Export NC files

00:02

In this video, will export NC Files.

00:05

After completing this step, you'll be able to create an NC. Program.

00:09

Review an NC file and create a setup sheet.

00:14

In fusion 360, we want to carry on with our gear housing for CNC milk.

00:18

At this point we've created all the tool paths in our op one and op two setups.

00:23

We've used the fixture in the second operation and we've removed all the material starting from the back side of the part where we faced,

00:31

did a 2D contour drilled and tapped and then we flip the part over holding it in the fixture.

00:37

Now we want to create some sort of NC file that will take these tool paths and convert them to something our machine can use.

00:45

In order to do that. I'm going to start by creating what's called an NC program.

00:49

It's important to note that there are currently two methods to get this NC file out of fusion 360.

00:56

NC program, as well as in the actions we have something called post process.

01:01

There are some benefits to using NC program. So this is the option that we're going to choose.

01:06

I'm going to start by selecting, create NC program.

01:10

Notice that we have a program name number automatically comes in at 1001, because this is the op one that we currently have selected.

01:19

The comment has not come through. So we want to make sure that we do have a year housing up one as our comment.

01:28

We need to determine what machine we want to use and I'm going to start by going into the capabilities and selecting just milling.

01:35

I then need to filter by vendor. I can also just search for one or take a look at ones that I have saved locally for this example.

01:44

We're going to be using Haas automation and we're going to take a look at all the various posts that are available to us.

01:50

We have a hose pre NGC, which is the next gen controller and then you'll notice that we have a UMC 750,

01:58

which is a five axis machine we have Next gen which has inspection.

02:03

We're going to use this one that's called us Next gen control.

02:07

This house Next end control is the newer controller and will give us access to some of the newer features such as dynamic work offsets.

02:16

We're not going to be using this for our example or TCPC which is tools center point control.

02:22

This is generally used from multi axis tool baths.

02:25

So with those options turned off we're going to navigate to the operations tap in the operations tab.

02:31

We can select individual tool paths, entire setups or we can select everything.

02:37

Notice that when we select both op one and op to it shows us the work offset of one for op one and zero for up two.

02:46

Now infusion 360 setups, these are both referencing G 54 this is going to produce a warning anytime we use zero as a work offset.

02:55

That's going to produce a warning in the NC program For this NC program.

02:60

I'm only going to focus on using op one and I'm going to say Okay.

03:04

When I say okay, this creates an NC program that's inside of the browser.

03:09

I want to go into op too and I want to edit that set up for my Wcs offset.

03:16

I'm going to set this up as number two. This is going to be a G 55.

03:21

Now, this is helpful if we're machining multiple parts and we have both sides of the part available in a single machine.

03:28

For example, if your machining op one on 1 part and opt to on a second part.

03:33

Now that I have NC program one, I'm going to rename this 1000 and one and then I'm going to create a new NC program.

03:42

This new NC program is going to be 1002 and it's going to be called my gear housing Op2.

03:52

Once again, I want to make sure that I am using the same next gen controller,

03:56

and you'll notice that it's already pre selected for us in any settings that we changed,

04:01

are currently deselected or selected based on our last NC program.

04:07

In the operations, I'm going to select all of up to which is giving me my work offset. Going to say, okay.

04:15

And I'm going to rename this as 1002.

04:19

Now that I have my second NC program. Let's go ahead and just create one more.

04:26

I'm going to call this 1003. This is going to be a program that captures both of my setups.

04:33

I'm going to move on to operations and I'm going to select op one and up to showing that I have two different work offsets and I'm going to say Okay.

04:42

I'm going to rename this as 1003. And now I have three different NC programs.

04:48

When I select each of these, I have a few different options,

04:51

I can right click and I can post process them which will give me the G code or the NC file that I can take to my machine.

04:58

I can create a setup sheet or I can even simulate.

05:02

If I select 1003 which includes both setups and simulate and I jump all the way to the end.

05:08

You can see that this gives us the results of simulating all of the tool path we created.

05:14

If I instead simulate 1002, I'm only taking a look at the second set of operations,

05:21

notice that this allows me to go through and it allows me to validate those operations,

05:26

and I can see that there is actually a tool collision here I need to be worried about.

05:32

What it's telling me is that I'm actually colliding with my fixture in this setup.

05:37

If I hide the stock and if I even expand this and I hide my front cover, you can see that the tool is actually intersecting with my fixture.

05:48

In some cases, this might actually be okay allowing it to clearance the fixture as it goes.

05:53

But it's probably something that we would want to account for the time we design and create that fixture,

05:58

because we know that we have a board that goes through the park.

06:01

This is something that we wouldn't catch if we're simulating both setups at the same time.

06:07

But now that we've taken a look at this, let's go ahead and let's post 1001.

06:12

We're going to right click and select post process.

06:15

If you already have an NC file that has that name in your temp directory, then it's going to ask you if you want to overwrite.

06:22

If I say no, it'll aboard the process.

06:25

If we edit the NC program in the settings tab, you can determine where you want the output to go.

06:31

By default, it's going to be in your local fusion

06:36

If you want to point it to a specific location, you can do that and you can even post it to fusion team, selecting a specific folder.

06:44

I'm not going to be posting this to team and I am just going to overwrite the 1001 that I have.

06:49

It's sort of a throwaway number that I use whenever I'm creating these files.

06:56

Once the NC file has been posted, it's going to open up in whichever code editor you've determined inside of your user preferences.

07:04

If you haven't set one up, sometimes this opens up in a text editor. In my case, it opens up in visual studio code.

07:12

Anywhere, it opens up is fine as ultimately it's just a text file. But there are some benefits to using text editors.

07:19

If you have a specific NC code editor,

07:22

it'll do things like highlight the X, Y and Z values in various colors to make it easy to see excess or red value.

07:29

Why as a green value and Z as a blue value, it will also change whether or not they're bold based on if they're positive or negative.

07:37

So various things like this can be helpful about using a specific NC editor, but again, it's not required.

07:43

So we're only taking a look at this in visual studio code.

07:47

What we want to be aware of is that our program name or number is at the top are comment gear housing up one is here,

07:54

and it's giving us some comments based on some of the settings and RNC program, we're using high feed G one instead of G zero,

08:02

you'll notice the tools that we're using and then it begins the program calling our first tool change,

08:07

which is are facing tool setting up to spindle speed and referencing our G 54 coordinate system,

08:13

as it goes to each operation, you'll notice it calls its tool change.

08:17

It's turning on and off the spindle and it's referencing our coordinate system.

08:22

Let's go ahead and let's post 1003.

08:26

When we post process 1003 because it has multiple WCS settings, note that it gives us a warning.

08:34

The post must be customized to handle that and we need to be careful of things like tool clearance between parts and fixtures.

08:41

But as we open this code, you'll notice that are facing operation is still referencing G 54 as is our 2D contour.

08:50

But let's go ahead and let's use our control f or command f to find G 55.

08:57

Notice that our second facing operation is referencing G55 as well as the to the adaptive are drilling operations,

09:07

and any subsequent operations that were in that second op.

09:10

So everything here makes sense.

09:12

And if we are able to post code for 1001 and 1002 at the same time and run both parts on the same mill because we are using the same set of tools.

09:22

This can simplify the manufacturing process.

09:25

We could go a step further and we could minimize the tool changes between both of those by allowing it to jump,

09:33

between each using that same tool and minimizing those tool changes further.

09:38

This can be done by taking a look at the N.C. file and reordering to minimize tool changes.

09:45

If we do that, we'll take a look and note that face one and face two happen directly after each other even though they have different work offsets,

09:53

it's going to post them out in that order.

09:55

Then it goes to our 2D. Contour.

09:57

Which is using our half inch flat and then it jumps to our to the adaptive and too deep pocket goes to our drilling operations.

10:05

Ultimately it goes back to our 2D pocket, our 2D bore and all the ones that we're using to finish up to.

10:13

But keep in mind that reorder to minimize tool changes is extremely handy,

10:17

especially if you have multiple parts lined up and you want to machine them all at the same time.

10:22

At this point let's make sure that we save the design and we want to focus on the last step which is creating a setup sheet.

10:29

We're going to make a setup sheet for 1003 and this is going to be placed in a project location inside of your data panel.

10:36

Once we select, save the new setup sheet begins to be created.

10:40

Notice that we're creating a detailed set up sheet but we have other options such as tools only or compact.

10:47

Some of these will allow us to make some changes but inside of here we have critical information such as the number of setups,

10:54

the number of operations, the tools that are being used and as we go down we can see the specific tools, their parameters and even their values,

11:02

such as how far the tool is sticking out from the holder.

11:06

As we go through here, you'll notice that the bottom we have information about the setup, the stock size the WCS locations.

11:13

And then, information about all the parameters of each tool path.

11:17

So this is great information and this will be saved directly inside of your data panel and you can also print this out,

11:24

so you can hand it to a machine operator.

11:26

At this point, no additional saves need to be made, since that does not require any additional save so we can go ahead and move on to the next steps.