Lathe drill and boring toolpaths

00:02

In this video, we'll create Lathe drill and bore toolpaths.

00:06

After completing this step, you'll be able to create a drill operation and create a boring toolpath.

00:14

In Fusion 360, we want to carry on with our CAD/CAM Lathe dataset.

00:18

At this point we've faced the front we've created in profile roughing and finishing toolpaths and we've created a single groove on the outside.

00:26

Now we want to drill and bore the inside before we get to threading and internal grooving.

00:31

To get started, we're gonna go to drilling and select drill.

00:35

We need to first select our tool and we'll do that by navigating to the Fusion 360 library.

00:40

Then using the diameter filter on only drills. Setting it equal to 18 mm.

00:49

We're going to select 18 mm and aluminum drilling.

00:53

The next thing that we want to do is we want to select the geometry.

00:56

So in the second tab we'll select the inside portion of the hole.

01:01

It's important to note that this hole goes a little bit deeper because of the groove,

01:05

but we're going to be using our boring tool to go all the way down.

01:08

If I view this from the front, you can see here that this goes to the bottom of our hole, however, we actually need to go a little bit deeper.

01:17

I'm going to be using the option on my heights and selecting drill tip through bottom.

01:23

We're going to make some adjustments to the drill bit.

01:25

So for right now we're just going to simply allow it to go a bit deeper and we'll come back to make our final adjustments in a minute,

01:32

we're going to say okay, and then inside of the toolpath we're gonna right click and edit our tool.

01:38

We're going to be taking a look at this as if it's a you drill or an insert type drill.

01:44

This means that there's not going to be a taper on the end and instead of 118 degrees, we're going to set this at 180 degrees.

01:52

This will create a perfectly flat end and this will allow us to go in feed all the way to the bottom of the hole.

01:58

And it will allow us to do this without pilot drilling the hole.

02:03

We're going to accept this. And then we also need to make an adjustment to the toolpath itself.

02:08

In the heights, we want to make sure that the whole bottom is not actually where we're going to.

02:13

Instead we're going to go all the way to the base where our groove is because the drill is now flat on the bottom.

02:19

The drill tip through bottom is not going to make any adjustments.

02:23

So we need to use the selection option and select the area we want to go to.

02:28

In the cycle section because this is an insert drill, we're going to be using the drilling and wrap it out.

02:34

This allows us to feed to the depth that we specified and then rapidly remove the tool from the hole.

02:39

If we were using a standard type drill, we would want to try something like a partial retract or deep drilling,

02:46

we'll say okay and allow it to create the operation.

02:50

Now that we've drilled most of the material away from the whole, let's do inspect and measure and remind ourselves what size hole we're dealing with.

02:58

It's a 23 mm hole because it's for an internal 25 mm threat.

03:04

So I want to use a boring bar to remove the rest of the material from the inside, before I create our groove.

03:10

To do this, I'll go to turning and select turning profile roughing.

03:16

I need to first select an appropriate tool and to do this, we'll go into our introduction to CAD/CAM Lathe and select our internal boring tool.

03:25

In this case it's tool number six and we're going to have to make some adjustments to this tool.

03:29

But let's get started by making sure that we're doing inside profiling and then we can select our geometry.

03:36

Noting that we don't actually select the inside of the hole, but rather we need to adjust how far we want to allow the tool to look for geometry.

03:46

I'm going to bring this plane just to the back of this groove.

03:52

And I'm going to rotate this around and also use the rest machining option from previous operation. I want to say, okay.

04:00

And now note that we are boring but we have a tool that's just a little too large to fit.

04:07

You'll notice that we have a warning and this is telling us that the toolpath crosses the rotary axis.

04:12

It's not telling us anything about the clearance issues with the tool.

04:16

Let's go ahead and make some adjustments to the tool first and then we'll modify the toolpath once more, we're gonna right click and edit our tool.

04:24

We need to make some adjustments based on available boring bars that will fit inside of this part.

04:30

On the insert section, I'm going to change the units from mm to inches because this is what I have available.

04:36

Then I'm going to begin defining the tool.

04:38

The shape is going to be C and I'm going to modify the relief angle to B which is 5 degrees.

04:44

Note that it's highlighting this measurement on the screen. Tolerance and cross section will be the same.

04:50

However, the insert size that we want to use is a two which is a quarter inch insert.

04:55

The thickness that we're going to be using is a number five, which is a 5/16. And the corner radius that we're going to be using is a .5.

05:05

Once we have these defined we also need to modify our holders set up once again make sure that we're in inches

05:12

and now let's take a look at some of the settings that we can change.

05:16

We'll still be using the style L which is a negative five degree. Then we want to make sure that we're using a right handed tool.

05:24

And we're also using the clamping method D or rigid lock.

05:29

But we do need to modify some of these values.

05:32

When we click on them, notice that it's showing a metric value because the document units are metric.

05:37

But in this case we can manually enter a value and in our case it's going to be .234 inches.

05:44

I'm going to hit tab to go to the next box and the head length is going to be 3/8 or .375.

05:50

The overall length is fine. However, the shank width is also .375.

05:56

You can see that makes a much smaller tool.

05:59

Next, in the setup section, we want to make sure that we're using are clockwise spindle orientation.

06:04

Notice how it flips the tool over and this is based on the orientation of the tool and the rotation of our spindle.

06:12

From here, let's go ahead and accept the change.

06:15

Say yes because we do want to update our toolpaths

06:18

and let's select our profile roughing and use control or command G or select generate from the action section.

06:25

Notice now that it does machine the area of concern and we do have some warnings.

06:31

It still tells us that the toolpath crosses the rotary axis.

06:34

So I'm going to modify the toolpath and take a look at our radii.

06:40

Right now the inner radii is set to zero and we're going to modify that value.

06:46

Make sure that we set the inner radii to a manual value.

06:50

I'm gonna use diameter. And notice that the offset value is 0.

06:55

We're gonna set this to 18 mm.

06:58

Also notice our clearance is based on the stock -10 mm.

07:03

Instead of that, I'm going to use a selection.

07:05

I'm going to select the inside diameter and notice that I have a very small clearance value here but I'm going to set this to -5 mm instead of 10.

07:15

We also want to double check our passes as we are leaving stock behind.

07:19

This is a roughing operation but I am going to remove stock to leave because we're going to come back and tap this hole.

07:26

I do want to make sure that I don't take too many cuts out at once because I still need a good consistent finish.

07:34

And also note that we're not going to allow grooving.

07:37

We don't want the tool to try to go into the groove and potentially mess up some of the other geometry

07:42

and this is something we're going to have to come back in machine anyways.

07:46

We're going to say, okay, allow it to regenerate and note that we no longer have a warning about crossing the rotary axis.

07:53

I do want to make one more note before we move on and that's with our drill bit.

07:58

Let's go ahead and right click and edit the tool.

08:01

First, I want to go to post processor and change the tool number to tool number 10.

08:06

Next, I want to go to the settings down below the tool numbers and note that we have something called live tool.

08:13

Live tool is a setting that will dictate whether or not the tool will be spinning.

08:19

In our case, when we post this, it's going to be specific to a certain machine.

08:24

If we post this out to an accumulate this might not make a difference.

08:28

However if we post it to [] slave it will define the spindle speed of the drill bit in a live tooling situation.

08:36

If we deselect that and we go back and repost the code, it's going to define the spindle speed of the spindle holding our part.

08:45

So it's important to understand the functionality of your specific machine and what settings are required.

08:51

Let's go ahead and accept this.

08:53

I'm going to minimize both the drilling and the profile roughing. And I want to rename profile roughing 2 and I'm going to call it bore.

09:03

And then I want to make sure that we save the design before moving on.

Video transcript

00:02

In this video, we'll create Lathe drill and bore toolpaths.

00:06

After completing this step, you'll be able to create a drill operation and create a boring toolpath.

00:14

In Fusion 360, we want to carry on with our CAD/CAM Lathe dataset.

00:18

At this point we've faced the front we've created in profile roughing and finishing toolpaths and we've created a single groove on the outside.

00:26

Now we want to drill and bore the inside before we get to threading and internal grooving.

00:31

To get started, we're gonna go to drilling and select drill.

00:35

We need to first select our tool and we'll do that by navigating to the Fusion 360 library.

00:40

Then using the diameter filter on only drills. Setting it equal to 18 mm.

00:49

We're going to select 18 mm and aluminum drilling.

00:53

The next thing that we want to do is we want to select the geometry.

00:56

So in the second tab we'll select the inside portion of the hole.

01:01

It's important to note that this hole goes a little bit deeper because of the groove,

01:05

but we're going to be using our boring tool to go all the way down.

01:08

If I view this from the front, you can see here that this goes to the bottom of our hole, however, we actually need to go a little bit deeper.

01:17

I'm going to be using the option on my heights and selecting drill tip through bottom.

01:23

We're going to make some adjustments to the drill bit.

01:25

So for right now we're just going to simply allow it to go a bit deeper and we'll come back to make our final adjustments in a minute,

01:32

we're going to say okay, and then inside of the toolpath we're gonna right click and edit our tool.

01:38

We're going to be taking a look at this as if it's a you drill or an insert type drill.

01:44

This means that there's not going to be a taper on the end and instead of 118 degrees, we're going to set this at 180 degrees.

01:52

This will create a perfectly flat end and this will allow us to go in feed all the way to the bottom of the hole.

01:58

And it will allow us to do this without pilot drilling the hole.

02:03

We're going to accept this. And then we also need to make an adjustment to the toolpath itself.

02:08

In the heights, we want to make sure that the whole bottom is not actually where we're going to.

02:13

Instead we're going to go all the way to the base where our groove is because the drill is now flat on the bottom.

02:19

The drill tip through bottom is not going to make any adjustments.

02:23

So we need to use the selection option and select the area we want to go to.

02:28

In the cycle section because this is an insert drill, we're going to be using the drilling and wrap it out.

02:34

This allows us to feed to the depth that we specified and then rapidly remove the tool from the hole.

02:39

If we were using a standard type drill, we would want to try something like a partial retract or deep drilling,

02:46

we'll say okay and allow it to create the operation.

02:50

Now that we've drilled most of the material away from the whole, let's do inspect and measure and remind ourselves what size hole we're dealing with.

02:58

It's a 23 mm hole because it's for an internal 25 mm threat.

03:04

So I want to use a boring bar to remove the rest of the material from the inside, before I create our groove.

03:10

To do this, I'll go to turning and select turning profile roughing.

03:16

I need to first select an appropriate tool and to do this, we'll go into our introduction to CAD/CAM Lathe and select our internal boring tool.

03:25

In this case it's tool number six and we're going to have to make some adjustments to this tool.

03:29

But let's get started by making sure that we're doing inside profiling and then we can select our geometry.

03:36

Noting that we don't actually select the inside of the hole, but rather we need to adjust how far we want to allow the tool to look for geometry.

03:46

I'm going to bring this plane just to the back of this groove.

03:52

And I'm going to rotate this around and also use the rest machining option from previous operation. I want to say, okay.

04:00

And now note that we are boring but we have a tool that's just a little too large to fit.

04:07

You'll notice that we have a warning and this is telling us that the toolpath crosses the rotary axis.

04:12

It's not telling us anything about the clearance issues with the tool.

04:16

Let's go ahead and make some adjustments to the tool first and then we'll modify the toolpath once more, we're gonna right click and edit our tool.

04:24

We need to make some adjustments based on available boring bars that will fit inside of this part.

04:30

On the insert section, I'm going to change the units from mm to inches because this is what I have available.

04:36

Then I'm going to begin defining the tool.

04:38

The shape is going to be C and I'm going to modify the relief angle to B which is 5 degrees.

04:44

Note that it's highlighting this measurement on the screen. Tolerance and cross section will be the same.

04:50

However, the insert size that we want to use is a two which is a quarter inch insert.

04:55

The thickness that we're going to be using is a number five, which is a 5/16. And the corner radius that we're going to be using is a .5.

05:05

Once we have these defined we also need to modify our holders set up once again make sure that we're in inches

05:12

and now let's take a look at some of the settings that we can change.

05:16

We'll still be using the style L which is a negative five degree. Then we want to make sure that we're using a right handed tool.

05:24

And we're also using the clamping method D or rigid lock.

05:29

But we do need to modify some of these values.

05:32

When we click on them, notice that it's showing a metric value because the document units are metric.

05:37

But in this case we can manually enter a value and in our case it's going to be .234 inches.

05:44

I'm going to hit tab to go to the next box and the head length is going to be 3/8 or .375.

05:50

The overall length is fine. However, the shank width is also .375.

05:56

You can see that makes a much smaller tool.

05:59

Next, in the setup section, we want to make sure that we're using are clockwise spindle orientation.

06:04

Notice how it flips the tool over and this is based on the orientation of the tool and the rotation of our spindle.

06:12

From here, let's go ahead and accept the change.

06:15

Say yes because we do want to update our toolpaths

06:18

and let's select our profile roughing and use control or command G or select generate from the action section.

06:25

Notice now that it does machine the area of concern and we do have some warnings.

06:31

It still tells us that the toolpath crosses the rotary axis.

06:34

So I'm going to modify the toolpath and take a look at our radii.

06:40

Right now the inner radii is set to zero and we're going to modify that value.

06:46

Make sure that we set the inner radii to a manual value.

06:50

I'm gonna use diameter. And notice that the offset value is 0.

06:55

We're gonna set this to 18 mm.

06:58

Also notice our clearance is based on the stock -10 mm.

07:03

Instead of that, I'm going to use a selection.

07:05

I'm going to select the inside diameter and notice that I have a very small clearance value here but I'm going to set this to -5 mm instead of 10.

07:15

We also want to double check our passes as we are leaving stock behind.

07:19

This is a roughing operation but I am going to remove stock to leave because we're going to come back and tap this hole.

07:26

I do want to make sure that I don't take too many cuts out at once because I still need a good consistent finish.

07:34

And also note that we're not going to allow grooving.

07:37

We don't want the tool to try to go into the groove and potentially mess up some of the other geometry

07:42

and this is something we're going to have to come back in machine anyways.

07:46

We're going to say, okay, allow it to regenerate and note that we no longer have a warning about crossing the rotary axis.

07:53

I do want to make one more note before we move on and that's with our drill bit.

07:58

Let's go ahead and right click and edit the tool.

08:01

First, I want to go to post processor and change the tool number to tool number 10.

08:06

Next, I want to go to the settings down below the tool numbers and note that we have something called live tool.

08:13

Live tool is a setting that will dictate whether or not the tool will be spinning.

08:19

In our case, when we post this, it's going to be specific to a certain machine.

08:24

If we post this out to an accumulate this might not make a difference.

08:28

However if we post it to [] slave it will define the spindle speed of the drill bit in a live tooling situation.

08:36

If we deselect that and we go back and repost the code, it's going to define the spindle speed of the spindle holding our part.

08:45

So it's important to understand the functionality of your specific machine and what settings are required.

08:51

Let's go ahead and accept this.

08:53

I'm going to minimize both the drilling and the profile roughing. And I want to rename profile roughing 2 and I'm going to call it bore.

09:03

And then I want to make sure that we save the design before moving on.

Video quiz

For an internal boring operation, which setting in the Radii tab of a Turning Profile Roughing operation will keep the tool from crossing the rotary axis?

(Select one)
Select an answer

1/1 questions left unanswered

Step-by-step guide

It appears you don't have a PDF plugin for this browser.

Was this information helpful?