Any referenced datasets can be downloaded from "Module downloads" in the module overview.
Transcript
00:09
Now that we've created the features necessary to rough and finish this part, it's time to simulate our toolpath that we just created and make any necessary revisions.
00:18
Let's start by running a centerline simulation.
00:29
Now that we have a good look at the wire diagram of the toolpath we've generated, I'm going to open up the Results window, go to the Operations List, and I want to take a look specifically at the finishing steep and shallow operation.
00:42
Remember, the steep and shallow finishing strategy allows us to use a different milling strategy
00:48
on shallow surfaces from what we're using on steep surfaces.
00:52
By zooming on this top part, we can see the division here.
00:56
On the shallow surface, I'm doing a 3D spiral surface milling strategy.
01:01
Then we can see as we transition into the steeper surface, there's a 20 thousandths overlap before I move on to a Z level finishing strategy.
01:11
This gives us a pretty good representation of what the toolpath we just created looks like.
01:15
But let's run a 3D simulation to see what our physical results are like.
01:24
Without making any revisions, it looks like we actually created some pretty successful toolpaths.
01:31
This part is a great example of the power of steep and shallow finishing in combination with Z level roughing.
01:37
If we wanted to, we could send this NC Code to our machine right now, but let's dig a little bit deeper into how these parts are machined.
01:46
To start, let's take a deeper look at our Z level roughing operation.
01:51
I’ll eject this simulation, uncheck surface milling 2, and run another 3D simulation so that we're just looking at our results from the Z level roughing operation.
02:03
We can see that our Z level roughing operation removes a fair amount of material in roughly 1 hour and 22 minutes.
02:13
However, let's say, we want to remove more material with our Z level roughing operation.
02:18
This will ensure that we're not removing too much material with our finishing operation, hopefully resulting in the best surface finish that we can get.
02:27
So, to remove more material with the Z level operation, let's eject the simulation, open up the surface milling 1 feature, navigate to the Z level roughing operation, milling tab, and let's indicate a new stepdown or Z increment value of a quarter of an inch.
02:46
I'll set that value, apply it to the feature and run another 3D simulation.
02:58
Now just by changing that stepdown, we can already visually see we've removed a lot more material with our Z level roughing operation.
03:06
However, let's go to the Details tab and see what our machining time looks like.
03:12
We've added just over an hour to our final machining time just by cutting our stepdown in half.
03:18
So, while we were able to remove more material than our original Z level roughing operation, we almost doubled the time.
03:27
In situations like this, I like to utilize an option in FeatureCAM called Step Cutting.
03:33
To find step cutting, we’ll eject the simulation, open the feature back up, navigate to the Z level operation, and on the Strategy tab, click re-machining.
03:45
Two options down, you'll see the option we're looking for, step cutting.
03:50
Step cutting allows us to stepdown a certain amount defined by our Z increment
03:56
and then step back up an indicated amount to machine away any extra material.
04:02
So, if we do a step up of a quarter of an inch, select "Okay", go back to our roughing operation, and unset our Z increment value so that we'll be stepping down a half inch.
04:15
We’ll get the exact same surface finish, hopefully with less machining time.
04:20
So "Apply", "OK".
04:23
Slow down the simulation slider a bit so we can see what's going on and press "Play".
04:46
We can see with step cutting in a Z level roughing operation, first, the tool goes down or Z increment amount, a half inch in this case, machines that entire Z level, then steps back up a quarter inch and machines away any remaining material, then back down a half inch and then back up a quarter inch and so on, until the entire model has been roughed.
05:08
So here, we can see we've gotten the same result as when we were stepping down a quarter inch each time by changing our Z increment value.
05:15
But if we go to the Details tab, we can see we're achieving the same result in an hour and a half, as opposed to 2 hours and 24 minutes.
05:25
So as we can see, Step Cutting is a great tool to get the most efficient toolpath possible in a Z level roughing operation.
05:34
So now that we've made our Z level roughing operation, as efficient as possible, let's turn back on our finishing operation, run a full 3D simulation, and let's compare our simulation results to our solid model to see if we've machined away all the material necessary to machine the solid model.
05:52
So I’ll eject this simulation, turn back on our surface milling operation.
05:58
And to compare our 3D simulation results to our solid model, we're going to use a tool in FeatureCAM called Part Compare.
06:07
As I just described, Part Compare compares our 3D simulation results to the solid model that we're trying to machine.
06:14
This way, we can have a good idea if we've missed any areas, or if we've machined into our model in any areas.
06:21
So to use Part Compare, first, we need to tell FeatureCAM what solid model would we like to compare our results to.
06:29
If I open up the solid section in the Part View, we can see the solid model that we imported, I can right click and we'll see towards the bottom an option titled Use Solid as Part Compare Target.
06:41
Once I select that, we can run a 3D simulation.
07:30
And once we have our results, we can go up to the simulation section in our Home tab, select Show and then select Part Compare.
07:41
Part Compare must be run after you've run a 3D simulation but before you've ejected your simulation results.
07:48
Once you've indicated a model that you would like to compare to, run your 3D simulation and then select Part Compare.
07:56
Any section shown in green in our Part Compare are within tolerance.
08:00
Anything shown in blue means there's extra material that needs to be machined.
08:05
And anything that would show up in red would be material that we've removed and gouged into our model.
08:11
As we can see, most of the model is actually within tolerance.
08:15
However, if you look closely in these bottom corners, it looks like there is a little bit of extra material left, indicated by the light blue color.
08:25
So it looks like while our steep and shallow finishing operation was mostly effective, it didn't quite get those corners.
08:32
So to clean this part up, let's take a look at another finishing strategy.
08:36
I’ll eject this simulation, make sure the entire model is selected.
08:42
Create new feature, surface milling feature from all of these faces, choose a single operation.
08:49
And the finishing strategy we're going to take a look at is in the specialized strategy section, Corner re-machining.
08:57
Corner re-machining will generate toolpath in any corners that were not fully machined by other finishing operations.
09:04
Exactly what we need in this case.
09:07
So select Corner re-machining, "Next", indicate how we'd like to machine these corners, we can do multiple pencil passes, move along, across or some combination to machine these corners.
09:19
And then we need to tell FeatureCAM what we've already machined.
09:23
To do this, open up the Re-machining tab and enter in a previous tool diameter for our finishing operation.
09:31
That finishing operation, again, use that default half inch ball end mill.
09:36
So for previous tool diameter, I’ll enter in a value of 0.5, make sure that Ball Nose is selected.
09:43
And we didn't have any taper on that tool.
09:46
Finally, we can indicate an overcut percentage, here it's at 5%.
09:51
We'll leave that default value, press "OK", "Next".
09:56
Leave the remaining default values.
09:60
Select "Finish", "OK".
10:03
And let's first run a centerline simulation of this new feature.
10:12
If we select just that corner re-machining finishing pass here in the operations list, we can see that we've generated toolpath only in the areas that a half inch ball end mill could not get to.
10:23
So with that, if we run a final 3D simulation, and show our Part Compare, we can see that we have now machined this entire model within tolerance.
10:45
Now that we have both accurate and efficient toolpath to machine this entire model, we're ready to save our NC Code and send it to our machine.
10:54
As a review, we took a look at a few different things in the Simulate and Revise section of this lesson.
11:00
First, we utilized Step Cutting to make a more efficient for more accurate Z level roughing operation.
11:07
Then we used Part Compare to evaluate how our finishing operation has done in removing all of the material to machine this part.
11:15
And then we used the Corner re-machining strategy to cleanup any of the leftover material from our half inch ball end mill used in the steep and shallow finishing operation.
11:25
We covered a lot of information in the Simulate and Revise section of this lesson.
11:30
If you have any questions or unclear on anything, I strongly recommend that you go back and rework through this section of the lesson.
11:39
The material covered in this lesson will go a long way to help you understand how to get the most efficient and accurate toolpath that you can when using 3d surface milling strategies in FeatureCAM.
11:51
Once you're comfortable with all the material, run your final simulation and move on to the next section, NC code.
00:09
Now that we've created the features necessary to rough and finish this part, it's time to simulate our toolpath that we just created and make any necessary revisions.
00:18
Let's start by running a centerline simulation.
00:29
Now that we have a good look at the wire diagram of the toolpath we've generated, I'm going to open up the Results window, go to the Operations List, and I want to take a look specifically at the finishing steep and shallow operation.
00:42
Remember, the steep and shallow finishing strategy allows us to use a different milling strategy
00:48
on shallow surfaces from what we're using on steep surfaces.
00:52
By zooming on this top part, we can see the division here.
00:56
On the shallow surface, I'm doing a 3D spiral surface milling strategy.
01:01
Then we can see as we transition into the steeper surface, there's a 20 thousandths overlap before I move on to a Z level finishing strategy.
01:11
This gives us a pretty good representation of what the toolpath we just created looks like.
01:15
But let's run a 3D simulation to see what our physical results are like.
01:24
Without making any revisions, it looks like we actually created some pretty successful toolpaths.
01:31
This part is a great example of the power of steep and shallow finishing in combination with Z level roughing.
01:37
If we wanted to, we could send this NC Code to our machine right now, but let's dig a little bit deeper into how these parts are machined.
01:46
To start, let's take a deeper look at our Z level roughing operation.
01:51
I’ll eject this simulation, uncheck surface milling 2, and run another 3D simulation so that we're just looking at our results from the Z level roughing operation.
02:03
We can see that our Z level roughing operation removes a fair amount of material in roughly 1 hour and 22 minutes.
02:13
However, let's say, we want to remove more material with our Z level roughing operation.
02:18
This will ensure that we're not removing too much material with our finishing operation, hopefully resulting in the best surface finish that we can get.
02:27
So, to remove more material with the Z level operation, let's eject the simulation, open up the surface milling 1 feature, navigate to the Z level roughing operation, milling tab, and let's indicate a new stepdown or Z increment value of a quarter of an inch.
02:46
I'll set that value, apply it to the feature and run another 3D simulation.
02:58
Now just by changing that stepdown, we can already visually see we've removed a lot more material with our Z level roughing operation.
03:06
However, let's go to the Details tab and see what our machining time looks like.
03:12
We've added just over an hour to our final machining time just by cutting our stepdown in half.
03:18
So, while we were able to remove more material than our original Z level roughing operation, we almost doubled the time.
03:27
In situations like this, I like to utilize an option in FeatureCAM called Step Cutting.
03:33
To find step cutting, we’ll eject the simulation, open the feature back up, navigate to the Z level operation, and on the Strategy tab, click re-machining.
03:45
Two options down, you'll see the option we're looking for, step cutting.
03:50
Step cutting allows us to stepdown a certain amount defined by our Z increment
03:56
and then step back up an indicated amount to machine away any extra material.
04:02
So, if we do a step up of a quarter of an inch, select "Okay", go back to our roughing operation, and unset our Z increment value so that we'll be stepping down a half inch.
04:15
We’ll get the exact same surface finish, hopefully with less machining time.
04:20
So "Apply", "OK".
04:23
Slow down the simulation slider a bit so we can see what's going on and press "Play".
04:46
We can see with step cutting in a Z level roughing operation, first, the tool goes down or Z increment amount, a half inch in this case, machines that entire Z level, then steps back up a quarter inch and machines away any remaining material, then back down a half inch and then back up a quarter inch and so on, until the entire model has been roughed.
05:08
So here, we can see we've gotten the same result as when we were stepping down a quarter inch each time by changing our Z increment value.
05:15
But if we go to the Details tab, we can see we're achieving the same result in an hour and a half, as opposed to 2 hours and 24 minutes.
05:25
So as we can see, Step Cutting is a great tool to get the most efficient toolpath possible in a Z level roughing operation.
05:34
So now that we've made our Z level roughing operation, as efficient as possible, let's turn back on our finishing operation, run a full 3D simulation, and let's compare our simulation results to our solid model to see if we've machined away all the material necessary to machine the solid model.
05:52
So I’ll eject this simulation, turn back on our surface milling operation.
05:58
And to compare our 3D simulation results to our solid model, we're going to use a tool in FeatureCAM called Part Compare.
06:07
As I just described, Part Compare compares our 3D simulation results to the solid model that we're trying to machine.
06:14
This way, we can have a good idea if we've missed any areas, or if we've machined into our model in any areas.
06:21
So to use Part Compare, first, we need to tell FeatureCAM what solid model would we like to compare our results to.
06:29
If I open up the solid section in the Part View, we can see the solid model that we imported, I can right click and we'll see towards the bottom an option titled Use Solid as Part Compare Target.
06:41
Once I select that, we can run a 3D simulation.
07:30
And once we have our results, we can go up to the simulation section in our Home tab, select Show and then select Part Compare.
07:41
Part Compare must be run after you've run a 3D simulation but before you've ejected your simulation results.
07:48
Once you've indicated a model that you would like to compare to, run your 3D simulation and then select Part Compare.
07:56
Any section shown in green in our Part Compare are within tolerance.
08:00
Anything shown in blue means there's extra material that needs to be machined.
08:05
And anything that would show up in red would be material that we've removed and gouged into our model.
08:11
As we can see, most of the model is actually within tolerance.
08:15
However, if you look closely in these bottom corners, it looks like there is a little bit of extra material left, indicated by the light blue color.
08:25
So it looks like while our steep and shallow finishing operation was mostly effective, it didn't quite get those corners.
08:32
So to clean this part up, let's take a look at another finishing strategy.
08:36
I’ll eject this simulation, make sure the entire model is selected.
08:42
Create new feature, surface milling feature from all of these faces, choose a single operation.
08:49
And the finishing strategy we're going to take a look at is in the specialized strategy section, Corner re-machining.
08:57
Corner re-machining will generate toolpath in any corners that were not fully machined by other finishing operations.
09:04
Exactly what we need in this case.
09:07
So select Corner re-machining, "Next", indicate how we'd like to machine these corners, we can do multiple pencil passes, move along, across or some combination to machine these corners.
09:19
And then we need to tell FeatureCAM what we've already machined.
09:23
To do this, open up the Re-machining tab and enter in a previous tool diameter for our finishing operation.
09:31
That finishing operation, again, use that default half inch ball end mill.
09:36
So for previous tool diameter, I’ll enter in a value of 0.5, make sure that Ball Nose is selected.
09:43
And we didn't have any taper on that tool.
09:46
Finally, we can indicate an overcut percentage, here it's at 5%.
09:51
We'll leave that default value, press "OK", "Next".
09:56
Leave the remaining default values.
09:60
Select "Finish", "OK".
10:03
And let's first run a centerline simulation of this new feature.
10:12
If we select just that corner re-machining finishing pass here in the operations list, we can see that we've generated toolpath only in the areas that a half inch ball end mill could not get to.
10:23
So with that, if we run a final 3D simulation, and show our Part Compare, we can see that we have now machined this entire model within tolerance.
10:45
Now that we have both accurate and efficient toolpath to machine this entire model, we're ready to save our NC Code and send it to our machine.
10:54
As a review, we took a look at a few different things in the Simulate and Revise section of this lesson.
11:00
First, we utilized Step Cutting to make a more efficient for more accurate Z level roughing operation.
11:07
Then we used Part Compare to evaluate how our finishing operation has done in removing all of the material to machine this part.
11:15
And then we used the Corner re-machining strategy to cleanup any of the leftover material from our half inch ball end mill used in the steep and shallow finishing operation.
11:25
We covered a lot of information in the Simulate and Revise section of this lesson.
11:30
If you have any questions or unclear on anything, I strongly recommend that you go back and rework through this section of the lesson.
11:39
The material covered in this lesson will go a long way to help you understand how to get the most efficient and accurate toolpath that you can when using 3d surface milling strategies in FeatureCAM.
11:51
Once you're comfortable with all the material, run your final simulation and move on to the next section, NC code.
