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
00:02
In this video, will finish mill and drill apart.
00:06
After completing this step,
00:07
you'll be able to create a 2D contour toolpath, create a spot drilling operation, a chip breaking operation and a bore toolpath.
00:16
In fusion 360, we want to carry on with our gear housing for CNC mill.
00:21
At this point we need to talk about the order of operations and considering tool changes.
00:27
For example, we have tool number six which is a half inch flat end mill, then we go to our face mill, then back to a half inch end mill.
00:35
We want to avoid these tool changes. So what we're going to do is we're going to reorder these by dragging them into a certain order.
00:42
Keeping in mind that our face mill operation took into account the original outside profile.
00:49
So I want to come into my face mail operation.
00:52
I'm going to go to my geometry and I'm going to turn off that chain selection and instead use this contour.
00:59
That stock contour, allowing a machine that area and then our 2D adaptive can remove material from the outside,
01:05
and our 2D pocket can start to take away some material all with that half inch end mill.
01:11
Let's double check our 2D pocket settings and make sure that we're not leaving any stock behind and we are using that as a final finishing pass.
01:21
Now we need to account for drilling the outside holes.
01:24
We need to machine the outside of the part and then we also need to machine all these different bores.
01:30
So it's a good time for us to use inspect and take a look at some of these different areas,
01:35
such as the radius value of this Philip notice that the radius is 0.197 or a diameter of 0.394,
01:43
which means a half inch end mill is too large to machine end that tells me that I need to finish this off with a quarter inch end mill or larger.
01:51
Something that fits that size but is a little bit undersized to give us a good surface finish,
01:57
because I know we haven't created a three, its end mill and our tool library, we're going to be using a quarter inch to finish it off.
02:03
Let's also take a look at the smaller bores and see what sizes were working with.
02:08
We have a diameter of .315 and for this one here we have a diameter of .413.
02:15
So this tells me that I can likely get in there with a quarter in general even though it's going to be tight.
02:21
So the next step is to consider which tool we want to use next, these holes on the outside, we don't have a drill bit that's 0.236.
02:30
This is likely a metric size. And if we change our secondary units to millimeters, you can see that it comes out at a six millimeter hole.
02:39
Well, what we need to do is we need to drill with what we have,
02:42
and then we can take another enamel such as an eighth inch enamel and finish off the size of those holes.
02:48
So the first thing that I'm going to consider is spot drilling those holes.
02:51
Since I know that I'm going to have to come back with an end mill to finish them off.
02:55
So I'm going to select my spot drill.
02:59
I'm going to go into my cam DFM library and select spot drill and I'm going to use it for aluminum drilling.
03:07
I'm going to manually select the holes.
03:09
I'm going to go around and select each of these and then for my heights, I'm going to be using the top of whole and then drill tip through bottom.
03:21
We're going to say okay.
03:22
And that allows me to spot drill those positions even though we're going to be using an end mill.
03:27
It's not really needed that we spot drill but we have to be careful that we have a tool that can actually cut that geometry.
03:33
If you're using a small end mill that isn't center cutting, then it's going to be problematic. Taking it into that area.
03:40
Now that we have this rapid operation. I know that I have a .201 drill.
03:45
So I'm going to duplicate this,
03:48
and then I'm going to modify the duplicate and I'm going to drill those holes using that 0.201 or number seven drill.
03:57
Again, it's not the right size but it gets us pretty close.
04:00
I'm going to reverse the order and I'm going to change the cycle to a partial retract.
04:06
I also want to make sure that I go to the heights and then I use the whole bottom and I allow the drill tip to go through and say, okay.
04:15
Now we've drilled all the way through, allows us to just poke through the other side of the stock.
04:19
Keeping in mind we've already faced the other side.
04:22
Now that these are close, I know when I come back with an 8th inch end mill,
04:26
I can finish those holes off and I'm only removing a small amount of material.
04:32
Another thing that we could consider is using that same drill to pre drill all these other locations.
04:38
I'm not going to be doing that because I'm going to be using a 2D pocket,
04:42
but just keep in mind that we do have options and it might be a good idea for us to do something like that.
04:47
I'm going to create a 2D pocket using my quarter inch flat. And this is going to be tool number five.
04:54
I'm going to use it for aluminum roughing in this operation and then I want to select my geometry.
04:60
I'm going to allow it to machine that pocket as well as these pockets.
05:05
These are going to be press fit for bearings.
05:07
So I need to be careful and I need to do a final operation to bore them to the right size.
05:13
Because of this, I'm going to make sure that I'm leaving a small amount of material in the radial direction.
05:19
But I am going to take the axial material down to zero.
05:23
I'm not going to make any other adjustments to the toolpath.
05:26
I just want to take a look and see what geometry is cut,
05:30
noticing that it's going down all the way to the final death and doing this in one pass.
05:35
Depending on the material and the specifications, that might be okay, but it is something you need to be aware of.
05:41
Now that I have removed the majority of the material from those areas. I need to go back and finish off those insides, the outsides and these holes.
05:49
So there's still a lot that we need to do. And let's go ahead and let's explore ways in which we can finish them off.
05:56
We're still going to be using the quarter in gen mill and now I'm going to take a look at a 2D bore.
06:01
Going to use that quarter inch flat and for the geometry, we need a circular faced selection.
06:07
We're going to use this as our option. We're going to do the same thing for each of these other areas.
06:13
In the past this section, we need to make sure that we're not leaving any stock and I'm going to say, okay.
06:19
So it's going to go through and do my final cut on the boards of those areas.
06:23
And then I need to make sure that I machine out the insides.
06:27
This is going to be passing for a shaft. It's not going to have a tight fit or tight tolerance.
06:32
So I'm going to go back in with a 2D contour,
06:35
and I'm going to use that same quarter inch end mill and I'm gonna machine all the way down to that on each of these.
06:44
When I'm using the 2D contour again, I need to make sure that I'm not leaving stock.
06:48
I need to consider if I need to do multiple depths, but in this instance I'm actually going to use a ramp option.
06:55
The ramp option will follow the selected contour and it will just work its way down.
06:59
So I'm going to say, okay and take a look at the results.
07:03
Everything looks pretty good here. However, we are spending a lot of time with this helical entry well above the part.
07:10
So we need to consider how much time we're spending and if that makes sense, notice that the lead out has dropped based on linking constraints.
07:19
And that's simply because the tool is too large, in order to completely lead out based on the default parameters,
07:28
I'm going to make one adjustment to the 2D contour and that's in the heights section.
07:33
The feed height where it starts to create that feed operation, right now, is based on the top and the top height is based on the stock.
07:41
What I'm going to do is change this to a selection since I know I have machine down to at least this face,
07:46
I'm going to set that The top height is now based on that selection and then the feed height is based on .1,
07:54
where we have to be careful with this is in the fact that it's trying to jump over geometry.
08:00
Now it's telling me that the ramp clearance and the vertical lead in radius is higher than the feed height,
08:05
and it says that we should consider reducing the ramp clearance value and raise those to match.
08:12
We're going to say okay and we want to make sure that these clearance heights, these ramp heights where it's wrapping up to are going to be fine.
08:20
Everything looks pretty good from there. I'm happy with those results.
08:23
I still have a warning about my lead ins and lead out, but at this point I think the toolpaths look pretty good.
08:29
We still need to finish the outside in which we're going to use that quarter inch 10 mil.
08:33
So once again we'll create a 2D contour, quarter inch flat around the outside of the park,
08:40
we're not going to be leaving any stock and depending on our requirements,
08:45
we can determine whether or not we want to repeat the finish pass,
08:48
whether or not we want to have a roughing pass and if we want to use that ramp option again.
08:55
Now, in the case of this toolpath, I want to allow it to do a roughing pass and the roughing pass is going to be a very small amount.
09:03
I'm going to use .05 and we're going to do one roughing pass and one finish pass.
09:09
So this is going to allow it to do that roughing pass. And then it's going to step in that .05 to do it's finished pass.
09:15
Now remember that roughing pass is supposed to remove a bit of material, so maybe we can take that in a little bit more 2.025.
09:25
That will remove some material and then they'll allow us to do a final finish cut on the last bit.
09:31
Keeping in mind that we are seeing some stock here. But again we have stock left from the other side that we know it's going to be removed.
09:38
The last thing that we need to do is we need to finish the final diameter of these holes.
09:44
If they are critical, then we want to use something like a bore toolpath.
09:51
I'm going to go in with an 8th in flat end mill on aluminum finishing and I'm going to select the inside bore of each hole.
10:00
While this isn't strictly required. We could do a
10:03
This is a good way for us to come in and make sure that we're not engaging too much material with that tool.
10:10
Everything looks pretty good, and it's always a good idea for us to save often.
10:13
So at this point, let's make sure that we do save the design before we move on to the next step.
Video transcript
00:02
In this video, will finish mill and drill apart.
00:06
After completing this step,
00:07
you'll be able to create a 2D contour toolpath, create a spot drilling operation, a chip breaking operation and a bore toolpath.
00:16
In fusion 360, we want to carry on with our gear housing for CNC mill.
00:21
At this point we need to talk about the order of operations and considering tool changes.
00:27
For example, we have tool number six which is a half inch flat end mill, then we go to our face mill, then back to a half inch end mill.
00:35
We want to avoid these tool changes. So what we're going to do is we're going to reorder these by dragging them into a certain order.
00:42
Keeping in mind that our face mill operation took into account the original outside profile.
00:49
So I want to come into my face mail operation.
00:52
I'm going to go to my geometry and I'm going to turn off that chain selection and instead use this contour.
00:59
That stock contour, allowing a machine that area and then our 2D adaptive can remove material from the outside,
01:05
and our 2D pocket can start to take away some material all with that half inch end mill.
01:11
Let's double check our 2D pocket settings and make sure that we're not leaving any stock behind and we are using that as a final finishing pass.
01:21
Now we need to account for drilling the outside holes.
01:24
We need to machine the outside of the part and then we also need to machine all these different bores.
01:30
So it's a good time for us to use inspect and take a look at some of these different areas,
01:35
such as the radius value of this Philip notice that the radius is 0.197 or a diameter of 0.394,
01:43
which means a half inch end mill is too large to machine end that tells me that I need to finish this off with a quarter inch end mill or larger.
01:51
Something that fits that size but is a little bit undersized to give us a good surface finish,
01:57
because I know we haven't created a three, its end mill and our tool library, we're going to be using a quarter inch to finish it off.
02:03
Let's also take a look at the smaller bores and see what sizes were working with.
02:08
We have a diameter of .315 and for this one here we have a diameter of .413.
02:15
So this tells me that I can likely get in there with a quarter in general even though it's going to be tight.
02:21
So the next step is to consider which tool we want to use next, these holes on the outside, we don't have a drill bit that's 0.236.
02:30
This is likely a metric size. And if we change our secondary units to millimeters, you can see that it comes out at a six millimeter hole.
02:39
Well, what we need to do is we need to drill with what we have,
02:42
and then we can take another enamel such as an eighth inch enamel and finish off the size of those holes.
02:48
So the first thing that I'm going to consider is spot drilling those holes.
02:51
Since I know that I'm going to have to come back with an end mill to finish them off.
02:55
So I'm going to select my spot drill.
02:59
I'm going to go into my cam DFM library and select spot drill and I'm going to use it for aluminum drilling.
03:07
I'm going to manually select the holes.
03:09
I'm going to go around and select each of these and then for my heights, I'm going to be using the top of whole and then drill tip through bottom.
03:21
We're going to say okay.
03:22
And that allows me to spot drill those positions even though we're going to be using an end mill.
03:27
It's not really needed that we spot drill but we have to be careful that we have a tool that can actually cut that geometry.
03:33
If you're using a small end mill that isn't center cutting, then it's going to be problematic. Taking it into that area.
03:40
Now that we have this rapid operation. I know that I have a .201 drill.
03:45
So I'm going to duplicate this,
03:48
and then I'm going to modify the duplicate and I'm going to drill those holes using that 0.201 or number seven drill.
03:57
Again, it's not the right size but it gets us pretty close.
04:00
I'm going to reverse the order and I'm going to change the cycle to a partial retract.
04:06
I also want to make sure that I go to the heights and then I use the whole bottom and I allow the drill tip to go through and say, okay.
04:15
Now we've drilled all the way through, allows us to just poke through the other side of the stock.
04:19
Keeping in mind we've already faced the other side.
04:22
Now that these are close, I know when I come back with an 8th inch end mill,
04:26
I can finish those holes off and I'm only removing a small amount of material.
04:32
Another thing that we could consider is using that same drill to pre drill all these other locations.
04:38
I'm not going to be doing that because I'm going to be using a 2D pocket,
04:42
but just keep in mind that we do have options and it might be a good idea for us to do something like that.
04:47
I'm going to create a 2D pocket using my quarter inch flat. And this is going to be tool number five.
04:54
I'm going to use it for aluminum roughing in this operation and then I want to select my geometry.
04:60
I'm going to allow it to machine that pocket as well as these pockets.
05:05
These are going to be press fit for bearings.
05:07
So I need to be careful and I need to do a final operation to bore them to the right size.
05:13
Because of this, I'm going to make sure that I'm leaving a small amount of material in the radial direction.
05:19
But I am going to take the axial material down to zero.
05:23
I'm not going to make any other adjustments to the toolpath.
05:26
I just want to take a look and see what geometry is cut,
05:30
noticing that it's going down all the way to the final death and doing this in one pass.
05:35
Depending on the material and the specifications, that might be okay, but it is something you need to be aware of.
05:41
Now that I have removed the majority of the material from those areas. I need to go back and finish off those insides, the outsides and these holes.
05:49
So there's still a lot that we need to do. And let's go ahead and let's explore ways in which we can finish them off.
05:56
We're still going to be using the quarter in gen mill and now I'm going to take a look at a 2D bore.
06:01
Going to use that quarter inch flat and for the geometry, we need a circular faced selection.
06:07
We're going to use this as our option. We're going to do the same thing for each of these other areas.
06:13
In the past this section, we need to make sure that we're not leaving any stock and I'm going to say, okay.
06:19
So it's going to go through and do my final cut on the boards of those areas.
06:23
And then I need to make sure that I machine out the insides.
06:27
This is going to be passing for a shaft. It's not going to have a tight fit or tight tolerance.
06:32
So I'm going to go back in with a 2D contour,
06:35
and I'm going to use that same quarter inch end mill and I'm gonna machine all the way down to that on each of these.
06:44
When I'm using the 2D contour again, I need to make sure that I'm not leaving stock.
06:48
I need to consider if I need to do multiple depths, but in this instance I'm actually going to use a ramp option.
06:55
The ramp option will follow the selected contour and it will just work its way down.
06:59
So I'm going to say, okay and take a look at the results.
07:03
Everything looks pretty good here. However, we are spending a lot of time with this helical entry well above the part.
07:10
So we need to consider how much time we're spending and if that makes sense, notice that the lead out has dropped based on linking constraints.
07:19
And that's simply because the tool is too large, in order to completely lead out based on the default parameters,
07:28
I'm going to make one adjustment to the 2D contour and that's in the heights section.
07:33
The feed height where it starts to create that feed operation, right now, is based on the top and the top height is based on the stock.
07:41
What I'm going to do is change this to a selection since I know I have machine down to at least this face,
07:46
I'm going to set that The top height is now based on that selection and then the feed height is based on .1,
07:54
where we have to be careful with this is in the fact that it's trying to jump over geometry.
08:00
Now it's telling me that the ramp clearance and the vertical lead in radius is higher than the feed height,
08:05
and it says that we should consider reducing the ramp clearance value and raise those to match.
08:12
We're going to say okay and we want to make sure that these clearance heights, these ramp heights where it's wrapping up to are going to be fine.
08:20
Everything looks pretty good from there. I'm happy with those results.
08:23
I still have a warning about my lead ins and lead out, but at this point I think the toolpaths look pretty good.
08:29
We still need to finish the outside in which we're going to use that quarter inch 10 mil.
08:33
So once again we'll create a 2D contour, quarter inch flat around the outside of the park,
08:40
we're not going to be leaving any stock and depending on our requirements,
08:45
we can determine whether or not we want to repeat the finish pass,
08:48
whether or not we want to have a roughing pass and if we want to use that ramp option again.
08:55
Now, in the case of this toolpath, I want to allow it to do a roughing pass and the roughing pass is going to be a very small amount.
09:03
I'm going to use .05 and we're going to do one roughing pass and one finish pass.
09:09
So this is going to allow it to do that roughing pass. And then it's going to step in that .05 to do it's finished pass.
09:15
Now remember that roughing pass is supposed to remove a bit of material, so maybe we can take that in a little bit more 2.025.
09:25
That will remove some material and then they'll allow us to do a final finish cut on the last bit.
09:31
Keeping in mind that we are seeing some stock here. But again we have stock left from the other side that we know it's going to be removed.
09:38
The last thing that we need to do is we need to finish the final diameter of these holes.
09:44
If they are critical, then we want to use something like a bore toolpath.
09:51
I'm going to go in with an 8th in flat end mill on aluminum finishing and I'm going to select the inside bore of each hole.
10:00
While this isn't strictly required. We could do a
10:03
This is a good way for us to come in and make sure that we're not engaging too much material with that tool.
10:10
Everything looks pretty good, and it's always a good idea for us to save often.
10:13
So at this point, let's make sure that we do save the design before we move on to the next step.
Step-by-steps
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.