool instead of using the spot drill, we want to use our 4.2 mm drill.
02:44
Once again, the drill bit doesn't have a tool number so it's automatically incremental.
02:50
The whole geometry is going to be the same.
02:52
However, I'm going to use the reverse order option
02:54
which means it's going to start at the hole that it finished the spot drilling and work its way backwards.
02:60
On this specific part, it's not going to make much of a difference because it could simply jump to the next location.
03:07
But depending on the specific hole pattern, this can save a lot of time.
03:11
Next, we want to make sure that we take a look at the heights and we use whole bottom.
03:17
It's also important to note that the whole bottom is going to be based on the entire depth of the hole.
03:24
And we need to keep in mind that these are tapped holes.
03:27
If we're drilling exactly to the whole bottom,
03:29
we don't want to tap to the whole bottom because we're going to be bottoming out the tap on solid geometry.
03:36
So we need to be real careful on the detailed drawing to see if we need the exact depth of threads or if we need the exact depth of the hole.
03:45
Depending on geometry on the other side of the part, one of them might be more important than the other.
03:51
We're going to be using the whole death as the bottom.
03:54
So we're going to move on to our cycle and we're going to change this to a different type of cycle
03:58
because we don't want to feed all the way through the hole.
04:01
We want to allow it to extract some chips.
04:03
There are two options that we have chip breaking partial were tracked and deep drilling.
04:09
The chip breaking partial retract will allow it to go down a set amount, come back slightly and then proceed to go down again.
04:16
When we use full retract, it'll use that same packing depth however, will retract completely out of the hole.
04:24
This helps evacuate chips from the hole and in some cases this is going to be more important.
04:29
However, for our case we're going to use the partial attract as this will work fine for our geometry.
04:34
Using the default settings for packing depth and amount we're going to say, okay.
04:40
Now that we've created our spot drill and our drilling operation, it's time to create our tapping operation.
04:46
I'm gonna right click and I'm gonna duplicate this one more time.
04:51
Then we're going to right click and edit the duplicate.
04:54
Now, instead of drilling we're going to use our 5 mm tap and we're going to select that tool.
05:01
In the geometry section we'll deselect reverse. So now we're starting at the original point working our way around.
05:08
In the heights section, we want to be careful of the whole bottom because again we don't want to bottom out the tap.
05:14
So I'm going to add a positive value of .5 mm. So that way the tap doesn't go all the way to the bottom.
05:22
This generally needs to be figured out based on your specific geometry.
05:26
If you have a certain amount of threads that are going to be tapered and you need a full depth thread,
05:32
you need to calculate how deep your hole needs to go relative to the tap you're using.
05:37
And lastly the cycle needs to be changed to a tapping cycle.
05:41
This is extremely important as it slows down the spindle speed and also it synchronizes the spindle speed with the Z depth.
05:50
So this allows us to go to the bottom of the hole at the specific thread pitch
05:54
and then it will reverse the spindle as it's retracting out of the hole.
05:58
We're going to say okay. And now we've created our spot drilling, our drilling and our tapping operations.
06:05
At this point, we want to validate our tool numbers.
06:08
So we have tool one which is our large end mill tool to which was our 4 mm end mill.
06:13
And we have to all 3, 4 and 5 for spot drilling, drilling and tapping.
06:18
If we go back into our tool library, we have our library that we're using but we also have our CAD/CAM Milling dataset.
06:25
If we're going to carry on using these tools and we want to restructure the tool numbers.
06:30
We can modify them here by right clicking and re-numbering specific tools
06:35
or we can edit the tool and we can go to its post processor section to change the tool number.
06:41
Either option is going to be fine.
06:43
But when we're in the tool library and we're inside of our document, renumbering the tools,
06:49
in this case, using the re-number tool option allows us to pick the first tool and then we can change its offset value.
06:57
So it's important to note the options that we have.
07:01
But in our specific instance, we're going to carry on using these predefined tool numbers.
07:05
And that means that when we set up the machine, we need to make sure that the tool numbers match the specific cycles that are using them.
07:13
This helps us keep our tools in order inside of the tool changer.
07:17
And depending on the speed of your tool changer, this could save you a little bit of programming time.
07:23
We're going to save this design before moving on.
Video transcript
00:02
In this video, we're going to drill and tap.
00:06
After completing this step, you'll be able to create a spot drill operation, create a peck drill operation and create a tapping operation.
00:15
In Fusion 360, we want to carry on with our CAD/CAM Milling dataset.
00:19
At this point, we've gone all the way through the model, to rough and finish the major geometry and we've roughed and finish the slots.
00:27
Now we need to drill and tap all the holes in the design.
00:30
To do this, we're going to start by going to drilling and select the drill operation.
00:35
We need to select the proper tool so we'll go into our introduction library.
00:39
A note that we have a drill, a spot drill and then we have a tap.
00:43
For this operation, we're going to select the 5 mm spot drill.
00:47
One thing to note is none of the tools so far have had tool numbers which means that Fusion 360 is automatically going to increment them for us.
00:56
If you're starting fresh and don't have predefined tools inside of your machine, this can work.
01:01
However, it's always a good idea to define those tool numbers.
01:05
So once we're done programming the part we're going to go back and make some adjustments to these tool numbers.
01:10
Now that we have our tool selected, we need to move on to our geometry.
01:14
There are a few different ways that we can select holes in Fusion 360. We can manually select them based on faces.
01:21
We can use some other options such as selected points which allows us to select an edge
01:26
and it will automatically grab the center point or we can use the option to give it a diameter range.
01:33
We know that we're drilling a hole for an M5.
01:36
So if we set the lower end at 4 mm, noticed that it automatically grabbed all the holes for us and it knows exactly what the depth is.
01:45
We're going to move on to the heights section but note that we're using a spot drill.
01:49
So instead of using the whole bottom, I'm going to use the whole top and check the drill tip through bottom,
01:56
which allows the end of the spot drill to go through all the way up to the end of its taper.
02:01
This works for a smaller spot drill but if you have a larger spot drill, you want to be careful that you're not exceeding the diameter of the hole.
02:09
And lastly we needed to find the cycle. For us, drilling rapid out is going to work fine because we're barely taking the drill tip into the material.
02:17
So we're going to say, okay.
02:19
Now it starts at the red arrow and it moves its way all the way around until it gets to the green arrow.
02:26
Now we want to drill the holes so I'm going to right click on this drilling operation and duplicate it.
02:33
I'm going to select the duplicate right click and edit.
02:37
Now we're going to change our tool instead of using the spot drill, we want to use our 4.2 mm drill.
02:44
Once again, the drill bit doesn't have a tool number so it's automatically incremental.
02:50
The whole geometry is going to be the same.
02:52
However, I'm going to use the reverse order option
02:54
which means it's going to start at the hole that it finished the spot drilling and work its way backwards.
02:60
On this specific part, it's not going to make much of a difference because it could simply jump to the next location.
03:07
But depending on the specific hole pattern, this can save a lot of time.
03:11
Next, we want to make sure that we take a look at the heights and we use whole bottom.
03:17
It's also important to note that the whole bottom is going to be based on the entire depth of the hole.
03:24
And we need to keep in mind that these are tapped holes.
03:27
If we're drilling exactly to the whole bottom,
03:29
we don't want to tap to the whole bottom because we're going to be bottoming out the tap on solid geometry.
03:36
So we need to be real careful on the detailed drawing to see if we need the exact depth of threads or if we need the exact depth of the hole.
03:45
Depending on geometry on the other side of the part, one of them might be more important than the other.
03:51
We're going to be using the whole death as the bottom.
03:54
So we're going to move on to our cycle and we're going to change this to a different type of cycle
03:58
because we don't want to feed all the way through the hole.
04:01
We want to allow it to extract some chips.
04:03
There are two options that we have chip breaking partial were tracked and deep drilling.
04:09
The chip breaking partial retract will allow it to go down a set amount, come back slightly and then proceed to go down again.
04:16
When we use full retract, it'll use that same packing depth however, will retract completely out of the hole.
04:24
This helps evacuate chips from the hole and in some cases this is going to be more important.
04:29
However, for our case we're going to use the partial attract as this will work fine for our geometry.
04:34
Using the default settings for packing depth and amount we're going to say, okay.
04:40
Now that we've created our spot drill and our drilling operation, it's time to create our tapping operation.
04:46
I'm gonna right click and I'm gonna duplicate this one more time.
04:51
Then we're going to right click and edit the duplicate.
04:54
Now, instead of drilling we're going to use our 5 mm tap and we're going to select that tool.
05:01
In the geometry section we'll deselect reverse. So now we're starting at the original point working our way around.
05:08
In the heights section, we want to be careful of the whole bottom because again we don't want to bottom out the tap.
05:14
So I'm going to add a positive value of .5 mm. So that way the tap doesn't go all the way to the bottom.
05:22
This generally needs to be figured out based on your specific geometry.
05:26
If you have a certain amount of threads that are going to be tapered and you need a full depth thread,
05:32
you need to calculate how deep your hole needs to go relative to the tap you're using.
05:37
And lastly the cycle needs to be changed to a tapping cycle.
05:41
This is extremely important as it slows down the spindle speed and also it synchronizes the spindle speed with the Z depth.
05:50
So this allows us to go to the bottom of the hole at the specific thread pitch
05:54
and then it will reverse the spindle as it's retracting out of the hole.
05:58
We're going to say okay. And now we've created our spot drilling, our drilling and our tapping operations.
06:05
At this point, we want to validate our tool numbers.
06:08
So we have tool one which is our large end mill tool to which was our 4 mm end mill.
06:13
And we have to all 3, 4 and 5 for spot drilling, drilling and tapping.
06:18
If we go back into our tool library, we have our library that we're using but we also have our CAD/CAM Milling dataset.
06:25
If we're going to carry on using these tools and we want to restructure the tool numbers.
06:30
We can modify them here by right clicking and re-numbering specific tools
06:35
or we can edit the tool and we can go to its post processor section to change the tool number.
06:41
Either option is going to be fine.
06:43
But when we're in the tool library and we're inside of our document, renumbering the tools,
06:49
in this case, using the re-number tool option allows us to pick the first tool and then we can change its offset value.
06:57
So it's important to note the options that we have.
07:01
But in our specific instance, we're going to carry on using these predefined tool numbers.
07:05
And that means that when we set up the machine, we need to make sure that the tool numbers match the specific cycles that are using them.
07:13
This helps us keep our tools in order inside of the tool changer.
07:17
And depending on the speed of your tool changer, this could save you a little bit of programming time.
07:23
We're going to save this design 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.