Export NC Code for a CNC mill

00:02

export N C. Code for a CNC mill.

00:05

After completing this video, you'll be able to

00:08

export NC code for a single coordinate system with an appropriate post processor,

00:12

export NC code for multiple coordinate systems and identify code snippets

00:20

Infusion 3 60. Let's carry on with our mounting block ready to post.

00:24

At this point we're going to make a slight change to the op to set up.

00:28

We're going to activate it right click and edit

00:32

the first thing that we want to do is navigate to

00:34

the post process tab and set our wcs to G 55.

00:39

We're going to select OK. And note that we need to make sure that we double check our N.

00:44

C program. So let's right click and edit R N C program

00:48

by moving over to our operations. We can see the work offset is listed as a two.

00:53

In general. A work offset of zero or one is going to represent G 54 inside of our

00:58

controller and a work offset of two is going to represent G 55.

01:03

We're going to select OK. And I want to create one more N. C. Program.

01:08

This NC program is going to contain both.

01:10

Set up one and set up to we're going to select

01:13

op one and op two and notice that the work offsets.

01:16

One and two are displayed

01:19

when we have multiple work offsets.

01:20

We can also reorder to minimize tool changes which will change the order

01:24

in which the tools are used if multiple tools are used and we want

01:28

to machine both parts at the same time as can minimize the amount of

01:31

time spent moving back and forth between parts or by creating our tool changes

01:37

in the settings.

01:38

We want to make sure that we have an appropriate program number in this case. 10013.

01:43

And our comment will be both O P. S. Both ops

01:48

we're going to select OK. And now we've created a new NC program.

01:52

I'm going to call this one both O P. S for both.

01:55

Ops when we're posting code from fusion 3 60 we can

01:59

post code for a single tool path for multiple tool paths,

02:03

an entire set up.

02:04

Or we can post it for everything in an NC program.

02:08

If we select op one in this case and right click, we can select the option to post.

02:13

Process.

02:14

This is going to open up and create a new NC. Program.

02:17

You can c n c program for has been created in RNC programs folder.

02:20

So if you're using NC programs that you've already created,

02:23

it's a good idea for you to select those right click and select post process.

02:28

This will prevent you from creating a secondary

02:31

NC program that is only using the same data

02:35

in this case. My NC program and G code will open up in visual studio code.

02:40

If you have a different post editor, then it will likely open up in that for you

02:45

in this case note that we have program 10011 with a comment sir.

02:50

Prep We didn't rename any of our tool paths.

02:53

So they're coming up with their default names. Phase two to the adaptive one and so on

02:58

at the very top of our program.

02:60

Note that the comments are listed with brackets and we can see the

03:04

tools that are being used as we go down inside of our code.

03:07

We can see that the first operation Phase two is using tool

03:11

number four and using the M code invoking a tool change.

03:14

Then it's starting the spindle at 5000 rpm and it's referencing G 50 for it's

03:21

also turning the coolant on and then it begins its motion to face our part.

03:25

I'm going to go ahead and close out this NC program

03:28

then I want to move on to the one for both.

03:30

Ops

03:31

if I right click and use the post process option.

03:34

Note that we get an info or warning that tells

03:37

us this has multiple setups with different WCS settings.

03:40

This is important because not all machines can handle this,

03:43

but in this case I'm going to go ahead and say okay and post the code.

03:48

Now you can see at the very top it looks the same.

03:50

We are posting both ops and we have a different program number but we are using

03:55

the same tools and it begins with Phase two and G 54 is being referenced.

03:59

However, if we want to find G 55 in the code.

04:03

I'm going to use my fine dialogue and I'm going to type in G 55.

04:08

Note that the two D contour on the opposite side of the part is referencing G 55.

04:13

If we go down through the list,

04:14

the second instances are adaptive tool path and then R two D chant for

04:19

Those are a few of the tool paths on the backside of our part during op two.

04:23

So note that posting the code for both operations

04:27

allowed us to create an NC file or G code

04:30

that references both G- 54 and G- 55 allowing us

04:34

to set up multiple parts in a single machine.

04:37

It's also important to note that the symbols next to

04:39

RNC programs inside of our browser will change up.

04:43

One has been posted so now it's valid but op two is still out of date

04:47

in order to ensure that this is valid.

04:49

We need to post process once we post process that will recalculate

04:53

everything and back in fusion 3 60 it is now valid.

04:58

The warning triangle tells us that this uses multiple offsets

05:01

as warning is going to stay even if we were to post the code.

05:06

So remember that the green check mark tells us that the NC

05:09

program is valid if it has an orange circle with an arrow.

05:12

This tells us that it's out of date doesn't

05:14

necessarily mean that there is a problem with the

05:16

NC program just that it hasn't been posted since

05:19

a change has been made to the program,

05:21

and a yellow triangle with a caution sign is telling

05:24

us that multiple work offsets are used in this program.

05:28

We can still post all of these out to G code,

05:31

but just keep in mind that those symbols do

05:33

mean something has to happen with your NC program.

05:36

At this point,

05:37

let's make sure that we do save this document

05:39

before moving on to the practices and challenges.