& Construction

Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
& Manufacturing

Professional CAD/CAM tools built on Inventor and AutoCAD
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.
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.
Step-by-step guide