Drill mounting holes

00:02

Drill mounting holes.

00:05

After completing this video, you'll be able to create drilling operations

00:11

in fusion 3 60. Let's carry on with our data set. From the previous example

00:15

at this stage, we've taken a look at an adaptive clearing.

00:18

We have used two D contour to finish the outside of the part

00:22

two D pocket to semi rough the piston bore.

00:25

We used a bore tool path to finish the piston bore

00:28

two D pocket to finish off various faces and a two D

00:31

contour to finish off the area that we're calling our rotor relief.

00:35

The next thing that we need to do is we need

00:37

to take a look at drilling the holes on the part.

00:40

This has to happen a few different ways

00:42

because of the geometry that we're dealing with.

00:45

For example, as we rotate this around,

00:47

there's a counter bore on the back side of this part,

00:50

which means that the hole from the top side doesn't extend all the way down.

00:54

And this is something we need to be aware of when making our selections.

00:57

This hole here is a bit larger than all the others.

00:60

And using inspect, we can see that the diameter is 0.313

01:04

while the other holes are coming in at 0.255.

01:08

So when we take a look at these different values and information,

01:11

we need to plan accordingly when we're drilling our parts

01:15

to get started. However, we want to begin by spot drilling each of the holes.

01:19

We're gonna start by using the drilling tool path

01:22

and we need to select an appropriate tool.

01:24

Once again,

01:25

we're gonna go into our tool library and

01:27

notice that it's automatically filtering by hole making.

01:30

We have a couple of different tools that could be used.

01:33

But we wanna get started by using tool number one, which is a spot drill.

01:37

We're gonna be using the spot drill on all the holes.

01:40

And there are a couple of different ways that we can select those holes.

01:43

The selection mode can be based on selected faces,

01:46

selected points or even a diameter range.

01:49

We also have options for things like select same diameter

01:52

and auto mege

01:53

whole segments.

01:55

Whenever we're dealing with a

01:56

chand

01:57

countersunk or counter board hole.

01:59

If we're selecting it from that direction,

02:01

we can auto mege those segments making the selection process a bit easier.

02:05

However, because our counter board is from the backside of this part,

02:09

that option is not gonna work.

02:12

So let's get started manually selecting these holes

02:15

and I'm gonna sort of haphazardly select them.

02:18

And as soon as I have all of those selected

02:21

fusion 3 60 is going to use the optimized order.

02:24

And when we move over,

02:25

it's going to account for each of those holes we selected

02:29

and figure out the most efficient way to drill them.

02:31

Without me worrying about the order in which I selected them.

02:35

The next step is going to be determining our heights at this point.

02:39

We want to make sure that we identify the fact that by default,

02:42

it's going to be using the bottom of the hole.

02:45

We don't really want to take our spot drill all the way through these holes.

02:49

So we're gonna change the bottom height from whole bottom to whole top.

02:54

Then we're gonna use the drill tip through bottom,

02:56

which will allow us to simply engage the hole and create that spot drill.

03:01

However, we are using a quarter inch spot drill,

03:04

which means that we're getting relatively close to the actual diameter of the hole.

03:09

If we don't want to take it in that far, what we need to do is make some adjustments.

03:14

Now,

03:14

there is a breakthrough depth and an offset value and these are going to be slightly

03:19

different than we're used to when we're talking about changing the depth of a cut.

03:24

For example, if I change the breakthrough depth to 0.05 it's gonna go a bit deeper.

03:30

Now, remember the Z values at this point are negative, but

03:34

when we're talking about the breakthrough depth,

03:36

we're talking about an additional clearance or distance that we want to go through.

03:40

If I set this value to a negative value, notice it doesn't allow it.

03:44

It's not allowing me to use that value.

03:46

So what we need to do is we need to leave that at zero

03:49

and we can enter a manual offset value of 0.5.

03:55

So what this allows us to do is increase that Z

03:58

value in the positive direction up and away from the part,

04:01

we simply want to spot this so that our drill bit

04:03

is going to be centered when we begin drilling our hole.

04:06

The next thing that we want to do is take a look at our cycle, which in this case,

04:10

because we're just spotting the holes,

04:12

drilling and wrap it out will be perfectly fine.

04:14

And we'll say, OK,

04:16

when we hit F seven,

04:17

we can see that the order in which we selected the holes is

04:20

different than the order that it's actually going to be drilling them.

04:23

It's starting on this right hand side and it's

04:25

spotting each of these holes moving its way around.

04:28

Keep in mind that the yellow lines are rapid movements and we want

04:31

to make sure that all of our movements are above the part.

04:34

So we're not worried about intersecting any solid geometry

04:38

when we go on and we move into actually drilling the holes.

04:41

The next step in the process can be to right click and to duplicate this tool path

04:47

by duplicating tool paths for example, a drilling tool path,

04:50

we can save the time without having to reelect all the holes.

04:54

However, we're gonna do this in two individual steps.

04:56

So we're gonna use the drilling tool path again.

04:59

And we're going to manually make our selections again

05:02

this time. Instead of using tool number one, we're gonna be using tool number four.

05:06

So again, we have to go back to our library.

05:09

This is going to be a 2 57 or an F

05:12

which is typically going to be clearance for a quarter 20 screw.

05:16

While the holes in the part are 2 55 the 2 57 will fall within

05:21

the tolerance listed on the print so we can use this drill bit without problem.

05:25

We also want to make sure that we note that there is cutting data associated with us.

05:29

So we wanna make sure to select the aluminum drilling and you select

05:34

next, what we're going to be doing is only drilling three of the holes.

05:38

We're gonna leave the ones with the counter board to do individually afterwards.

05:42

So I'm gonna to manually make these selections.

05:45

The next thing we're gonna do is go to heights, turn on drill tip through bottom

05:50

and I'm gonna add an additional clearance as a positive value.

05:54

This means that the drill is going to go through the bottom of the holes.

05:58

And as we rotate the part around, we want to make sure that it is extending everywhere

06:02

keep in mind the material here on both sides of the part has not been machined yet.

06:07

When we look at the stock, those are still going to have full material.

06:11

But the reason we want the drill bit to extend through

06:13

here is because when we start roughing and finishing those sides,

06:17

we're gonna leave somewhere between 2030 thou on the part when we're roughing it

06:22

and we want that roughing operation to go all the way through.

06:25

So that way we have a hole in the part rather than leaving a sharp

06:29

edge or a potential material that will get dragged or smeared across the part.

06:34

So making sure that we extend at least the amount of rough stock to leave that we're

06:38

gonna have when we flip the part over is going to be sort of a good practice.

06:43

Then when we have our drill cycles, now that we're actually drilling a hole,

06:46

we're gonna change this to either a chip breaking or deep drilling,

06:50

just hold the cursor over the drilling cycles.

06:53

And you can get information about what each of these is going to do

06:56

for us.

06:57

The chip breaking or G 73 is going to allow us to engage the

07:01

drill bit retract and then keep that pecking motion as we're creating our holes.

07:06

Deep drilling is another way that we could do this,

07:08

but this allows the drill bit to come all the way back

07:10

out of the hole rather than just a small peck and retract.

07:14

So we wanna make sure that we're using chip breaking

07:16

and I'm gonna use all the default settings and say,

07:18

OK,

07:20

so now we need to take care of the last two

07:23

holes before we move on to doing a boring operation.

07:26

The last two holes here again have that counter bore,

07:29

which means it's going to be slightly different, but we're gonna use the same tool

07:33

moving to our geometry. I'm gonna select these holes.

07:36

But the main difference here is that we want to make sure

07:39

that we go all the way to the bottom of the part.

07:41

So rotating this around, we're going to use the selection option

07:47

and then we want to extend through the bottom.

07:50

And again, we're gonna add a small amount in this case, 0.05

07:54

by doing this,

07:55

we want to make sure that we extend all the way past

07:58

that counter board to make sure that the hole is gonna be centered

08:01

while it's not strictly required, we could just go to the bottom of our 2 57 hole.

08:06

It is helpful for us to do this in this stage,

08:09

making sure that all of the holes are perfectly aligned.

08:12

The counter bar on the other side is only gonna be clearance for a

08:16

socket head cap screw.

08:18

But again,

08:18

it's going to be good practice for us to make

08:20

sure that we do all of the critical features.

08:22

In this case, holes from one side.

08:25

The next step is to make sure that we do have the appropriate cycle.

08:29

This is a slightly deeper hole, but the chip breaking cycle will still be fine.

08:33

So we're gonna say, OK,

08:35

the last thing that we need to note is that some of these holes, specifically,

08:39

these two holes are larger than the drill bits we have loaded in the machine.

08:43

Now, in some instances,

08:44

you might find that you want to use a machining cycle

08:48

and a small end mill to finish off specific holes,

08:51

whether it's a case of a limited number of available spots for your

08:54

tools or if you need more precision than a drill bit might offer.

08:59

So in this case, what we're gonna do is again, take a look at our two D board tool path,

09:03

which we've already used.

09:04

This could be done with two D contour. It could also be done with a two D pocket.

09:09

Assuming that we had enough of a pre drill to take an end mill in there,

09:13

we could go all the way down and just simply move our way out.

09:16

Either of those options is gonna be fine.

09:18

All of the things that you need to

09:20

consider when you're deciding which tool path to use

09:23

for us.

09:23

Since we've already looked at the board tool path,

09:25

we're just going to reuse this again, going into our tool library.

09:29

This time, we want to use a quarter inch flat end mill, which is tool number five,

09:34

we're gonna take this tool

09:35

using the board tool path and simply make our selections.

09:39

Remember that the bore tool path is automatically taking

09:42

a look at the height of the selected face.

09:45

So we don't have to worry about altering or changing the starting height.

09:48

However, it is rapiding well above the part.

09:52

So we could potentially be wasting some time by moving that high above the part.

09:57

So what we wanna do is we want to think about these rapid movements,

10:00

we're starting and ending at this clearance height, those are rapiding down,

10:05

but the movement across is happening to this retract height.

10:10

So the option that we have here for the board tool

10:12

path is for us to reduce this retract height plane.

10:15

Notice that it is also bringing our clearance height down.

10:19

Keep in mind that this can be dangerous,

10:21

especially if you're not sure where the tool

10:24

is going to be rapiding between movements.

10:26

So make sure that you are aware where the tool is coming from and where it's moving to.

10:31

This is something that we definitely need to validate in simulation because

10:35

we can take a look at what happens between tool paths.

10:38

If I shift, select multiple tool paths,

10:41

note that it is showing all of these tool paths, all the drilling cycles.

10:45

So for example, if I show the bore and then I shift, select the pocket,

10:50

I get a preview on the screen of both of those,

10:52

if I take a look at this drilling tool path, we're ending at this hole here.

10:56

And then if I shift, select the bore, we're moving our way over to here.

11:01

And what this means is that we potentially might want to simply reverse this.

11:05

But keep in mind

11:06

between these two, we have a tool change,

11:09

which means that the tool is gonna retract completely before moving over again.

11:14

These are all things that we need to think about.

11:15

When we're planning out our tool paths

11:18

at this point, it looks like we've got everything taken care of.

11:21

But let's go ahead and make sure that we save before we move on to the next step.