Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
Professional CAD/CAM tools built on Inventor and AutoCAD
Any referenced datasets can be downloaded from "Module downloads" in the module overview.
Transcript
00:08
Now that we have our features created, let's simulate the machining of these features and make any revisions necessary.
00:16
Simulations in FeatureCAM not only provide us with a visual representation of our toolpath, but while simulations are running in the background, FeatureCAM is calculating our NC Code to machine our part.
00:28
Now there's a few different types of simulations in FeatureCAM, but for this class, we’ll be sticking to what I find are the two most useful.
00:36
Navigate to the Home tab in your ribbon and find the simulation section.
00:41
Here, we'll see a drop-down titled Sim Mode.
00:44
This is where we select what type of simulation we'd like to run.
00:47
In this course, we’ll first look at centerline simulations, which give us a wire diagram of our toolpath, and 3D simulations, which give us a 3D representation of what the machining of our part will look like.
01:03
So let's start by selecting centerline.
01:05
And then you'll see at the bottom of our graphics window, we have simple DVD style controls to run our simulation.
01:12
I’ll press "Play", and we can see the wire diagram toolpath generated during that centerline simulation.
01:19
Now, you may have noticed that that simulation went by really quick.
01:23
So let's select stop and eject that simulation.
01:26
And let's look at the slider on the right hand side of our simulation options and let's slide it all the way to the left.
01:33
This is our simulation speed.
01:36
So now this is a simple part.
01:37
So as I press "Play", it'll still go by quickly.
01:41
But now we can see the toolpath has been slowed down, we're getting a better idea of what our toolpaths will look like.
01:48
Another thing you may notice about centerline simulations is that some of the wire diagram toolpath is black and some of it is green.
01:56
I'm going to right click and take an isometric view.
01:59
And here we can see our green toolpath happens above our part and the black toolpath seems to happen while our features are being machined.
02:09
As you may expect, green toolpath in FeatureCAM indicates rapid movements, while black toolpath indicates feeding movements.
02:18
So in general, when you see black toolpath in a centerline simulation, machining is happening.
02:24
And when you see green toolpath, the tool is simply rapiding around the part.
02:29
Now let's take a look at the other simulation type we’ll be using a lot in this class.
02:33
I'll stop and eject the simulation.
02:36
Go back up to the Sim mode in our simulation section and select 3D.
02:43
Let's bring the slider all the way back to the left and hit "Play" to watch the machining of this part.
02:57
Now obviously, these 3D simulations give us a good idea of what the actual machining of our part will look like from our aluminum block.
03:05
We saw our end mill come in, cut our triangular pocket, our center drills come in and spot drill the four holes.
03:12
And finally, our twist drill machine out those four remaining holes.
03:17
Now while 3D simulations are really helpful for visualizing the actual machining of our part, they're not just pretty pictures.
03:31
So at any point, for some reason, we accidentally rapid it into our aluminum block, a warning would have been thrown and FeatureCAM would have let us know that this code is not safe and should not be sent to the machine.
03:45
It looks like we didn't get any warnings in this case, so we should be good to go.
03:49
As I mentioned earlier, these simulations drive the calculation of our NC Code.
03:55
Our NC Code can be found on the right side in our results fly-out.
03:60
In the results fly-out at the bottom, you'll notice a tab titled NC Code.
04:05
So while the simulation ran, all of this NC Code was calculated and posted into our results fly-out.
04:12
We do have NC Code ready to be sent to our machine to machine this part.
04:15
But first, let's make a couple of revisions.
04:19
I'm going to click on results here to get rid of our fly-out menu, eject this simulation, and I'm going to open up our Pocket Properties window, by double clicking pocket 1 on the left hand side of our user interface in the Part View section.
04:33
The big change I want to make here is let's add a chamfer to the top edge of this pocket.
04:39
To do so, you'll notice I'm just on the dimensions page of our Pocket Properties window.
04:44
I can come here to the chamfer parameter, and let's enter in a chamfer of 0.05.
04:52
As I click "Apply", notice on the left, an entirely new operation has been created for us, our chamfer operation.
04:59
If I select the chamfer operation, we can see a tool has been selected for this chamfer operation, feeds and speeds have been calculated, stepovers have been automatically entered, as well as any milling attributes.
05:13
We'll dig through these menus a little bit later, but the same holds true for our roughing and finishing operation.
05:21
Tools, feeds and speeds, stepovers, and so on have all been calculated for us.
05:27
So with that, as I press "OK" and run another 3D simulation, we can see our pocket is milled out just like it was before.
05:39
And then it is chamfered on that top edge before moving on to the drilling.
05:45
So with that small change, we've added an entire new operation to the machining of our part, just with a couple of clicks.
05:53
Similarly, let's now change the holes.
05:56
I'll open up hole 1 in my Part View section.
06:00
And rather than doing a plain hole, let's select this fly-out and let's turn it into a tapped hole.
06:07
You'll notice that as I select tapped hole, my dimensions page changes accordingly.
06:12
Obviously, because tapped holes require different inputs than just a plain hole.
06:17
Let's keep our major diameter of a quarter of an inch and our depth of an inch.
06:24
And then rather than entering in exact TPI and then rather than entering in an exact pitch, if I select standard thread, I can select from a long list of predefined thread sizes in FeatureCAM.
06:39
This helps us eliminate any error on our end by selecting a standardized hole size.
06:45
For this, let's just go with this 1/4-20 hole.
06:48
We can see that my diameter section has been locked to a quarter inch and my pitch section has been locked to 20.
06:55
Now all I can control is my thread depth and hole depth and chamfer.
07:00
Let's keep a thread depth of three quarters of an inch and a hole depth of one inch.
07:06
With that, I'll hit "Apply", "Ok", and run another 3D simulation.
07:23
As you may have noticed, we added that entire tap cycle and we went around spot drilled each of the four holes, then drilled each of the four holes, and finally tapped each of the four holes.
07:34
With both of our features revised and modified, and the simulations checked off, let's make one last change to the machining of this part before we send our NC Code to the machine.
07:45
I’ll eject this simulation and the last thing I want to do is you may have noticed we didn't add a facing operation at the beginning of this part.
07:54
Right now, if I open up my results fly-out and look at our operation list, we'll see that we rough our pocket and finish it before chamfering.
08:04
We spot drill our holes, drill our holes, and then tap our holes, but at no point did we clean off the top face of this part.
08:11
So right now, let's add a facing operation to this part before we post our NC Code.
08:17
I'll open up the new feature wizard, simply select Face from Dimensions, "Next", let's just locate this face feature as Z equals zero to clean up any excess material on this part.
08:31
By default, FeatureCAM has entered in a facing thickness of 0.02.
08:36
If I had located it below the face of my stock, it would have calculated that thickness.
08:41
In this case, let's just enter in a thickness of 0.02 since we don't know how much extra material we may have on this part.
08:48
Well, you notice on our strategies page, by default, we're just going to create a finish pass with our face operation.
08:55
That's fine.
08:56
And with our final operation confirmed, we'll press "Finish", "OK".
09:02
And notice that the face operation in the operations list has been placed at the very beginning of the machining of this part.
09:09
This is a good example of FeatureCAM’s built-in intelligence and automation.
09:14
FeatureCAM knows that generally when you're machining with a face operation, you want that located at the very beginning of your program, and has made the change necessary.
09:23
With both of our features modified, our face feature created, we're ready to run a final simulation.
09:44
Looks good.
09:45
We successfully worked through the simulate and revise section of our workflow.
09:50
The idea here is that we simulate our toolpath not only to generate NC Code, but to make sure we like how our part's being machined, make any revisions necessary, and then simulate those revisions over and over again until we have a final part that we're ready to post NC Code and send to our machine.
Video transcript
00:08
Now that we have our features created, let's simulate the machining of these features and make any revisions necessary.
00:16
Simulations in FeatureCAM not only provide us with a visual representation of our toolpath, but while simulations are running in the background, FeatureCAM is calculating our NC Code to machine our part.
00:28
Now there's a few different types of simulations in FeatureCAM, but for this class, we’ll be sticking to what I find are the two most useful.
00:36
Navigate to the Home tab in your ribbon and find the simulation section.
00:41
Here, we'll see a drop-down titled Sim Mode.
00:44
This is where we select what type of simulation we'd like to run.
00:47
In this course, we’ll first look at centerline simulations, which give us a wire diagram of our toolpath, and 3D simulations, which give us a 3D representation of what the machining of our part will look like.
01:03
So let's start by selecting centerline.
01:05
And then you'll see at the bottom of our graphics window, we have simple DVD style controls to run our simulation.
01:12
I’ll press "Play", and we can see the wire diagram toolpath generated during that centerline simulation.
01:19
Now, you may have noticed that that simulation went by really quick.
01:23
So let's select stop and eject that simulation.
01:26
And let's look at the slider on the right hand side of our simulation options and let's slide it all the way to the left.
01:33
This is our simulation speed.
01:36
So now this is a simple part.
01:37
So as I press "Play", it'll still go by quickly.
01:41
But now we can see the toolpath has been slowed down, we're getting a better idea of what our toolpaths will look like.
01:48
Another thing you may notice about centerline simulations is that some of the wire diagram toolpath is black and some of it is green.
01:56
I'm going to right click and take an isometric view.
01:59
And here we can see our green toolpath happens above our part and the black toolpath seems to happen while our features are being machined.
02:09
As you may expect, green toolpath in FeatureCAM indicates rapid movements, while black toolpath indicates feeding movements.
02:18
So in general, when you see black toolpath in a centerline simulation, machining is happening.
02:24
And when you see green toolpath, the tool is simply rapiding around the part.
02:29
Now let's take a look at the other simulation type we’ll be using a lot in this class.
02:33
I'll stop and eject the simulation.
02:36
Go back up to the Sim mode in our simulation section and select 3D.
02:43
Let's bring the slider all the way back to the left and hit "Play" to watch the machining of this part.
02:57
Now obviously, these 3D simulations give us a good idea of what the actual machining of our part will look like from our aluminum block.
03:05
We saw our end mill come in, cut our triangular pocket, our center drills come in and spot drill the four holes.
03:12
And finally, our twist drill machine out those four remaining holes.
03:17
Now while 3D simulations are really helpful for visualizing the actual machining of our part, they're not just pretty pictures.
03:31
So at any point, for some reason, we accidentally rapid it into our aluminum block, a warning would have been thrown and FeatureCAM would have let us know that this code is not safe and should not be sent to the machine.
03:45
It looks like we didn't get any warnings in this case, so we should be good to go.
03:49
As I mentioned earlier, these simulations drive the calculation of our NC Code.
03:55
Our NC Code can be found on the right side in our results fly-out.
03:60
In the results fly-out at the bottom, you'll notice a tab titled NC Code.
04:05
So while the simulation ran, all of this NC Code was calculated and posted into our results fly-out.
04:12
We do have NC Code ready to be sent to our machine to machine this part.
04:15
But first, let's make a couple of revisions.
04:19
I'm going to click on results here to get rid of our fly-out menu, eject this simulation, and I'm going to open up our Pocket Properties window, by double clicking pocket 1 on the left hand side of our user interface in the Part View section.
04:33
The big change I want to make here is let's add a chamfer to the top edge of this pocket.
04:39
To do so, you'll notice I'm just on the dimensions page of our Pocket Properties window.
04:44
I can come here to the chamfer parameter, and let's enter in a chamfer of 0.05.
04:52
As I click "Apply", notice on the left, an entirely new operation has been created for us, our chamfer operation.
04:59
If I select the chamfer operation, we can see a tool has been selected for this chamfer operation, feeds and speeds have been calculated, stepovers have been automatically entered, as well as any milling attributes.
05:13
We'll dig through these menus a little bit later, but the same holds true for our roughing and finishing operation.
05:21
Tools, feeds and speeds, stepovers, and so on have all been calculated for us.
05:27
So with that, as I press "OK" and run another 3D simulation, we can see our pocket is milled out just like it was before.
05:39
And then it is chamfered on that top edge before moving on to the drilling.
05:45
So with that small change, we've added an entire new operation to the machining of our part, just with a couple of clicks.
05:53
Similarly, let's now change the holes.
05:56
I'll open up hole 1 in my Part View section.
06:00
And rather than doing a plain hole, let's select this fly-out and let's turn it into a tapped hole.
06:07
You'll notice that as I select tapped hole, my dimensions page changes accordingly.
06:12
Obviously, because tapped holes require different inputs than just a plain hole.
06:17
Let's keep our major diameter of a quarter of an inch and our depth of an inch.
06:24
And then rather than entering in exact TPI and then rather than entering in an exact pitch, if I select standard thread, I can select from a long list of predefined thread sizes in FeatureCAM.
06:39
This helps us eliminate any error on our end by selecting a standardized hole size.
06:45
For this, let's just go with this 1/4-20 hole.
06:48
We can see that my diameter section has been locked to a quarter inch and my pitch section has been locked to 20.
06:55
Now all I can control is my thread depth and hole depth and chamfer.
07:00
Let's keep a thread depth of three quarters of an inch and a hole depth of one inch.
07:06
With that, I'll hit "Apply", "Ok", and run another 3D simulation.
07:23
As you may have noticed, we added that entire tap cycle and we went around spot drilled each of the four holes, then drilled each of the four holes, and finally tapped each of the four holes.
07:34
With both of our features revised and modified, and the simulations checked off, let's make one last change to the machining of this part before we send our NC Code to the machine.
07:45
I’ll eject this simulation and the last thing I want to do is you may have noticed we didn't add a facing operation at the beginning of this part.
07:54
Right now, if I open up my results fly-out and look at our operation list, we'll see that we rough our pocket and finish it before chamfering.
08:04
We spot drill our holes, drill our holes, and then tap our holes, but at no point did we clean off the top face of this part.
08:11
So right now, let's add a facing operation to this part before we post our NC Code.
08:17
I'll open up the new feature wizard, simply select Face from Dimensions, "Next", let's just locate this face feature as Z equals zero to clean up any excess material on this part.
08:31
By default, FeatureCAM has entered in a facing thickness of 0.02.
08:36
If I had located it below the face of my stock, it would have calculated that thickness.
08:41
In this case, let's just enter in a thickness of 0.02 since we don't know how much extra material we may have on this part.
08:48
Well, you notice on our strategies page, by default, we're just going to create a finish pass with our face operation.
08:55
That's fine.
08:56
And with our final operation confirmed, we'll press "Finish", "OK".
09:02
And notice that the face operation in the operations list has been placed at the very beginning of the machining of this part.
09:09
This is a good example of FeatureCAM’s built-in intelligence and automation.
09:14
FeatureCAM knows that generally when you're machining with a face operation, you want that located at the very beginning of your program, and has made the change necessary.
09:23
With both of our features modified, our face feature created, we're ready to run a final simulation.
09:44
Looks good.
09:45
We successfully worked through the simulate and revise section of our workflow.
09:50
The idea here is that we simulate our toolpath not only to generate NC Code, but to make sure we like how our part's being machined, make any revisions necessary, and then simulate those revisions over and over again until we have a final part that we're ready to post NC Code and send to our machine.
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.