Create a drilling operation

00:02

In this video, will create a drilling operation.

00:05

After completing this step, you'll be able to create a spot drilling operation and a chip breaking operation.

00:13

In fusion 360, we want to carry on with our gear housing for CNC mill.

00:18

At this point we want to begin to drill and tap the threaded holes on the back side of our part.

00:23

To do that, we're going to start by going to drilling and select drill.

00:28

We first need to select the tool we need and if we go into our cam DFM library, notice that it only shows us three different tools.

00:35

When the tools are created in the library,

00:37

there are some check boxes that allow them to be used for things like live tooling in a CNC lathes or whole making.

00:44

So in this case we want to select tool number one which is our eighth inch spot drill and notice that we have to cutting data presets.

00:53

We have aluminum finishing an aluminum drilling that are of interest to us notice the rpm difference as well as the plunge feed rate difference.

01:02

The aluminum finishing is going much slower than the aluminum drilling.

01:06

In this case, I'm going to use aluminum drilling and select.

01:10

Then I need to go to my geometry tab and select the holes.

01:14

There are a few different ways that we can do this, we can select faces, points or use a diameter range.

01:21

If we take a look at a diameter range, we can say go between .2 and .25.

01:29

When we do this notice that it's getting the outside holes and we don't want to drill them from this direction.

01:34

Those are critical and we want a machine. All that from the other side.

01:38

We know that the tapped hole is .201.

01:41

So if we reduce that value 2.21, it will enable us to grab all the holes of interest and omit the larger ones.

01:50

Notice that there are no containment boundaries. We're not changing the order.

01:54

Were simply letting it go in the order in which it grabbed these holes.

01:58

Next, for the heights, this will be important because we're only spot drilling and we don't want to go all the way to the bottom of the hole.

02:05

So we need to make some adjustments first by changing the bottom height,

02:09

we're going to go to the whole top and then we're going to use the drill tip through bottom dialogue.

02:15

If we view this from the side and we zoom in, you can see this allows the drill tip to go all the way in until it gets to the nominal diameter.

02:25

Now in this case because we are spot drilling, this is going to be good.

02:28

And we're using an 8th in spot drill,

02:31

which means that it's small enough that will allow us to spot drill without worrying about enlarging the whole at all.

02:37

So we're going to say, okay, and now we've created our first drilling operation that allows us to spot drill those holes.

02:44

If we want to reuse the same information.

02:47

One thing that we can do is we can right click on our tool path and we can select duplicate.

02:53

When we duplicate it, will create an exact copy and then we can right click and edit.

02:59

We'll start by changing the tool we're using, we'll go to Cam DFM and we'll select tool number two, which is our number seven Drill.

03:07

The next thing that we want to do is go to geometry and reverse the order,

03:12

because the spot drill is starting at one point and working its way around when we reverse the order.

03:17

That means that when the tool change happens,

03:20

the drill is already in the right position and it makes sense for us to just go backwards through that same orientation.

03:27

Next, we want to change the depth.

03:29

In this case, we're going to go to the whole bottom,

03:32

but we don't want to go all the way through the part because if we use drill tip through bottom,

03:38

we need to be careful that we're not going down too far.

03:41

Remember that these are blind holes.

03:43

So we want to be aware of how deep we're going.

03:46

And keeping in mind that the drilling tool path uses our face selection and it's not accounting for the taper at the bottom of the hole.

03:54

So in this instance we're going to use drill tip through bottom and then we're going to validate this with simulation later.

04:01

Next we want to go to our cycle and determine how we want these holes to be drilled because we're only going down less than quarter inch.

04:09

We could probably just simply take the drill bit in and pull it back out.

04:14

But because we are creating a hole that's going to be a tapped hole,

04:18

I want to be a little bit more careful and I want to use what's called a chip breaking cycle.

04:23

The chip breaking allows us to define a partial retract, meaning that the drill bit will go down a certain amount,

04:29

then it will retract a certain amount, giving it a chance to clear the chips and allow more coolant to get in there.

04:36

So we're going to use the default values but note that there's a pecking depth value.

04:40

And as a chip break distance we're going to say, okay and allowed to create that.

04:46

Now I want to validate the depth and we're going to do that by using simulation, which will come at a later point.

04:53

We still need to program a few more things.

04:55

So let's make sure that we get the tapping operation and then we can validate our tool paths.

05:00

For now, let's go ahead and save and then we can move on to the next step.