00:02
create tool paths. To finish cut parts.
00:05
After completing this video, you'll be able to create a facing tool path,
00:10
Contour tool path, create chance for and two D.
00:12
Contour champ for tool paths and create a drilling and tapping tool path
00:20
Infusion 3 60. We want to carry on with our mounting block part.
00:23
You have any difficulties in the last video.
00:25
Make sure that you upload the supply dataset mounting block rough dot F. Three Z.
00:30
At this point we've already created a two D. Pocket tool path and a two D.
00:34
Adaptive tool path to make sure that we
00:36
can identify the differences between the two.
00:38
But now we want to take a look at finishing tool paths.
00:42
Remember that the order of operations is typically dictated by the part
00:45
but in general you will use a facing tool path first.
00:48
Then you'll rough apart before you finish it.
00:51
In this case now we're going to go back and take a look at a
00:54
two D facing tool path and then we'll move on to some finishing tool paths.
00:58
Under the 2D dropdown will select face
01:01
and we need to select a tool for facing
01:03
when you're facing apart.
01:05
In some cases you might use a large end mill while in
01:08
other cases you might use a shell mill or a face mill.
01:11
In this example we're going to use a large three quarter end mill
01:15
under the geometry section fusion 3 60 will automatically bring in the
01:18
border or the outside shape of the stock used in your setup.
01:22
No selection is needed but you can select a different area if
01:25
you want to focus the tool on just a specific area.
01:28
However it's important to note that with a facing tool path,
01:31
the tool will always enter and exit the outside of your selection
01:36
for the heights fusion 3 60 will automatically pick the top height as the
01:40
stock top and the bottom height as the model top in the passes section.
01:44
You want to make sure that you dictate the
01:46
number of passes based on the step over amount.
01:49
In this case our tool is three quarters of an inch
01:51
so I'm going to go 30.7 inches between each step.
01:54
Once we say okay our passes are created in order to face the part
01:60
We can also take this facing tool path and we can drag it
02:03
all the way up to the top of our tool path list.
02:05
This means that even though it was created after our pocket and adaptive tool paths
02:10
it can be moved up in the line and that way we can have it at the very top.
02:14
Next I'm going to take my two D.
02:16
Pocket right click and suppress when I suppress the tool path,
02:20
it will still remain inside of our setup.
02:22
it's no longer going to be used to calculate stock removal or any rest machining.
02:26
Now we have our original facing tool path and then we have our adaptive tool path.
02:32
Keep in mind our adaptive tool path has left material on the walls and the floors.
02:37
We need to make sure that we go back and we remove this material.
02:40
But remember that with the small size here we've got
02:43
a little bit of stock left in the middle.
02:44
And this is going to be an important consideration when planning our tool paths.
02:49
The next thing that we want to do is take a look at a two D.
02:51
Contour and how that can be used to finish off that inside pocket.
02:56
Two D drop down and select two D contour,
02:58
we need to select a tool and in this case
03:00
our quarter inch flat end mill will work just fine
03:03
from our geometry selection we need to select a chain or a face that we want to use,
03:08
notice that we have our selected contours and pocket recognition.
03:12
We're going to use the selected contours option
03:14
and select the bottom edge of our pocket.
03:17
The red arrow is going to determine which side of that edge is going to be machined.
03:21
In this case we want to make sure it stays on the inside.
03:24
In the heights section,
03:25
this will automatically be done at the selected contour bottom height
03:30
for our passes with the two D contour, it's going to create a single pass
03:34
directly on that edge.
03:37
In this case it will offset it based on our tool
03:39
diameter because we're using a compensation type of in computer.
03:43
If we turn compensation off the center of the tool
03:45
will be directly on the center of our selection.
03:48
Other options such as in control where and in verse
03:51
where will put specific codes inside of your G.
03:53
Code when you post process your tool path.
03:56
This will allow you to make adjustments to the offset of
03:58
the tool path based on parameters set inside of your machines.
04:03
in this example we're going to leave this on in computer but it's a good
04:06
idea for you to review these settings and which one is best for you.
04:09
You can always hover over a dialog box and take a look at the tool tips.
04:14
Next as we go down the line, notice that there's a finished feed rate.
04:17
We can make adjustments to these parameters
04:19
and determine if we want the finishing feed
04:22
rate to be faster or slower than the default feed rate of our tool.
04:25
In this case we're going to leave it at 72
04:28
next as we go down the list,
04:30
there are some other parameters such as overlap for the finishing lead out,
04:34
In this case it's called lead and distance.
04:37
Then we also have roughing passes multiple depths and stock to leave roughing
04:42
passes will allow us to make multiple
04:44
passes horizontally from the selected contour.
04:47
Multiple depths will allow us to make multiple cuts at different Z values and
04:51
stock to leave will determine how much material we want to leave on the wall
04:55
and are linking parameters. We have a ramping option
04:58
that allows us to use our selected contour and ramp the tool down at a specified angle
05:03
in this case, two degrees is the default,
05:05
which means that the tool will follow the external contour shape,
05:09
but it will be moving down at a two degree angle the entire time.
05:12
This can help with a consistent tool load
05:14
and prevent too much tulle burial into material.
05:17
If we say okay, the tool path is going to be created with a two D,
05:20
consistent ramp going down our selected contour
05:24
in the bottom section of our window,
05:26
I'm going to turn off the tool paths and note that
05:28
we have stock left at the bottom of our pocket.
05:31
Now part of this is because we didn't create a tool path in this case
05:35
are too deep pocket to remove all the material from the bottom of our part.
05:39
The two D. Adaptive was used as a roughing tool path. Only
05:43
in some cases you might determine that you want to use a two D.
05:46
Pocket instead of a two D contour simply because you want to
05:49
machine the bottom face of that pocket as well as the walls.
05:53
I'm going to right click on my two D contour and suppress it.
05:56
Say yes, Then I'm going to go back to my
05:59
pocket, right click and un suppress it and then drag it to the very bottom.
06:04
Under my two D. Adaptive, let's go ahead and edit R. Two D.
06:07
Pocket tool path in the past this section in
06:10
this case we want to turn off multiple depths.
06:13
We're going to machine the entire pocket at the maximum depth and say okay
06:17
this will allow us to create a tool path that will machine
06:20
the entire bottom of the pocket as well as all the walls.
06:23
You can go back and turn on your tool path,
06:25
visibility and see that our tool path is created only at the bottom,
06:29
notice also that it's creating two helical entries.
06:32
This is because we've got material left in the middle of our part,
06:35
we can always make adjustments to previous tool paths such as our adaptive cut,
06:40
Go to our stock to leave and instead of using a .02 radial stock to leave,
06:45
we can leave a smaller amount such as .005 and see if we
06:49
can get the tool to go all the way through the center.
06:52
It leaves a smaller amount of material here.
06:53
But we still have a potential problem using this size tool.
06:57
These are all things that we need to consider and just using a tool path like a two d.
07:01
Pocket doesn't necessarily mean that you can avoid these issues.
07:04
The tool will still go directly through that area and
07:06
we'll have a large tool load in those corners.
07:10
The next thing that we want to talk about is d burying the inside edges.
07:13
This is typically done with a two D champ for tool path,
07:16
there are two ways in which we can do this using R two D tool paths
07:20
contour has a chance for option. If you select a tool that's applicable for two D.
07:26
champers tool path itself has some additional options,
07:29
such as collision detection with surrounding geometry.
07:33
The first thing that we need to do is select an appropriate champ for mill tool.
07:36
We don't have any in our document or in our sample library.
07:40
So we need to go down into our fusion 3 60 library and we want
07:44
to make sure that we take a look at the engraved champ for mill type
07:48
from here. We need to select a tool that we want to use.
07:51
In this case we're going to go into our milling tools,
07:53
inch section and select the second tool which is 0.4 to five
07:56
inch 45 degree champ for we'll select this and say OK,
08:01
And next we'll move on to our geometry.
08:04
We're going to select the upper edge of the pocket.
08:06
Next we'll move into our passes and here's
08:08
where we're going to determine the champ for.
08:10
With this is going to be a relatively small chance for at .01 and we're going to
08:15
use a very small chance for tip offset because
08:18
we have a relatively large champ for tool.
08:20
We need to make sure that we're not pushing it too deep into the pocket
08:23
because we do have some collision areas that we need to be aware of.
08:27
Also note that we have a chance for clearance amount.
08:29
This is going to prevent the tool from intersecting with other solid geometry.
08:34
the tool will move around and create a chance for if we zoom in note that we're
08:38
not able to cut the champ for in the center because of the geometry of the tool,
08:43
this means that we would need to use a smaller
08:45
diameter tool in order to get into all these corners.
08:49
We can make adjustments to the tool or we could potentially
08:52
select another tool that could be used for this application.
08:56
If we select the tool that we want to use,
08:58
make sure that we are using engraved chant for tools.
09:01
Notice that inside of our sample library, we don't have anything available.
09:05
In some cases you might choose to use an engraved tool which will
09:08
allow you to get into those corners closer for this example however,
09:12
we're going to cancel and just note that we aren't able to
09:14
get all the way into those corners with the supplied tool.
09:18
The last thing that we need to do on this side of the part is drill and tap all the holes
09:22
for this. We're going to select drilling.
09:25
We're going to select our tool from our three axis
09:27
sample library which is going to be tool number one,
09:29
our spot drill and then we're going to select our holes in the geometry selection.
09:35
We have a couple options that we can use
09:37
selected faces points or diameter range for this selection.
09:41
I'm going to use the faces option and select the inside of each hole.
09:46
We're also going to move over to the heights
09:48
instead of going all the way to the bottom of
09:50
the hole because we are using a spot drill,
09:52
we're going to go to the whole top.
09:54
Then I'm going to use the drill tip through bottom option
09:57
which will allow us to just create a small spot.
10:00
Once the tool path is generated,
10:02
we can see a preview on the screen showing that small spot drill.
10:05
Next I'm going to right click on that tool path and I
10:08
want to duplicate it because we already have our whole selected.
10:11
We can simply duplicate the tool path,
10:13
change the tool that we want to use from our three access sample library.
10:17
In this case, a tool number to a .201 drill.
10:21
We're going to move on to the geometry,
10:23
make sure that all the holes are selected and then
10:26
to our heights instead of using our whole top,
10:28
we're going to use the whole bottom and still
10:30
allow the drill tip to go through the bottom.
10:32
We can also add a breakthrough depth.
10:34
If we want the tool to go a little bit farther in this case .05
10:39
last we want to set the cycle of the drill because we are doing more than just a spot.
10:43
We're going to be using a chip breaking cycle
10:46
that allows the drill bit to go in a small amount and then come back out a
10:49
little bit to allow the chips to clear and cool it to get into those holes.
10:53
This is especially important on deeper holes.
10:56
Next I'm going to create another drilling operation this time I
10:60
want to make sure that I'm using the tap tool.
11:02
We could simply duplicate the operation one more time.
11:07
the tap tool has a slightly different approach to
11:09
how the geometry is going to be accounted for.
11:12
When we move over to our cycle,
11:14
notice that it automatically is set to tapping based on our tool selection.
11:18
If you duplicate a tool path and simply change to a tapping tool,
11:22
you need to make sure that you are using the tapping cycle.
11:25
This allows the tool to go in at a small feed rate and then it'll stop at
11:29
the bottom and reverse the tool back out of the hole to prevent damage to the threats.
11:34
In this case we're going to say,
11:35
okay and now we've created our tool paths for spot drilling,
11:39
drilling and tapping those holes
11:42
at this point let's go ahead and navigate back to a
11:44
home view and make sure that we saved before moving on
AutoCAD
AutoCAD LT
Fusion
AutoCAD Revit LT Suite
Architecture, Engineering & Construction Collection
Revit
Civil 3D
BIM Collaborate Pro
Product Design & Manufacturing Collection
Maya
Inventor
Navisworks
3DS Max
Flow Production Tracking
Revit LT
Forma
Recap Pro
Alias Concept
Maya Creative
Flame
Arnold
Mudbox
Flow Capture
Media & Entertainment Collection
