& 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 create Lathe chamfer toolpaths.
00:06
After completing this step, you'll be able to create a chamfer toolpath and create a new tool.
00:13
In Fusion 360, we want to carry on with our CAD CAM Lathe dataset.
00:17
We're going to get started by hiding this section analysis and we want to take a look at creating a chamfer toolpath.
00:23
We remove the champers from this model early on and this is going to make our selection process a little easier.
00:29
We're going to go to turning and select turning chamfer.
00:33
First, we want to select an appropriate tool from our introduction to CAD CAM Lathe toolset.
00:38
We'll select tool number 3 and select.
00:42
Next, we'll select our geometry which is going to be this front edge and this edge on the larger diameter.
00:49
We then needed to find our passes.
00:51
We're going to define the chamfer width two and then say okay.
00:55
This is going to define a chamfer toolpath and if we hide the models you can see the champers have now been cut.
01:01
Next we need to chamfer this inside edge but at this point it's problematic because we don't have the appropriate tool.
01:09
So we're gonna make a new tool and take care of any updates needed to our tool library.
01:14
First, we're going to go into our documents and CAD CAM Lathe dataset and note that tool number 11 is still listed as an M24 by 2.0.
01:23
So first we want to edit this tool and modify its description so that it represents our 25 mm tap.
01:31
Next we want to create tool number 12. To do this, we're going to select the plus icon and turning general.
01:39
First, I'm going to go to my insert section and I'm going to change the units to inch.
01:45
Just because our part is metric doesn't mean we have to use all metric tools.
01:49
It simply depends on what tools you have available.
01:52
We're going to be modifying this to use an off the shelf specific holder and toolset.
01:58
We're gonna start by changing the shape to M or an
02:03
The relief is going to be a C or 7 degrees.
02:07
We're going to leave the tolerance value at M and the type is going to be set to end.
02:13
From here, we're going to modify the insert size to be a number4 or a 0.5 inch.
02:19
Then we're going to modify the thickness to be a number 3 or 3/16 and the corner radius is going to be a 0.5.
02:28
Next we'll go to the holder set up and when we take a look at the holder, we're going to be modifying these values as well.
02:34
We're going to carry on using inches and we're going to set the style to custom, we're going to define the hand as right hand and rigid lock.
02:45
Then we want to begin to modify some of the parameters in the geometry section based on an off the shelf holder.
02:51
The cutting width is going to be 1.25 inches. The head length is going to be 1.2. The overall length will be 6 inches.
03:01
The shank width will be 1 inch, the trailing angle is going to be 0, but the leading angle is going to be 5.
03:08
And then the shank height value is going to be 1 inch.
03:12
Notice we also have a round shank option.
03:16
In our case, we're not going to be using the round shank option but we need to go to setup.
03:21
When we take a look at setup, we need to modify the orientation of the tool.
03:25
We can use these arrows to change the orientation based on how the tool is loaded inside of our holders.
03:32
In the cutting data section, we're going to be using all these presets.
03:35
But again it's important to understand that the cutting data needs to come from your tooling manufacturer
03:41
as well as testing that you do on your specific machines and tools.
03:46
And lastly in the post processor section we want to make sure that this is tool number 12.
03:51
And then we're going to select, okay.
03:54
Now that we have a new tool, we can select close and go to turning and select turning chamfer.
04:00
We're going to select our tool, tool number 12 and then we're going to modify to make sure that we are doing outside chamfering.
04:11
We're gonna move on to our geometry and we're going to select this edge here.
04:15
Then we're going to define the geometry at 2 mm.
04:19
I do want to move back to the first tab and note that when we define it as an external chamfer notice the direction the tool is going.
04:29
If we modify this to an inside chamfer, notice now how it's cutting in the opposite direction.
04:35
This is going to be a very important distinction.
04:37
And as we go through this process, we're going to note that the tool is likely to produce some problems based on our insert and our geometry.
04:45
But it's an important exercise for us to create these tools and validate their use inside of our program.
04:51
It's very easy for us to define the tool and even one without a holder and cut our geometry in Fusion
04:57
Get out to a machine and then it just doesn't work in reality.
05:01
So it's always a great idea to check everything out in the software before moving to the machine.
05:06
The in process stock doesn't necessarily show us everything we need to see.
05:10
So let's go to actions and select simulate and just take a quick look at this toolpath.
05:15
Notice that the insert is actually hitting this back edge.
05:19
So this is causing a problem because as the tool moves, it's cutting the geometry fine.
05:24
But as it begins to come out, the insert itself is hitting.
05:28
If we go to our tool definition and we show the holder itself, you can see that there's even more problems.
05:34
The tool just does not fit in the geometry needed because the holder is so large.
05:40
In order to fix this, we're going to go back into our toolpath.
05:44
We're going to edit and we're going to change the tool.
05:48
We're gonna go to our Fusion 360 library and we're gonna filter by our general tooling so we'll select turning general.
05:56
We're going to take a look at the options we have.
05:59
I'm going to select the "VNMT". Use the select option and note that we have a tool orientation in modes and directions.
06:09
This tool orientation is intended if your machine is able to change the tool angle.
06:14
Our machine is not. So I'm going to select "OK".
06:17
And then I'm going to go and modify the tool itself.
06:22
When I modify the tool, I need to go to set up and I need to change the direction the tools coming from.
06:28
I'm also going to go to post processor and set this at tool number 13 and then accept.
06:35
Will select the toolpath and regenerate and we'll go back to simulate to see if this alleviated the problem.
06:43
Now you can see that the tool comes in.
06:45
It goes into chamfer but the holder itself is causing problems.
06:55
Again, depending on the tools you have available. This type of geometry might be problematic.
07:01
Another thing that we can try is to use a different tool.
07:05
We do have our boring bar that was used to board the inside and we can select this and we can give this a shot.
07:12
The geometry of our boring bars obviously small enough to fit inside
07:16
and it shouldn't cause any problems assuming that the boring bar itself and the insert can handle the cut we're asking.
07:23
What I would generally do is likely start from the inside and just make sure that the tool fits all the way inside without causing any issues.
07:33
We can hide our model and we can make sure that the geometry being cut is okay.
07:38
You'll note that the tool is pulling extremely far away from the cut and it's really going quite a bit further.
07:44
That's going to be defined inside of our toolpath based on the radii values on the third tab.
07:51
Those clearance and retract values need to be based off of real numbers.
07:55
So for our clearance and our retract, we're going to get started by first defining the clearance based on a selection.
08:02
We'll grab the inside and then we're going to modify the retract from a selection as well
08:08
and notice that the inner radius is also based off the stock ID.
08:12
So I'm going to use this as my selection and say, okay.
08:17
Also note that the tool does more complete retract but it's not going quite as far away.
08:23
So the geometry being cut looks a little bit better but we need to validate this.
08:28
So the tool comes in, makes the cut, pulls over, but it's not getting quite far enough in.
08:34
So you can see that we don't have that intersection issue anymore.
08:39
Again, it's important that we test this out in Fusion machine.
08:45
As we need to validate all of the clearances and values for all the tools that we're using.
08:50
In this case, let's make a save and then we can move on to the next step.
Video transcript
00:02
In this video, we'll create Lathe chamfer toolpaths.
00:06
After completing this step, you'll be able to create a chamfer toolpath and create a new tool.
00:13
In Fusion 360, we want to carry on with our CAD CAM Lathe dataset.
00:17
We're going to get started by hiding this section analysis and we want to take a look at creating a chamfer toolpath.
00:23
We remove the champers from this model early on and this is going to make our selection process a little easier.
00:29
We're going to go to turning and select turning chamfer.
00:33
First, we want to select an appropriate tool from our introduction to CAD CAM Lathe toolset.
00:38
We'll select tool number 3 and select.
00:42
Next, we'll select our geometry which is going to be this front edge and this edge on the larger diameter.
00:49
We then needed to find our passes.
00:51
We're going to define the chamfer width two and then say okay.
00:55
This is going to define a chamfer toolpath and if we hide the models you can see the champers have now been cut.
01:01
Next we need to chamfer this inside edge but at this point it's problematic because we don't have the appropriate tool.
01:09
So we're gonna make a new tool and take care of any updates needed to our tool library.
01:14
First, we're going to go into our documents and CAD CAM Lathe dataset and note that tool number 11 is still listed as an M24 by 2.0.
01:23
So first we want to edit this tool and modify its description so that it represents our 25 mm tap.
01:31
Next we want to create tool number 12. To do this, we're going to select the plus icon and turning general.
01:39
First, I'm going to go to my insert section and I'm going to change the units to inch.
01:45
Just because our part is metric doesn't mean we have to use all metric tools.
01:49
It simply depends on what tools you have available.
01:52
We're going to be modifying this to use an off the shelf specific holder and toolset.
01:58
We're gonna start by changing the shape to M or an
02:03
The relief is going to be a C or 7 degrees.
02:07
We're going to leave the tolerance value at M and the type is going to be set to end.
02:13
From here, we're going to modify the insert size to be a number4 or a 0.5 inch.
02:19
Then we're going to modify the thickness to be a number 3 or 3/16 and the corner radius is going to be a 0.5.
02:28
Next we'll go to the holder set up and when we take a look at the holder, we're going to be modifying these values as well.
02:34
We're going to carry on using inches and we're going to set the style to custom, we're going to define the hand as right hand and rigid lock.
02:45
Then we want to begin to modify some of the parameters in the geometry section based on an off the shelf holder.
02:51
The cutting width is going to be 1.25 inches. The head length is going to be 1.2. The overall length will be 6 inches.
03:01
The shank width will be 1 inch, the trailing angle is going to be 0, but the leading angle is going to be 5.
03:08
And then the shank height value is going to be 1 inch.
03:12
Notice we also have a round shank option.
03:16
In our case, we're not going to be using the round shank option but we need to go to setup.
03:21
When we take a look at setup, we need to modify the orientation of the tool.
03:25
We can use these arrows to change the orientation based on how the tool is loaded inside of our holders.
03:32
In the cutting data section, we're going to be using all these presets.
03:35
But again it's important to understand that the cutting data needs to come from your tooling manufacturer
03:41
as well as testing that you do on your specific machines and tools.
03:46
And lastly in the post processor section we want to make sure that this is tool number 12.
03:51
And then we're going to select, okay.
03:54
Now that we have a new tool, we can select close and go to turning and select turning chamfer.
04:00
We're going to select our tool, tool number 12 and then we're going to modify to make sure that we are doing outside chamfering.
04:11
We're gonna move on to our geometry and we're going to select this edge here.
04:15
Then we're going to define the geometry at 2 mm.
04:19
I do want to move back to the first tab and note that when we define it as an external chamfer notice the direction the tool is going.
04:29
If we modify this to an inside chamfer, notice now how it's cutting in the opposite direction.
04:35
This is going to be a very important distinction.
04:37
And as we go through this process, we're going to note that the tool is likely to produce some problems based on our insert and our geometry.
04:45
But it's an important exercise for us to create these tools and validate their use inside of our program.
04:51
It's very easy for us to define the tool and even one without a holder and cut our geometry in Fusion
04:57
Get out to a machine and then it just doesn't work in reality.
05:01
So it's always a great idea to check everything out in the software before moving to the machine.
05:06
The in process stock doesn't necessarily show us everything we need to see.
05:10
So let's go to actions and select simulate and just take a quick look at this toolpath.
05:15
Notice that the insert is actually hitting this back edge.
05:19
So this is causing a problem because as the tool moves, it's cutting the geometry fine.
05:24
But as it begins to come out, the insert itself is hitting.
05:28
If we go to our tool definition and we show the holder itself, you can see that there's even more problems.
05:34
The tool just does not fit in the geometry needed because the holder is so large.
05:40
In order to fix this, we're going to go back into our toolpath.
05:44
We're going to edit and we're going to change the tool.
05:48
We're gonna go to our Fusion 360 library and we're gonna filter by our general tooling so we'll select turning general.
05:56
We're going to take a look at the options we have.
05:59
I'm going to select the "VNMT". Use the select option and note that we have a tool orientation in modes and directions.
06:09
This tool orientation is intended if your machine is able to change the tool angle.
06:14
Our machine is not. So I'm going to select "OK".
06:17
And then I'm going to go and modify the tool itself.
06:22
When I modify the tool, I need to go to set up and I need to change the direction the tools coming from.
06:28
I'm also going to go to post processor and set this at tool number 13 and then accept.
06:35
Will select the toolpath and regenerate and we'll go back to simulate to see if this alleviated the problem.
06:43
Now you can see that the tool comes in.
06:45
It goes into chamfer but the holder itself is causing problems.
06:55
Again, depending on the tools you have available. This type of geometry might be problematic.
07:01
Another thing that we can try is to use a different tool.
07:05
We do have our boring bar that was used to board the inside and we can select this and we can give this a shot.
07:12
The geometry of our boring bars obviously small enough to fit inside
07:16
and it shouldn't cause any problems assuming that the boring bar itself and the insert can handle the cut we're asking.
07:23
What I would generally do is likely start from the inside and just make sure that the tool fits all the way inside without causing any issues.
07:33
We can hide our model and we can make sure that the geometry being cut is okay.
07:38
You'll note that the tool is pulling extremely far away from the cut and it's really going quite a bit further.
07:44
That's going to be defined inside of our toolpath based on the radii values on the third tab.
07:51
Those clearance and retract values need to be based off of real numbers.
07:55
So for our clearance and our retract, we're going to get started by first defining the clearance based on a selection.
08:02
We'll grab the inside and then we're going to modify the retract from a selection as well
08:08
and notice that the inner radius is also based off the stock ID.
08:12
So I'm going to use this as my selection and say, okay.
08:17
Also note that the tool does more complete retract but it's not going quite as far away.
08:23
So the geometry being cut looks a little bit better but we need to validate this.
08:28
So the tool comes in, makes the cut, pulls over, but it's not getting quite far enough in.
08:34
So you can see that we don't have that intersection issue anymore.
08:39
Again, it's important that we test this out in Fusion machine.
08:45
As we need to validate all of the clearances and values for all the tools that we're using.
08:50
In this case, let's make a save and then we can move on to the next step.
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.