Finish details on a part

00:02

In this video, will finish details on a part.

00:05

After completing this step, you'll be able to use

00:14

In fusion 360, We want to carry on with our coupler for CNC mill so far, we've only added one tool path which is a 3D. adaptive clearing.

00:22

That allowed us to remove a lot of material from the part. However, we need to go back and we need to make some adjustments.

00:29

The original model had a small fill it in the bottom corner,

00:33

so we need to make sure that the axial stock to leave was enough to account for that, fill it.

00:38

So in our passes I'm going to go back to my stock to leave in the axial direction and add .015.

00:46

And in the radial direction I'll do .015 as well that allows us to leave enough material on the sides and the bottom of these bosses.

00:55

And that means that the tool can come through and it can add that fill it when we're using a bull nose mill.

01:01

The next thing that I need to do is finish off this face with that bull nose mill.

01:06

I can do this with a 2D Pocket tool path but first I need to select the tool.

01:12

Notice that tool number seven still has some cutting data errors. It's telling us that it's missing some required data.

01:18

So we need to go in and edit this tool under cutting data, we're going to go through each of these and see.

01:24

What information is missing.

01:26

You can see that it's missing the passes and linking information for a lot of these different cutting datas.

01:32

And that's because originally when we created this tool we went from a ball nose mill and we changed it to a bull nose mill.

01:40

Now these two different tools have different linking parameters.

01:44

So one thing that we can do is we can modify all these parameters or if this is problematic,

01:49

we can always go into the fusion 360 library and we can filter by milling and bull nose mill and find one that contains all of that data.

01:58

So what we're going to do is grab a quarter bull nose mill,

02:01

we're going to right click and copy the tool and go into our cam DFM and we're going to pace the tool.

02:06

I'm going to take the original one that has issues and I'm going to delete that and then I'm going to modify the bull nose mill we just copied.

02:14

First, I want to change it to tool number seven.

02:17

And next I'm going to go into my cutter data and I'm going to make it a four flute and make sure that the corner radius is .015.

02:25

We're going to say, okay and now we have tool number seven that allows us to use that cutting data that's already populated for us.

02:34

We're going to use it with aluminum finishing. And remember that our machine configuration has a max rpm of 12,000.

02:41

So this means that some of these are getting really close to that limit, but nothing has gone over the limit yet.

02:47

For a geometry for my 2D pocket, I'm going to select this face and I want to use stock contours and rest machining.

02:57

The tool that came before it was .25 with a corner radius of .125.

03:05

In the past is we're not leaving any stock, and we're going to say okay and allow it to machine that geometry,

03:11

noting that it is giving us an error, it's empty based on the rest machining tool path parameters.

03:18

It thinks that the material has all been removed,

03:21

because rest machining inside of a 2D operation is generally taking a look at areas where a tool could not get to.

03:28

So if we just say okay and allow it to generate this tool path, let's go ahead and take a look at the cutting moves.

03:35

It's machining this entire face,

03:36

it's going around all the bosses and it's using that to finish all the geometry,

03:42

over the opening because it thinks that that's already been machined and it's leaving the small, fill it around the corner,

03:49

so everything looks pretty good there and it's enabled us to get that geometry and that data that we need.

03:55

But now we need to finish off some additional areas.

03:58

We've got this boar here that goes all the way through and if we measure that we can see that it is .24,

04:05

it's relatively small and it might be easier for us to machine from the other side.

04:10

However, this boar has to be machined from this side as does this taper.

04:15

We also need to machine the outside so we need to consider what tools we have and when we want to perform these operations,

04:23

tool number five is a quarter in gen mill until number seven is a quarter inch bull nose.

04:28

Either will work just fine. However, I'm going to use the quarter inch animal to machine the outside before moving on to the inside.

04:36

We're going to do this with a 2D contour and I'm simply going to select this bottom edge.

04:42

And we're going to move on to our heights and instead of the selected contour, I wanted to come all the way down to this bottom face.

04:51

Inside of our passes, we need to make sure that we're not leaving any stock so make sure that that's turned off,

04:57

and all the rest of the settings will be as default.

04:59

This means that it's going to come down, it's going to make a single pass around the part and then it's going to retract.

05:06

Next we need to try to get into this boar,

05:09

we've already cleaned out some of the material and we know that it's large enough that we can go in with that quarter inch 10 mil.

05:15

So I'm going to go into a 2D bore using tool number five and then we want to select our geometry.

05:26

I'm going to use all the default settings allowing it to go in and clear that material out.

05:31

I do want to modify my 2D contour.

05:34

I'm going to edit and select a different tool, making sure that I am using tool number five.

05:40

And then we'll say okay allow it to regenerate and then we'll move our 2D. pocket which are bull nose end mill all the way to the end.

05:48

Keep in mind because some of these operations are model aware. It's going to take some time to recalculate.

05:55

So now we've got our 3D adaptive our 2D contour around the outside our bore on the inside and our

06:03

That cleans up this top face.

06:06

The next thing that we need to take care of is we need to take care of this taper.

06:10

The taper can be done with a bull nose mill or a ball end mill.

06:14

In this case we're going to use a 3D tool path called

06:19

and we're going to select a ball nose mill and we haven't created one in our library.

06:24

So we need to go into our filters and we need to filter by Bolland mill and we need to look for a ball and mill that's going to work.

06:32

In this case, I'm going to take a look at using a quarter inch ball in mill with aluminum finishing and select.

06:40

That's a rather large tool, so I need to be aware of how much room I actually have,

06:45

but let's go ahead and take a look at what geometry we can cut with this.

06:50

The machining boundary by default is going to be a silhouette but I want to contain the tool within this area.

06:57

I'm going to allow the tool to center on the boundary and I've got contact only selected.

07:02

We can also use a slope to limit the slope from anything that is above 1°.

07:10

And we want to go all the way up to 89°. This will prevent us from machining the flat faces or the vertical walls.

07:18

We're going to go into our past the section to make sure that we're not leaving anything,

07:22

and then we need to take a look at our maximum step down value.

07:26

This is going to be important as we want to make sure that we have a very small value in terms of the step over to replicate that face,

07:34

and I'm going to use .05. then I'm going to say Okay.

07:38

I'm going to allow it to generate the tool path, noting that the resolution is probably not fine enough for what we need.

07:45

So we're going to make some modifications to those settings.

07:49

Instead of the maximum step down of being .5, we're going to go to a .01.

08:00

And now we're getting a little bit closer to that final shape.

08:04

But let's note that it is going all the way into this pocket and we don't want it to machine that far.

08:10

So let's make a few more adjustments.

08:12

This time we're going to modify the height instead of the model bottom, we're going to use a selection which is going to be this edge.

08:19

And will allow it to go past that edge a small amount by putting a -0.1.

08:26

We'll say okay and this will contain the tool a little bit better allowing us to get a little bit closer to the final shape.

08:33

We could also use other types of tools.

08:36

We could come back with a smaller ball end mill or a bull nose mill,

08:40

or potentially even come in with a chance for mill that can cut that very quickly and easily depending on the requirements for that geometry.

08:48

Whether or not it needs to be that large of a champ for,

08:51

whether or not it has some sort of specific engineering requirement would determine what we would do in terms of its finishing geometry.

08:60

For this design, It's pretty much a cosmetic feature and it's not a requirement for engineering.

09:06

The last thing that I want to do is I want to come back and I want to chant for these upper edges.

09:11

We have to tool paths that will work for this,

09:13

we have a 2D contour and we have a 2D champ for the

09:19

because it allows us to actually set a physical distance requirement,

09:25

between the tool and other solid geometry to D champ for inside of a 2D contour works,

09:31

assuming you select a chance for tool,

09:34

we're going to go into our cam DFM library and select tool number nine,

09:38

and then we're going to select all the edges that we want to chance for,

09:42

these are going to be all the upper edges of these bosses and then we need to determine the champ for geometry in the past is section.

09:56

The tip offset is going to determine how far down the tool is going past the champ for,

10:02

and then the clearance is going to be between the tool and any other solid geometry,

10:06

which in our case is not going to be a problem, we're going to say, okay, allow it to generate and now we've champ erred those edges.

10:14

You'll note that there is a small amount of material that's been removed on top,

10:19

and really we need to go back to a simulation to make sure that this is okay,

10:23

but I'm going to go back in and make one small adjustment to the passes and I'm going to reduce the chance for with 2.01.

10:30

And I'm going to reduce the tip offset 2.01 and say, Okay,

10:34

this is going to put a much smaller champ for on the edge using a better portion of the tool.

10:42

At this point, let's make sure we save and then we want to take a look at one more aspect of these CNC programs.

10:48

Going to go back into my 3D adaptive and I want to take a look at the passes section.

10:54

When we modify values in the past is section we have a maximum roughing step down and when we modify this value,

10:60

the fine step down and the minimum step down both changed.

11:03

If we hold down the shift key and hover over those dialogues, we'll get a preview of the camp expressions that are used to define those.

11:11

We can also right click and edit the expression.

11:15

In this case, math dot minimum is going to take the smaller of the two values, the tool diameter times

11:25

So based on your tool diameter and based on the maximum step down value that is added here,

11:31

it's going to determine which value to use the same thing goes for the minimum step down unless we overwrite that value.

11:38

So by default, the minimum step down is going to be based on a fine step down times .1.

11:44

So it takes that .4 and you end up with .004.

11:49

KIM expressions are extremely handy and can help you set up your programs to run a little bit smoother,

11:55

and with more optimum settings based on your specific tools and machines.

12:00

Once again, let's make sure that we do save this before moving on to the next step.