Practice exercise

00:01

This is the practice exercise video solution

00:04

for this practice exercise.

00:05

Let's begin with the supply data set caliper bracket dash cams setup dot F 3D.

00:10

This already contains a setup

00:12

one with stock and we're gonna be machining this

00:14

without worrying about how it's held in a vice.

00:17

It's always important for us to understand how our parts

00:20

are held because it will affect the tool path,

00:22

the clearance and the way in which we approach the different operations.

00:26

But for this example, let's focus just on the tool path and not how the part is held

00:31

to get started. We can use a two D or a 3D adaptive clearing.

00:35

Once again, the 3D adaptive clearing is going to be model aware,

00:39

which means that we don't really have to make any selections on our part.

00:42

We're gonna start by going into our precision

00:44

machining tool library and selecting tool number seven,

00:47

which is our half inch flat end mill

00:49

in the geometry section fusion 3 60 automatically grabs our stock contour and

00:54

it's going to be looking in that area for areas to machine,

00:57

we can toggle off rest machining since this is our first tool path

01:01

in the height section, we do wanna make sure that we are going below the part

01:05

and in this case, I'm gonna set this at 0.05.

01:09

Then in our passes section,

01:12

we want to make sure that we identify stock to leave is currently set at 0.02 or 20.

01:16

Th

01:17

this means that even though we're going 0.05 below our part,

01:22

the actual stock that's gonna be remaining is 0.03.

01:25

The difference between those two values

01:27

we're gonna say, OK, and allow it to generate,

01:30

we can see that we've roughed out the entire part.

01:33

And now we're gonna move on to finishing the outside profile.

01:36

Once again, consideration on how the part is held is always important.

01:40

But for these practice examples, we're only gonna be focusing on the tool paths.

01:43

So from our two D menu, we're gonna select two D contour,

01:48

we're gonna carry on using the same tool number seven.

01:51

And the geometry will simply be this bottom edge,

01:54

the height by default is going to be based on that selected contour,

01:57

but we need it to come down a little bit further.

02:00

Remember that the Z values are based on the coordinate system.

02:04

In this case with everything except for drill tip

02:06

through bottom when we're using a drilling operation.

02:09

So

02:10

Z up and away from the part is positive and Z down is negative.

02:14

If this is tricky, we can always change the bottom height to model bottom,

02:18

which will bring back our plane

02:20

and we can take a look at entering a positive value

02:23

noting that it's coming up on the part or

02:25

a negative value noting that it's going below.

02:28

Remember in the two D or 3D adaptive tool pass that we use to rough

02:32

our part stock to leave is gonna come into play with the bottom height.

02:36

We wanna make sure that we don't take our two D

02:38

contour tool and bury it into the stock at the bottom.

02:41

So for this reason, we're gonna have 0.03

02:45

in the passes section.

02:47

We want to make sure that we're not using stock to leave and we can

02:49

carry on adding things like repeating the finishing

02:52

pass if needed or adding roughing passes.

02:54

If we want to make sure that we add additional passes,

02:57

I'm gonna set this at 0.2 inches and say, OK,

03:01

this allows us to create a roughing pass and then come back with our finishing pass

03:06

once again, the 3d Adaptive cleared out most of this material.

03:09

So the roughing pass is really not needed. In this case,

03:14

any changes can be done by right clicking and editing our tool path,

03:17

going to our passes section and toggling off roughing passes and saying, OK,

03:22

now that we have the outside of the part finished,

03:24

let's go back and focus on finishing off the various areas and faces.

03:29

We're gonna be using our two D drop down and selecting two D pocket

03:32

again with the same tool number seven.

03:34

And for our geometry, we want to select the various faces that we want to finish.

03:39

Fusion 3 60 will be able to identify areas

03:41

where there are contours that need to be created.

03:44

So for example, around the outside of this box, we see a darker blue line

03:48

note that on the top, we're not seeing a blue line around the opening or the hole.

03:53

This is perfectly fine and this will allow us to finish off the entire top of that box

03:58

in the passes section. Make sure that we disable stock to leave. And we'll say, OK,

04:03

this will create our finishing tool path to finish both the faces of the different

04:07

parts of the caliper bracket as well as the side faces around the boss.

04:12

If you want to,

04:13

you can always use F seven to toggle on and off the tool path to get

04:16

a better idea of what areas have been machined and what have been left behind.

04:21

Now that we've finished off the outside and the inside,

04:24

we need to go back and drill the holes to do this.

04:27

We're gonna be using a drilling tool path with tool number one,

04:30

which is our spot drill.

04:32

So make sure that we go into our library,

04:33

select tool number one and then select the holes that we want to drill.

04:37

Remember that when selecting holes, there are multiple methods.

04:40

In this case, I'm selecting the inside faces.

04:43

And then when we move on to our height section,

04:45

we're going to be using the whole top instead of the

04:48

whole bottom because we are using a spot drilling operation.

04:52

When we're using a spot drill,

04:53

we also have the option to simply click drill tip through bottom.

04:56

If the holes are larger than the diameter of the spot drill,

04:59

this generally will be fine.

05:01

However,

05:01

we're gonna be tapping this hole here and we wanna

05:04

make sure that the spot drill is not too large.

05:07

Everything does look, OK.

05:08

So I'm gonna simply use that drill tip through bottom and say, ok,

05:13

next, we need to drill the holes.

05:14

And for this, I want to double check and measure the whole sizes.

05:18

In this case, you can see the diameter is 0.313.

05:21

And if I measure the diameter of this hole,

05:24

let's go ahead and see what this one comes in at 0.38.

05:28

So in order for us to drill and tap this, we need to have the appropriate drill size.

05:33

If we go back to drilling and we make our selections here.

05:37

Let's go back to our tool and see if we have that drill in our library.

05:41

We can see that we have a 2 57 which is not gonna be the appropriate size.

05:46

If we don't have the proper size drill bit,

05:48

we can always use N mills to get it to the proper size.

05:51

Or add additional tools to our tool library.

05:54

For this example, I am gonna be using the larger drill bit that I have available,

05:58

making sure I'm using aluminum drilling

06:01

and I wanna go ahead and add all the holes to this,

06:04

making sure that on the heights we do drill tip through bottom,

06:07

we're gonna add a small offset of 0.05

06:11

and set our drill cycle to be a chip breaking, which is going to be a partial retract,

06:17

we'll say, OK, and allow it to drill each of those.

06:21

Now,

06:21

we want to finish off those holes and as explored

06:23

before we can do this with various different tool paths.

06:26

For example, we could use a bore a two D pocket or even a two D contour.

06:31

For this example,

06:32

I'm gonna be using a two D contour with the quarter inch flat

06:35

end mill that we have in our tool library as tool number five

06:39

for the geometry. Let's go ahead and select the bottom of each of these holes.

06:46

And then we want to take a look at the way in which we're machining. This,

06:50

the heights are gonna go all the way down to the bottom of the selected contour,

06:53

but we want to go down just a little bit further.

06:56

Remember that we can use the model bottom, which will show the plane

06:60

and then we can have a negative value allowing us to go down just a little bit

07:03

further to make sure that we're not leaving a sharp corner on the bottom of our part

07:08

for our passes section.

07:09

We are going to be doing a finishing pass, but we wanna make sure that we use a ramp.

07:14

This will allow us to do a helical ramp in.

07:17

We can do pre drill positions if we want the tool to

07:20

go all the way down to the bottom of the hole.

07:22

If we've drilled it large enough.

07:23

In this case,

07:24

the difference between a quarter inch ML and the 0.257 drill is

07:28

a little too tight for me to feel comfortable doing that.

07:31

So I'm gonna allow it to ramp into the hole and

07:33

that's gonna be the way in which we make our cut

07:36

notice when we have this ramping motion

07:38

that we are starting the ramp relatively high

07:42

because these holes are at different heights,

07:44

the ramp height is gonna be based on the tallest one.

07:47

So in order to change that we can right click and edit our heights,

07:51

we can bring our height down just a little bit,

07:54

which will allow us to start the feed a little bit later.

07:57

Uh Keep in mind that this is going to be something

07:59

we need to be very careful with whenever we're creating tool paths

08:02

because we wanna make sure that it does start

08:05

high enough above the part that we don't begin

08:07

too late and just simply engage with a tool

08:09

that's not spinning or moving at the appropriate speed.

08:13

This tool path does produce a problem.

08:15

It's telling us that our lead in and lead outs were dropped due to constraints.

08:18

It simply means that there's not enough room for the lead in and lead out.

08:22

So we're using the helical entry and the tool is

08:24

getting pulled straight back out of the hole perfectly fine.

08:27

Again, in this instance,

08:28

because we are using that ramp down at two degrees to cut the geometry.

08:33

Next, we need to tap those holes.

08:35

And once again, if we have the appropriate size, it should be in our library.

08:38

If we go to our practical machining library, note that we have a quarter 20

08:43

this is not gonna be the appropriate size.

08:45

So we would need to go into the fusion 3 60 library and pick out the right tap.

08:50

We're gonna be using a right handed tap and notice

08:52

that quarter 20 is the only one listed here.

08:55

But once we go into our library and we take a look at the right handed taps,

08:59

we can see here that we've got the appropriate sizes.

09:03

You need to know what the tap is that you need to use. In this case, it's a 5 16, it's 18.

09:09

We're gonna select this,

09:10

this will automatically enable the tapping cycle. And we can say, OK,

09:14

now, in this case, it says that we didn't select any holes,

09:17

make sure that we do select the holes that we

09:18

want to tap and allow it to create that operation.

09:22

The last thing that we want to do is deeper the top edges and to do this,

09:26

we use a two D chan for tool path.

09:29

We need to have an appropriate tool.

09:30

So once again, back into our tool library, we're gonna select tool number two,

09:34

which is a chan for mill.

09:36

And then we simply need to select our geometry.

09:39

Now keep in mind when we make our selections

09:42

that the tool is going to be going around all

09:44

of these various edges that don't currently have a Chamfer.

09:48

This means that we need to come through and manually give

09:51

it a value that we want the champ with to be.

09:54

I'm gonna go ahead and leave all the other options

09:56

as default allowed to go through and create that deep

09:59

or that two D chamber

10:01

at this point, we have all of the various operations created.

10:05

Once again,

10:05

there is a warning because of lead in and lead out

10:08

if you want to clear that you can always go in and

10:10

manually remove the lead in and lead outs by disabling that check

10:14

box and that will remove the warning from the tool path.

10:17

The warnings don't necessarily mean that the operation is going to fail.

10:21

It just is letting us know a change

10:23

that was made based on our selections and parameters

10:26

at this point. Let's make sure that we simulate all these tool paths

10:29

just to make sure that we validate all the stock is being removed.

10:33

I'm gonna jump ahead one operation at a time, taking a look at our roughing finishing

10:39

and the holes

10:40

making sure that we are tapping the holes properly

10:43

coming through and doing our final.

10:46

If there are any problems with any of the tool paths now would

10:49

be a good time to check it and change it before creating any documentation

10:54

at this point. Let's go ahead and make sure that we do save this before moving on.