Create toolpath patterns

00:02

In this video, will create a toolpath pattern.

00:06

After completing this step, you'll be able to create a toolpath pattern and modify a pattern posting order.

00:13

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

00:18

The next thing that we want to talk about since we've created all of our operations to machine,

00:23

the second side of our part is how we can pattern these operations to machine all three parts at once.

00:29

The first thing that I want to do is inspect the distance between these on our vice.

00:34

You'll notice that the center to center distance is going to be 2 inches.

00:38

This allows me to get a good understanding of how far apart each of our toolpaths are another thing that we need to consider,

00:46

when we're talking about our toolpaths are going to be the entry and exit positions.

00:51

So when we talk about our leads and our links, especially for things like 2D contour,

00:56

we want to make sure that they're entering from the vice side and not in between.

01:00

When they enter from in between.

01:02

We need to be careful that the tool itself isn't going to intersect the other part on the vice.

01:08

So as we look through the toolpaths, we want to make sure that we identify where they enter and exit.

01:14

The second 2D. Contour in this case, 2D. Contour three is entering from the side,

01:17

and if we want to modify that we can edit the toolpath,

01:21

go to its linking parameters and we can actually pick an entry position to pick an entry position.

01:28

I'm just going to pick a position that's in roughly the Y direction and say okay, and allow it to regenerate.

01:35

This now means that the tool enters and exits from the vice side which is much safer,

01:40

especially when we're talking about patterning.

01:42

In order for us to pattern everything I'm going to start by selecting all the toolpaths in the setup.

01:49

Then I'm going to go to the setup folder and select new pattern.

01:53

The new pattern is going to take all my selected toolpaths and then I can determine whether it's linear, circular, mirror duplication or component.

02:02

In our case it's going to be linear and we need to determine the direction.

02:07

I can select one of the edges on my Vice and then I can determine the spacing for direction.

02:13

When I select 2 inches, I might need to flip the direction and increase the number of instances but we should see everything line up on the vice.

02:21

We also have the option to order by tool.

02:25

Order by operation or preserve order by tool can be handy because it saves us from having a bunch of tool changes,

02:32

when we are machining three parts at the same time,

02:35

we have some post process options that allow us to override the wcs offset.

02:41

What this allows us to do is it takes the wcs offset in the setup in this case, one which is G 54 lets us pick another one.

02:51

In our case, that's not going to be helpful because we still need to make sure that we're referencing the same coordinate system.

02:57

So when I say, okay, it's going to create that toolpath pattern.

03:01

When I do that and I expand the linear pattern folder, notice that we have all the different patterns inside of here.

03:09

What I want to do is I want to select that linear pattern and go to simulate,

03:14

notice that inside of here our stock is not shown in the other two positions,

03:19

but the toolpaths are using that same tool and then it's going to move to the secondary position.

03:25

So assuming that the part itself has all of the operations machining the stock in the first position,

03:31

everything will be fine in the 2nd and 3rd.

03:33

As long as we've accounted for those overlaps between the tools.

03:38

You can see again, it's moving based on the tool numbers and everything is ordered properly.

03:46

There are other ways in which we can do this.

03:48

But what I want to do at this point is I want to save this and then I'm going to use undo to undo my linear pattern.

03:57

The reason that I want to undo the linear pattern is because it consumes all the toolpaths that we created.

04:03

When I consume all those tool pass,

04:05

what I'm actually doing is I'm creating that linear pattern and everything else is nested underneath while we can still pull them back out.

04:13

Because we're going to explore other options for patterning. I wanted to make sure that I used undue after I saved that version.

04:20

Now, let's make a save of this version and then let's move on to the next step.