Deburr and Simulate

00:02

Deeper and simulate.

00:05

After completing this video, you'll be able to create a two D champ for operation

00:09

and use simulation to verify stock removal

00:14

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

00:18

At this stage,

00:19

we've machined everything from operation one side including the adaptive,

00:24

the two D contour for the outside two D pocket to semifinish the bore,

00:28

a bore tool path to finish it

00:30

two D pocket to finish off all the flat faces.

00:33

A two D contour to finish off our rotor relief area with a bullnose mill,

00:38

our drilling operations as well as our final bore to

00:41

get the full size of that one mounting hole.

00:44

Now,

00:44

a couple of things that we need to consider at this 0.1 is going to

00:48

be all of the tool paths and the order in which we chose to do them

00:52

is based on the tool that was being used.

00:55

For example,

00:56

the two D contour to finish off the rotor

00:58

relief area was a different tool tool number eight.

01:01

So it was done after all the operations that required tool number seven,

01:05

the drilling happened before we moved on to doing the

01:08

two D board to finish off that final size.

01:11

Because once again, this was another tool change,

01:14

different machines will be able to change tools at different speeds.

01:17

Sometimes the tool change in the middle of an operation is not a big deal.

01:22

However,

01:23

if you can organize your operations and the way in

01:25

which you machine your parts based on those tool changes,

01:28

oftentimes, it will speed up the overall process,

01:31

especially if you have a lot of different tools in use.

01:35

The next thing that we need to do is we need to deeper

01:38

edges on the part because right now everything has an extremely sharp corner.

01:42

Oftentimes a detailed drawing might say break all edges or deeper

01:46

sharp corners

01:48

or there might even be a specified champ for value that it needs on all these corners.

01:53

In our case,

01:54

we are just going to be using a very small chamber to break or deeper all the edges.

01:59

This can be done a couple of different ways. Fusion 3 60 has a 3d tool path called deer

02:05

that's inside of the manage extension.

02:07

This allows us to create a finishing strategy that will deer

02:10

external corners with sharps or rounded edges.

02:14

Now, it's important to note that this can be done on three axis parts,

02:18

but it can also be done in four and five axis.

02:21

However, we're gonna be focusing on again,

02:27

in this case, we can use a two D contour or we can use the two D champ tool path.

02:32

There are some benefits to using two D chamfer over two D contour.

02:36

But two D contour when used with a champ

02:39

or an engraving tool will allow us to have the options to get this done.

02:43

The main benefit to us using a two D

02:46

chand tool path

02:47

is that it allows us to do a little bit of collision checking

02:51

or at least keeping clearance values between our tool and the part.

02:54

This is especially important around this edge here because we

02:58

have a very small overlap 0.025 between those two.

03:03

The first thing that we need to do is we need to select an appropriate tool.

03:07

Now, whenever you're selecting tools,

03:09

it's important to remember that we're pulling from

03:11

a tool library directly into our document.

03:14

You always want to make sure that you're

03:16

using the tools in your document before going

03:18

to a tool library because otherwise you'll end

03:21

up with duplicates that have the same tool number

03:24

for this. We need to make sure that we are using tool number two.

03:28

So we're gonna go into our tool library, select tool number two,

03:31

which is going to be our 90 degree carbide

03:34

cham

03:34

Mll.

03:35

We're gonna select this and then we're gonna move

03:37

on to our geometry to make our selections.

03:40

We can use this to deer,

03:41

all the edges on our part.

03:43

But there are going to be some limitations, for example, these vertical edges,

03:48

we're going to avoid those, but we are gonna focus on some of these edges.

03:52

So let's start at the very top, selecting the edges that we wanna champ for

03:56

moving our way down

03:58

and then selecting all of the various edges that

04:01

are going to be important for us to deer,

04:05

gonna move our way back around here

04:07

and finish off with this backside.

04:09

Once we have all of these edges selected,

04:12

we're gonna make sure that we take a look at the heights,

04:15

but these are all gonna be based on our selected contour.

04:18

As long as your clearance and feed heights are fine.

04:20

Go ahead and move on to the passes section.

04:23

This is where we're going to define our chan.

04:25

If we have a model that already contains a champ,

04:28

something that is in the design already,

04:31

the champ with value is gonna be zero.

04:33

However, in this case,

04:35

we're selecting sharp corners and we're using this to deeper after the fact,

04:39

which means that we need to enter a value,

04:41

we're gonna enter a value of 0.02.

04:44

The chan for tip offset is gonna determine how far

04:47

down on that champ for mill we're gonna be using.

04:50

So you need to know the geometry that you're using.

04:52

In our case, we're going to increase this 2.1.

04:55

And the reason for this is because the farther up that chan for MLL,

04:59

we end up using,

05:00

it's going to affect things like the forces the speed of the tool across the part

05:06

as well as how much clearance we can have or how tight we can get up to other geometry,

05:11

which brings me to the last setting, the clearance.

05:14

And remember we have 0.025 between the small edge

05:18

and the little shelf here between these two parts.

05:21

So if I leave the champ for clearance at 0.025 and the tip off set isn't large

05:26

enough so that we're all the way at the very edge of that champ for mill,

05:29

we're not gonna be able to cut around the backside of the part.

05:32

So I'm gonna reduce this clearance to 0.0125 which is extremely small,

05:37

but will give us enough of a clearance value to ensure

05:40

that we can transfer all the way around the park.

05:43

So as we take a look,

05:45

we can see that there is a small section here where we are not able to get our chamfer.

05:50

So once again,

05:51

that clearance value is important because it's gonna determine whether or

05:56

not we can chamfer all the way around the model.

05:58

We need to make some adjustments.

05:60

And the first thing that we want to do is take a look at the tool itself.

06:03

So I'm gonna take a look at the tool. I'm gonna say edit tool.

06:07

We're not gonna make any changes but we want to

06:09

take a look at the geometry of the cutter.

06:12

Inside of here,

06:13

we can see that the various areas when we

06:15

click on them will highlight on the tool display.

06:18

As we take a look at the shoulder length, the flute length and the taper angle.

06:23

All of these are going to affect how much we can cut. Point.

06:28

which means that we can increase that tip offset value slightly

06:33

without getting all the way to the edge of the tool.

06:36

If we edit this,

06:37

the two options we have are to decrease the

06:40

champ for clearance or increase the chan for tip offset

06:43

because I know I have 0.125 to go all the way to the edge of the tool.

06:48

I'm gonna increase this to 0.11 we never want to

06:51

ride all the way at the edge if possible.

06:53

So we're gonna say, OK, and allow it to rebuild.

06:56

Now, we can see the chan for operation is going all the way around the part.

06:60

So now we're getting that full de

07:03

if this chamfer is too large, we can always go back in and make an adjustment

07:08

notice that we are getting a warning and this

07:10

tells us that the contour is not machined,

07:12

giving the lead parameters.

07:15

So somewhere in this tool path, there is a problem with the lead parameters.

07:19

This could be potentially on the back side

07:22

and this is something also that we can make an adjustment on.

07:25

So let's make one more change to this tool path before we simulate,

07:29

we're gonna go into our passes. We're gonna reduce the chance for clearance to 0.12.

07:35

We are going to decrease the champ for width to 0.01.

07:40

And then we're gonna go into our leads and links

07:43

and we're gonna change the linear lead and value to 0.02 and say OK,

07:48

and allow it to regenerate.

07:50

It's still telling us that there is a problem somewhere with a lead in parameter.

07:55

It's likely going to be inside of this hole because of how deep we're taking the tool.

07:59

But this just means that it's defaulting to a smaller value,

08:03

which is perfectly fine.

08:04

In this case,

08:05

once again, we're using a relatively small value.

08:08

But all we're trying to do is break those sharp edges on the part.

08:12

Now that we have all of the tool paths created,

08:15

I'm going to click on the activate button again to go back to the top level of my setup.

08:20

Then I'm gonna go to actions and simulate

08:23

we've been looking at in process stock this entire time.

08:26

But simulate is the next step for us to validate our tool paths.

08:29

A couple of different ways that we can do.

08:31

This is one by holding down the left mouse button

08:34

and manually dragging across the screen.

08:36

This will allow us to manually navigate through the points of the simulation.

08:41

We can also click at the bottom

08:44

and jump ahead to different parts in the tool path.

08:47

You'll notice that there are some color changes at the bottom,

08:50

which may be kind of hard to see.

08:51

But this happens when we go between different operations.

08:54

This first operation, our 3D adaptive is taking up the majority of our time.

08:59

You can see that it takes about six minutes to machine.

09:02

When we jump ahead to our two D contour, the two D contour is relatively quick.

09:07

In relation to the adaptive,

09:09

we can also change the speed and play through to see it machining in real time.

09:15

We're using a stock comparison in the display options which allows

09:19

us to see blue where stock is still remaining green.

09:23

When we've reached the appropriate stock in this case or red.

09:27

If we've removed too much material,

09:29

we're going to see red any time we use the two D champ

09:32

to de

09:33

simply because those were not in the model.

09:36

And in this case,

09:37

it's going to assume that we've gouged or removed too much material.

09:41

Any time there is a red collision, we will be able to also see it at the bottom.

09:46

I'm gonna increase the speed so we can play through

09:49

and we just wanna make sure that the final result is as intended,

09:53

everything looks pretty good so far

09:56

because the chamfer or

09:57

deeper is relatively small.

09:59

You can see that it is actually not displaying

10:01

red likely because it's within that 0.01 tolerance.

10:05

Another thing that we can do is we can change the tolerance value that we see here.

10:10

For example, there's a leftover stock option and a tolerance option.

10:13

When we're using stock compare.

10:15

If you want it to be within a specified tolerance,

10:17

you can change these values and rerun your simulation.

10:20

As we look at the part, everything appears good.

10:23

But remember that we are looking at the model here.

10:26

So if you want to hide the models and just take a look at the stock,

10:29

we can see that it looks like there

10:31

may be some potential problems with that deeper operation

10:34

because of where we're using it on the tool.

10:37

So this tells me that I likely want

10:39

to make some adjustments or changes to our geometry

10:43

to see this. I'm gonna hop back one operation

10:47

and then I want to manually drag through this deer

10:51

and I want to identify where we're using this on the tool.

10:54

Now, even though we had the tool specified at a specific amount,

10:59

you can see that our chan for mill is riding way too low.

11:02

And this is a problem that we really only were

11:04

able to identify by taking a look at the simulation.

11:07

So I'm gonna bring the model back and I'm going to

11:09

exit the simulation and make an edit to this tool path.

11:13

I'm gonna go back to my parameters. I'm gonna reset my chan

11:17

tip offset to 0.1

11:19

and the chance for width, I'm gonna increase it to 0.2.

11:23

And then I want to rerun the simulation.

11:26

Let's go ahead and select all of

11:27

one,

11:29

go to simulate

11:30

this time. We're gonna use the go to end of tool path

11:33

and then we're gonna jump back one operation.

11:37

Let's go ahead and rotate this around

11:39

and begin dragging through and just see where we are on the tool

11:43

once more,

11:43

it just appears that we're too low on the tool to get the appropriate chamfer.

11:48

So we really need to change that tip offset to something that's small enough.

11:52

And this is where understanding the geometry of the tool that you're using and

11:55

how it's defined digitally as well as in the real world is extremely important.

12:01

So we're gonna change our chamber tip offset to 0.08.

12:05

I'm gonna go ahead and reduce that with back down to 0.01

12:09

say OK, and simulate this all one more time.

12:13

So once again, under actions and simulate jump all the way to the end

12:18

and then we'll jump back one operation

12:20

and manually go ahead and pull this through and just make sure

12:24

that we're at an appropriate place on our chan for mill.

12:27

This looks like a much better solution.

12:30

This means that we're no longer hitting the tool too high, which in reality,

12:34

that would be a non cutting portion of this tool.

12:37

And obviously it would cause some problems.

12:39

A couple of other things that we can get out of simulation would be

12:43

understanding what stock is left over when we go to flip the part over,

12:47

as well as information about the tool path itself.

12:50

For example, under information, we can see spindle feed rate,

12:54

which operation we're on

12:56

verification machine information,

12:58

as well as statistics for the overall machining time

13:01

based on our current feeds and speeds.

13:04

The number of operations we have,

13:06

it's gonna take under 12 minutes to machine the first operations.

13:10

This means that we've got six tool changes, 11 total operations.

13:14

But we're moving at a fast and efficient rate.

13:17

Now, with all of this information, it's time to move on to the next step.

13:20

But let's make sure that we go back to our name, view and save this before moving on.