00:00:07,500
Spot Drilling and Drilling are both hole machining operations.
00:00:11,100
There are many hole machining cycles in Fusion.
00:00:14,866
They are mostly derivatives of these two basic cycles.
00:00:18,766
Our part has a chamfer on the top of the hole.
00:00:21,766
We'll be creating that chamfer during the spot drilling process, with a 90 degree spot drill
00:00:27,500
Fusion will determine the diameter of the chamfer, from the information on the model.
00:00:33,333
so let's start by selecting the drill on icon from the toolbar
00:00:38,133
This brings up the drilling dialogue. On the Tool tab let's go to Select tool,
00:00:43,566
Which will open up our Tool library.
00:00:47,866
Right here we have a filter
00:00:51,833
click on the filter and in here, we can select the types of tools that we want it to look for.
00:00:57,733
right now the selected options are the chamfer mill, which you can see in the icon up here,
00:01:03,566
the drill and the center drill. So I could say I want to see
00:01:07,900
None,
00:01:10,100
Except for Spot drills. OK that
00:01:14,333
Now it will only show me spot drills.
00:01:17,066
now we're going to look to our Intro to 2D machining library,
00:01:21,166
For the half inch spot drill, In our existing library.
00:01:25,833
You can double click to select that.
00:01:29,200
On the Geometry tab, we can select the locations to spot drill.
00:01:32,966
For this lesson we'll be selecting by hole face.
00:01:36,966
or in this case the whole chamfer face.
00:01:41,933
But first I want to check the box that says Select same diameter.
00:01:46,166
This will force Fusion to look for all of the holes that are similar to the one that we pick.
00:01:51,066
I also have a check box under Optimize order.
00:01:54,266
Which will sort out the holes in the most efficient tool path.
00:01:58,166
Right now for our whole faces it says nothing is selected
00:02:02,600
our selection mode is currently set to selected faces
00:02:07,466
and I want pick this face here, that represents the chamfer.
00:02:13,866
You can see it immediately found all the other holes there like that
00:02:17,733
and optimized them in a more efficient order.
00:02:21,166
The first one I picked, is not the first one that it's machining.
00:02:25,633
on our Heights tab we can define the top and bottom Heights.
00:02:29,966
Make sure the Top height is set to the hole top
00:02:34,900
and at the Bottom height is set to the hole bottom.
00:02:39,133
what that will do is look at the angle of the chamfer and figure out where those walls
00:02:44,400
converge together and the point where they converge together is the final depth for the spot drill.
00:02:51,100
So we don't have to figure out any value to put in here for our depth offset.
00:02:56,966
Now let's go to our Cycle tab.
00:02:59,233
In here the cycle were going to be using is the basic drilling cycle it will feed into depth and then rapid out.
00:03:08,200
Press OK and all of our spot drilling is complete.
00:03:12,466
At this point you may want a stop the video and do this yourself
00:03:16,433
before we go into the next process for drilling holes.
00:03:23,333
Now to drill the holes we could make all the selections again
00:03:26,866
or we could pick this tool path we just did, right click and say Create Derived Operation -
00:03:34,366
Drilling - Drill.
00:03:37,666
If you remember from our previous lesson the diameter of the holes was an eighth of an inch.
00:03:43,166
So let's go to Select, from our tool library.
00:03:46,433
It looks like in our existing library
00:03:48,700
we don't have any eighth inch diameter drills. But that's not a problem.
00:03:52,500
We can go up here to look at our libraries
00:03:56,666
and we can do the Dimensions to tell it what we're searching for. I'm searching for a diameter somewhere between
00:04:05,000
0.120 and
00:04:07,866
0.130
00:04:10,200
so here's an eighth inch drill
00:04:13,266
we can double click to select that.
00:04:15,566
Now we can move to our Geometry tab
00:04:19,066
Now under Geometry, we selected faces and we told it to look for all the same Diameter.
00:04:24,533
Which we still want. But we're also going to tell it to Auto Merge hole segments
00:04:29,800
and were going to come over here and select an additional face.
00:04:33,033
This time I'll pick the drilled hole and
00:04:35,866
what it will do in that case is, look at all of that, to represent the total Z depth.
00:04:43,033
because I don't want to start drilling
00:04:45,666
from the bottom of the spot drill. I want it to start drilling
00:04:49,800
from the top of the chamfer.
00:04:52,433
So it's going to merge those whole segments together and still optimize the order
00:04:58,733
Lets take a look at our Heights. Top height will still be from the hole top.
00:05:03,866
or you could set that to, from the model top.
00:05:07,933
Since they're all going to be in reference to that model top.
00:05:11,000
But the advantage of having it be from the hole top is that
00:05:15,100
if all of your holes are at different Heights
00:05:18,400
it will drill each one, starting from the appropriate location.
00:05:23,333
Same thing for hole bottom.
00:05:25,066
If you have many holes and they all have different depths,
00:05:27,966
it will determine the hole bottom from each feature
00:05:32,800
now we want that hold a drill all the way through
00:05:35,366
so we're going to turn on
00:05:37,300
Drill Tip through bottom
00:05:39,366
and tell it that I want a breakthrough
00:05:42,233
by an additional .030"
00:05:45,233
Notice you don't have to tell it a -.030" Because it knows it's breaking through.
00:05:51,300
So it knows it has to go further in the negative direction.
00:05:55,333
You're just telling at a distance to go further
00:05:59,533
Take a look at our Cycle tab.
00:06:02,300
Now when we click on cycle type, you can see there's a lot of different cycles.
00:06:07,033
These are all the cycles that fusion supports. However your CNC Machine
00:06:12,100
may not support all of these different hole making cycles.
00:06:16,733
The most common ones are drilling
00:06:18,800
counter boring, chip breaking
00:06:21,333
deep hole drilling and tapping.
00:06:24,266
in this case lets do a deep drilling cycle.
00:06:28,100
the common peck drilling cycle.
00:06:30,500
Fusion automatically determined the incremental peck depth, based on a percentage
00:06:35,566
of the diameter of the tool. Now of course you can right click in here and say edit expression
00:06:41,266
to see exactly how it calculated that
00:06:44,233
it's the tool diameter times 0.25
00:06:47,766
so it's 25% of the diameter of the selected tool.
00:06:51,800
Leave it the way it is.
00:06:55,233
Say OK
00:06:57,600
Now all of our holes are drilled through the part.
00:07:02,100
Feel free to select the setup, right click your mouse and go to simulate.
00:07:06,766
Or you can select simulate off the toolbar.