Use a 3D parallel toolpath

00:02

In this video, we'll use a 3D parallel tool path.

00:06

After completing this step, you'll be able to create a 3D parallel tool path.

00:12

In fusion 360, we want to carry on with our coupler for CNC Mill design.

00:17

We're going to rotate the part and we want to go back into our model and we want to bring back our generic vice and the other couplers.

00:25

We're going to rotate this around back to a home view,

00:28

and then we're going to look at machining the other side of the part and talk about ways in which we can pattern these tool paths.

00:35

At this point, we need to create a new setup.

00:38

The new setup is not going to include the Vice.

00:40

We're going to make sure that we focus our attention solely on that first model.

00:45

We also do want to include the fixture as the soft jaws to make sure that we do some collision validation in simulation.

00:53

The coordinate system is okay.

00:55

However, we're going to reference it based off of the corner of the Vice.

01:01

When we're talking about patterning, we need a good reference and we know the corner of this Vice because we machined this geometry.

01:08

So for the corner point instead of using a box point,

01:11

we're going to use a selected point, we're going to set the WCS origin to that corner point of the Vice.

01:19

The next thing that we need to talk about is the stock.

01:21

We've already machined some geometry from the other side,

01:25

but we're going to be using a fixed size stock and notice that we have ground stock at model origin.

01:32

We're not going to do that, We're going to focus its attention around the part,

01:36

and we're going to set it up just like we did in the first operation 1.75 x 1.75.

01:43

And for the height we're going to do one but remember we're going to subtract .067 inches.

01:49

The reason that we're doing that is because we accounted for the overall height of the final part at .866.

01:58

Whenever we're using mathematical operators we need to include the units for each value.

02:03

So it needs to be 1 inch -167 inches.

02:08

That value right now is based on center but we want to make sure that we offset it from Z.

02:14

We can offset it from the bottom and we can set that offset value at zero.

02:21

That means that it's going to be completely set to the bottom of the part and we're only going to be offsetting .06 on the top of the part.

02:30

As we look at it here you can see that it completely matches the bottom and we're only offsetting on the top.

02:35

Remember that we did machine up past this champ for and we'll have to keep that in mind when we're creating our tool paths,

02:41

let's go back to home view and take a look at our post processing.

02:45

We're going to set this one up as program 1006 and we'll set it up as our coupler O.P.2.

02:56

The W. C. S we're gonna be using is number one or G. 54.

03:01

We're going to be assuming that when we flip the part over and put it in the soft jaw were only accounting for these three positions of the second up.

03:09

We also want to make sure that we rename set up to and this is going to be opt to.

03:15

With up to active, we need to talk about what tool pass we're going to use to clear this geometry.

03:21

To get started, let's take a look at 3D tool paths and try to figure out which one would be a good option.

03:26

We have a large tapered surface and we have some small Phillips that we need to account for.

03:31

We have both internal and external Phillips, a tapered face and champers.

03:36

When we look at some of the options it can be a little bit hard to select,

03:40

and it's going to take some trial and error and practice to be able to pick the right tool path first.

03:46

But let's explore what we have and see if parallel is going to be a good option for us.

03:51

Right now the tool selected as a champ for mill. So we need to go back in and maybe try to use a ball end mill.

03:58

I do want to edit this tool and make it tool number

04:03

This is the tool that we added and we want to make sure that we don't overlap any other tools in our tool library.

04:09

So now that we have our ball end mill, let's take a look at aluminum roughing and let's take a look at our geometry.

04:17

By default, it's based on a silhouette, which is going to be based on the outside of the part.

04:22

We also want to make sure that we allow it to use rest machining anytime we're using the stock setup.

04:30

So we're going to make it go from stock and we're going to say, okay and just see what the tool path gives us.

04:36

You can see that this is not an ideal situation.

04:39

Even if we modify the parameters to get a finer resolution, this is not the correct tool or tool path to get started on this part.

04:48

Because of that, we're going to right click and we'll delete parallel,

04:51

and we'll get started by using a 3D adaptive clearing to get rid of the majority of the material,

04:56

and we'll go back and use a quarter inch flat end mill with aluminum roughing.

05:01

When we do this and go to the geometry section will be using stock contour and rest machining from stock setup.

05:08

In the heights, we want to make sure that we're not going all the way to the bottom of the part.

05:13

So we need to use a selection.

05:15

In this case, I'm going to go down to this edge,

05:18

because I know I've machined all the material up to the top of this champ for, I know that's going to be a good reference for me.

05:25

In the past is we are going to have stock to leave,

05:28

so we're going to leave those values that .02 and we're going to leave all the rest of the default settings.

05:34

With the exception of the maximum roughing step down With this quarter in gen mills,

05:39

I could take it the full flute depth but I'm going to reduce that 2.04 and I'm going to use flat area detection again,

05:46

so that way you can find this flat and machine fairly close.

05:52

Whenever we're using 3D adaptive clearing.

05:54

This is a great tool path because it works its way down with those maximum steps,

05:60

and then it uses those smaller step values to work its way back up the part getting us relatively close to the final shape,

06:07

so you can see that this is a pretty good result for a first tool path.

06:11

And with our new set up, it was a great time for us to save before moving on to the next step.