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
00:09
Now that we've imported our solid model, setup our stock, handled machine preparation, and programmed all of our features using FeatureCAM's feature recognition, it's time to simulate our features and make any necessary revisions.
00:23
Let's start by running a centerline simulation.
00:29
As a review, you'll remember that centerline simulations show us a wire diagram of the toolpaths generated to machine this part.
00:37
Any line shown in black is a feed move and any line shown in green is a rapid move.
00:44
The centerline looks good, so let's run a 3D simulation as well.
00:53
Remember, 3D simulations not only show us a good visual representation of what the machining of our part will look like, but it also allows us to check, if at any point, we will be colliding or gouging into our stock or solid model.
01:08
It looks like our program is gouge free, and the final product seems to pass the eye test.
01:13
It looks just like our solid model.
01:15
But let's take a little bit deeper and make a few revisions to how this part is machined as opposed to what is finally machined.
01:24
We'll exit the simulation and let's start by opening up the boss1 feature properties.
01:31
We've seen this window a few times, but I want to give you a quick tour of a Feature Properties window.
01:36
First, we'll notice a few tabs that apply to the feature globally.
01:40
We can change the dimensions of the entire feature, the location, strategy, and any miscellaneous attributes.
01:48
Next, on the left side, we can see it's broken down into the roughing and the finishing operation.
01:55
As I select the roughing operation, you can see my tabs change.
01:58
Here I can step through the tabs and change specific details about the roughing operation itself.
02:05
For this exercise, I'd like to go to the Milling tab to take a look at some of the milling attributes.
02:12
These milling attributes help us really fine tune exactly how this part is machined.
02:16
And first, we'll be looking at the attribute called finish allowance.
02:21
This is a common milling attribute that you should be aware of.
02:24
By default, FeatureCAM leaves 50 thousandths after a roughing operation to be cleaned up by the finishing operation.
02:31
For some, 50 thousandths may be too much to be cleaning up with your finishing operation.
02:37
For others, you may want even more material allowance.
02:40
In our case, I'd like to change it to 10 thousandths as opposed to 50 thousandths.
02:45
So we're leaving less material after our roughing operation.
02:49
To do that, I'll select Finish Allowance, go into the New Value window, type in 0.01, set that value as the finish allowance value and "Apply" that to the feature.
03:03
Now my roughing operation leaves less material after it's done with the boss feature.
03:10
This would be a good point to open up the Help file that we mentioned earlier.
03:15
Read through the help file of the milling attributes page and read about the various attributes associated with each feature.
03:22
Programming features in FeatureCAM is very quick and automated process, but taking the time to dig deeper into a features milling attributes can save you a lot of time in the long run as well, and make sure that the program that you're posting and sending to your machine is exactly what you want.
03:39
Let's go ahead and make this exact same finish allowance change to the remaining pocket and side features.
04:04
With that, we can run simulation.
04:08
And we'll notice that while our final product looks the same, how it was machined is a little bit different.
04:16
Next, let's open up the results fly-out and take a look at some of the tools being used to machine our part in the Operations List.
04:24
Again, in our Operations List, we can see each individual operation, what feature that operation is associated with, the tool being used, the feed, the speed, and the depth of that feature.
04:38
For example, our first operation is face 1, it uses a face mill.
04:43
It has a feed of 130 inches per minute, a speed of 5,821 RPMs, and a depth of 0.025 inches.
04:55
Moving along, we can see that our boss, pocket, and two of our side features are milled using an inch end mill.
05:03
For this example, let's say we don't have a 1 inch end mill.
05:07
If I look through this program, we may notice that at one point, we do use a 0.5 inch end mill.
05:12
Let's say, I do have one of those and I need to make sure that these features are cut using that 0.5 inch end mill as opposed to the 1 inch end mill.
05:20
Starting with boss1, I can either double click on boss1 in the operations list or over on the left in the Part View.
05:27
Once I have the boss properties open, I'll go to the roughing operation, tools, and I'll narrow things down by typing in a diameter of 0.5.
05:38
If I select this recent tools checkbox, it's just going to show me the other tools used in this program.
05:44
Here's that 0.5 inch end mill, I'll select it, "Apply" it.
05:49
And notice that in the operations list, it's made that change for the rough pass and even the finish pass for this boss feature.
05:57
If I didn't wanted to make that change for the finish as well, I could simply go into the finish and override to a different tool.
06:06
Go ahead and make the same change for all of the other features using the 1 inch end mill.
06:18
With a few of our tools changed, next, let's look at the feeds and speeds being used for each operation.
06:25
I'll open up this boss1 feature again, go to the roughing operation and navigate to the feeds and speeds tab, F/S.
06:35
Here we can see the default feeds and speeds that FeatureCAM has calculated based on both this feature
06:41
and the fact that it knows that we're milling from aluminum.
06:45
It looks like FeatureCAM is recommending a speed of almost 5,000 RPMs and a feed of almost 50 inches per minute.
06:53
Just for this example, let's say, I only want to go 4,000 RPMs.
06:57
I'll type in that value, select Override and hit "Apply".
07:02
We'll see that it's made that change in the Operations List, and it's also recommended and calculated a new feed based on the speed that I just entered.
07:11
I strongly recommend that whenever you're programming a part, you take a final look at the feeds and speeds before you post your code and send it to the machine.
07:21
One thing I want you to notice that as I went and updated the feeds and speeds for that feature, an asterisk appeared next to the speed in the Operations List.
07:31
You'll see that same asterisk appeared next to the features where I did an override for the tools.
07:37
This asterisk means that there has been an override placed on the tool or the feed or the speed of this operation.
07:44
I personally like to use this as a checklist for a final ok before I generate NC code.
07:51
So I'll open up a feature, I'll go to the feeds and speeds tab, and if I like that speed and that feed, I'll just select Override, "Apply" and the asterisk appears next to those feeds and speeds in my Operations List.
08:06
This isn't necessary, but this is just the workflow that I like to use when programming parts and sending them to the machine in the real world.
08:14
So feel free to work through, look at every tool being used for each operation, and give a final check off on the feeds and speeds being used for operation before moving on to the next revision.
08:27
With our finished allowance altered, a couple of our tools changed, and our feeds and speeds checked off, let's take a look at a final couple milling attributes for the machining of this part.
08:38
At this point, while we have made several revisions as you may have expected, our simulation results were virtually unchanged.
08:45
But this is to be expected, as all the changes we made were directed towards how we machined the part as opposed to what we machined.
08:54
While our simulation looks largely unchanged, our NC Code is certainly very different.
08:59
Continuing along these lines, let's take a look at two additional milling attributes, stepdown and stepover.
09:06
To do this, I'm going to open up the pocket1 feature, go to the roughing operation, and navigate to the Milling tab.
09:14
Again, this is where I can find a lot of the common milling attributes associated with a features roughing or finishing operation.
09:22
Just like with our feeds and speeds, we'll notice that there is an asterisk out to the left of our finish allowance indicating that we have done an override from the default value, and I'd like to show you down to the Rough Pass Z increment parameter.
09:37
Notice that as I hover over these attributes, a little help window pops up, gives me a quick description of what rough pass Z increment is, as well as a little diagram.
09:48
Note that I could also find this information by selecting Help in the bottom part of this window.
09:53
So as I look at this, it's telling me that Rough Pass Z increment is the distance that the tool moves down in the Z axis with each pass.
10:02
So before I change this, I want to preview just this feature.
10:06
So I'll select Preview and I'll play a wire diagram of this toolpath.
10:10
And we’ll notice that I just go down to the bottom of the pocket and machine outward.
10:15
I'll eject this preview, and let's change this rough pass Z increment to a smaller value.
10:21
I'll change it to 0.01, "Set" and "Apply".
10:26
Now as I preview, take a look at the toolpath.
10:30
This part now takes a lot more stepdowns to machine this pocket.
10:34
Now, 0.01 might be overkill, but it does a good job of showing what this parameter does.
10:39
Likewise, I'm going to take a top view and take a look at the stepover.
10:44
If I eject this preview, go to the Stepover tab and change the distance between cuts to 0.01, apply that to the feature.
10:55
Now let's preview the toolpath.
10:59
As you may have expected, the stepover between each pass in our toolpath is much, much closer now.
11:06
This is obviously because we've changed the distance between cuts as we step outward when machining this pocket.
11:14
So just by changing these two attributes, we've drastically changed how this part is machined.
11:19
We were able to greatly increase the toolpath density in both the XY plane and the Z direction.
11:26
Now, feel free to experiment with any of the remaining attributes until you're happy with your final results.
11:32
When you're adjusting your toolpath, just remember that feeds and speeds, stepover and stepdown are all related to one another.
11:40
As you alter one of these attributes, you're going to want to consider altering the others.
11:44
For example, if you're taking a really heavy cut, the same feeds and speeds are not going to work for when you are taking a 0.01 inch stepover cut.
11:53
Feel free to mess around with any of these attributes, but the purpose of this exercise is to simply locate and explain these main three attributes.
12:02
After making any desired revisions, run a final simulation and move on to the next section, NC Code.
Video transcript
00:09
Now that we've imported our solid model, setup our stock, handled machine preparation, and programmed all of our features using FeatureCAM's feature recognition, it's time to simulate our features and make any necessary revisions.
00:23
Let's start by running a centerline simulation.
00:29
As a review, you'll remember that centerline simulations show us a wire diagram of the toolpaths generated to machine this part.
00:37
Any line shown in black is a feed move and any line shown in green is a rapid move.
00:44
The centerline looks good, so let's run a 3D simulation as well.
00:53
Remember, 3D simulations not only show us a good visual representation of what the machining of our part will look like, but it also allows us to check, if at any point, we will be colliding or gouging into our stock or solid model.
01:08
It looks like our program is gouge free, and the final product seems to pass the eye test.
01:13
It looks just like our solid model.
01:15
But let's take a little bit deeper and make a few revisions to how this part is machined as opposed to what is finally machined.
01:24
We'll exit the simulation and let's start by opening up the boss1 feature properties.
01:31
We've seen this window a few times, but I want to give you a quick tour of a Feature Properties window.
01:36
First, we'll notice a few tabs that apply to the feature globally.
01:40
We can change the dimensions of the entire feature, the location, strategy, and any miscellaneous attributes.
01:48
Next, on the left side, we can see it's broken down into the roughing and the finishing operation.
01:55
As I select the roughing operation, you can see my tabs change.
01:58
Here I can step through the tabs and change specific details about the roughing operation itself.
02:05
For this exercise, I'd like to go to the Milling tab to take a look at some of the milling attributes.
02:12
These milling attributes help us really fine tune exactly how this part is machined.
02:16
And first, we'll be looking at the attribute called finish allowance.
02:21
This is a common milling attribute that you should be aware of.
02:24
By default, FeatureCAM leaves 50 thousandths after a roughing operation to be cleaned up by the finishing operation.
02:31
For some, 50 thousandths may be too much to be cleaning up with your finishing operation.
02:37
For others, you may want even more material allowance.
02:40
In our case, I'd like to change it to 10 thousandths as opposed to 50 thousandths.
02:45
So we're leaving less material after our roughing operation.
02:49
To do that, I'll select Finish Allowance, go into the New Value window, type in 0.01, set that value as the finish allowance value and "Apply" that to the feature.
03:03
Now my roughing operation leaves less material after it's done with the boss feature.
03:10
This would be a good point to open up the Help file that we mentioned earlier.
03:15
Read through the help file of the milling attributes page and read about the various attributes associated with each feature.
03:22
Programming features in FeatureCAM is very quick and automated process, but taking the time to dig deeper into a features milling attributes can save you a lot of time in the long run as well, and make sure that the program that you're posting and sending to your machine is exactly what you want.
03:39
Let's go ahead and make this exact same finish allowance change to the remaining pocket and side features.
04:04
With that, we can run simulation.
04:08
And we'll notice that while our final product looks the same, how it was machined is a little bit different.
04:16
Next, let's open up the results fly-out and take a look at some of the tools being used to machine our part in the Operations List.
04:24
Again, in our Operations List, we can see each individual operation, what feature that operation is associated with, the tool being used, the feed, the speed, and the depth of that feature.
04:38
For example, our first operation is face 1, it uses a face mill.
04:43
It has a feed of 130 inches per minute, a speed of 5,821 RPMs, and a depth of 0.025 inches.
04:55
Moving along, we can see that our boss, pocket, and two of our side features are milled using an inch end mill.
05:03
For this example, let's say we don't have a 1 inch end mill.
05:07
If I look through this program, we may notice that at one point, we do use a 0.5 inch end mill.
05:12
Let's say, I do have one of those and I need to make sure that these features are cut using that 0.5 inch end mill as opposed to the 1 inch end mill.
05:20
Starting with boss1, I can either double click on boss1 in the operations list or over on the left in the Part View.
05:27
Once I have the boss properties open, I'll go to the roughing operation, tools, and I'll narrow things down by typing in a diameter of 0.5.
05:38
If I select this recent tools checkbox, it's just going to show me the other tools used in this program.
05:44
Here's that 0.5 inch end mill, I'll select it, "Apply" it.
05:49
And notice that in the operations list, it's made that change for the rough pass and even the finish pass for this boss feature.
05:57
If I didn't wanted to make that change for the finish as well, I could simply go into the finish and override to a different tool.
06:06
Go ahead and make the same change for all of the other features using the 1 inch end mill.
06:18
With a few of our tools changed, next, let's look at the feeds and speeds being used for each operation.
06:25
I'll open up this boss1 feature again, go to the roughing operation and navigate to the feeds and speeds tab, F/S.
06:35
Here we can see the default feeds and speeds that FeatureCAM has calculated based on both this feature
06:41
and the fact that it knows that we're milling from aluminum.
06:45
It looks like FeatureCAM is recommending a speed of almost 5,000 RPMs and a feed of almost 50 inches per minute.
06:53
Just for this example, let's say, I only want to go 4,000 RPMs.
06:57
I'll type in that value, select Override and hit "Apply".
07:02
We'll see that it's made that change in the Operations List, and it's also recommended and calculated a new feed based on the speed that I just entered.
07:11
I strongly recommend that whenever you're programming a part, you take a final look at the feeds and speeds before you post your code and send it to the machine.
07:21
One thing I want you to notice that as I went and updated the feeds and speeds for that feature, an asterisk appeared next to the speed in the Operations List.
07:31
You'll see that same asterisk appeared next to the features where I did an override for the tools.
07:37
This asterisk means that there has been an override placed on the tool or the feed or the speed of this operation.
07:44
I personally like to use this as a checklist for a final ok before I generate NC code.
07:51
So I'll open up a feature, I'll go to the feeds and speeds tab, and if I like that speed and that feed, I'll just select Override, "Apply" and the asterisk appears next to those feeds and speeds in my Operations List.
08:06
This isn't necessary, but this is just the workflow that I like to use when programming parts and sending them to the machine in the real world.
08:14
So feel free to work through, look at every tool being used for each operation, and give a final check off on the feeds and speeds being used for operation before moving on to the next revision.
08:27
With our finished allowance altered, a couple of our tools changed, and our feeds and speeds checked off, let's take a look at a final couple milling attributes for the machining of this part.
08:38
At this point, while we have made several revisions as you may have expected, our simulation results were virtually unchanged.
08:45
But this is to be expected, as all the changes we made were directed towards how we machined the part as opposed to what we machined.
08:54
While our simulation looks largely unchanged, our NC Code is certainly very different.
08:59
Continuing along these lines, let's take a look at two additional milling attributes, stepdown and stepover.
09:06
To do this, I'm going to open up the pocket1 feature, go to the roughing operation, and navigate to the Milling tab.
09:14
Again, this is where I can find a lot of the common milling attributes associated with a features roughing or finishing operation.
09:22
Just like with our feeds and speeds, we'll notice that there is an asterisk out to the left of our finish allowance indicating that we have done an override from the default value, and I'd like to show you down to the Rough Pass Z increment parameter.
09:37
Notice that as I hover over these attributes, a little help window pops up, gives me a quick description of what rough pass Z increment is, as well as a little diagram.
09:48
Note that I could also find this information by selecting Help in the bottom part of this window.
09:53
So as I look at this, it's telling me that Rough Pass Z increment is the distance that the tool moves down in the Z axis with each pass.
10:02
So before I change this, I want to preview just this feature.
10:06
So I'll select Preview and I'll play a wire diagram of this toolpath.
10:10
And we’ll notice that I just go down to the bottom of the pocket and machine outward.
10:15
I'll eject this preview, and let's change this rough pass Z increment to a smaller value.
10:21
I'll change it to 0.01, "Set" and "Apply".
10:26
Now as I preview, take a look at the toolpath.
10:30
This part now takes a lot more stepdowns to machine this pocket.
10:34
Now, 0.01 might be overkill, but it does a good job of showing what this parameter does.
10:39
Likewise, I'm going to take a top view and take a look at the stepover.
10:44
If I eject this preview, go to the Stepover tab and change the distance between cuts to 0.01, apply that to the feature.
10:55
Now let's preview the toolpath.
10:59
As you may have expected, the stepover between each pass in our toolpath is much, much closer now.
11:06
This is obviously because we've changed the distance between cuts as we step outward when machining this pocket.
11:14
So just by changing these two attributes, we've drastically changed how this part is machined.
11:19
We were able to greatly increase the toolpath density in both the XY plane and the Z direction.
11:26
Now, feel free to experiment with any of the remaining attributes until you're happy with your final results.
11:32
When you're adjusting your toolpath, just remember that feeds and speeds, stepover and stepdown are all related to one another.
11:40
As you alter one of these attributes, you're going to want to consider altering the others.
11:44
For example, if you're taking a really heavy cut, the same feeds and speeds are not going to work for when you are taking a 0.01 inch stepover cut.
11:53
Feel free to mess around with any of these attributes, but the purpose of this exercise is to simply locate and explain these main three attributes.
12:02
After making any desired revisions, run a final simulation and move on to the next section, NC Code.
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.