& Construction

Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
& Manufacturing

Professional CAD/CAM tools built on Inventor and AutoCAD
Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
Professional CAD/CAM tools built on Inventor and AutoCAD
Transcript
00:02
create cam documentation
00:06
in this video. We'll create an NC. Program and will create a setup sheet.
00:12
Infusion 3 60. Let's carry on with our engine case, Rh ready to program.
00:17
Now in this case we've created four operations.
00:21
We've got op one, op two, op three and up four.
00:25
Each of these are machines at different times
00:27
in the same vice using different sized parallels.
00:30
So a couple things that we need to do is we need to account
00:33
for notes that need to be displayed in what's called a setup sheet.
00:37
The easiest way for us to do this is to
00:39
create notes in individual operations or the tool paths themselves.
00:44
So first let's go ahead and take a look at op one.
00:48
The first thing to note about op one is that we use a specific size parallel a 1.375.
00:55
So I want to make sure that that notes included in our setup sheet.
00:58
So I'm going to right click on op one and I'm gonna select edit notes inside of here.
01:04
We're gonna say T. Y. P. For typical vice. 1.75 inch tall jaw
01:13
With our 1.375" parallels.
01:19
Once we say okay we're going to have a note icon that displays and
01:23
when we hover the cursor over it we can see what that note is.
01:26
More importantly that note gets displayed on our setup sheet.
01:30
Now you can do the same thing with any of the operations as well.
01:34
For example if we look down through here and we have a spot we
01:38
can right click and we can select edit notes for the spot drill.
01:43
We want to make sure not to go too deep.
01:46
So we're gonna say don't spot drill too deep.
01:51
So the notes can be very specific about the setup,
01:54
for example using a certain size parallel or it can be notes of
01:58
caution or maybe adjustments that could be made to the tool path.
02:02
Now these are going to be at the operation or
02:05
set up level and the individual tool path level.
02:08
We can go through and we can make notes on every tool path and every operation.
02:13
But I think this gets the point across from here.
02:16
The next thing that we want to do is we want to create something called an NC program.
02:21
When we go to the set up drop down. We have create N. C. Program
02:25
and
02:26
programs are a way for us to group tool
02:28
paths together in multiple setups into a combined program.
02:32
Now,
02:32
while we do have the ability to combine them together doesn't necessarily mean
02:37
that we have to we can still use them for individual operations.
02:40
So let's start taking a look at creating an NC program.
02:43
First notice that the post is selected here at the very top.
02:48
If we had selected a machine configuration inside of our setup
02:52
we could use that option to bring in the post.
02:54
Specifically
02:55
machine configurations can also be used for machine simulation.
02:59
We didn't really talk about machine simulation during verification but it
03:03
is a great way to not only verify the tool paths,
03:06
but also the motion inside of a specific machine
03:09
from here. We do want to make sure that we select a very specific post.
03:14
This is going to communicate or translate everything that we've
03:17
done here in Fusion 3 60 to a machine.
03:20
Now for me, what I want to do is select the
03:22
next gen control.
03:24
You can do this by going to choose from library and then you can
03:28
use the option to search by vendor and we can also search by capability.
03:34
For example, in the vendor we're going to select HaAS automation.
03:37
Notice that there are a lot of very specific machines,
03:40
we've got some turning machines,
03:41
we've gotta try onion a UMC 7 50 multi axis machine and
03:46
we've got this one at the bottom called Hoss pre NGC.
03:49
So I'm going to select the Hoss pre NGC as
03:52
my post and again that's going to communicate everything.
03:55
Notice that the file name and number has come in
03:58
as 1001 but the comment has not come in and
04:01
that's because an NC program gives us the ability to
04:05
not just take information from one setup but from multiples.
04:08
So in this case I'm going to add a comment O. P one engine case.
04:13
It's the same comment that we placed directly inside of our current setup.
04:18
Also note that we have the ability to post this to fusion team.
04:22
So if you want to save your N. C. Programs, Infusion team as well as locally.
04:26
You do have that option by default,
04:28
the output folder will be listed inside of your user documents for fusion 3 60 cam
04:34
you can open that folder location or you can specify a new location for me.
04:39
I'm going to specify a new location
04:42
inside of the folder where my data sets are saved.
04:44
I'm going to create a new folder and I'm going to call this N. C. Programs
04:49
inside of this folder. This is where I'm going to place all of the code.
04:53
So now all of those are going to be placed in there.
04:56
Also notice that inside of here we've got post properties rather than going
05:00
in and manually modifying a post processor which can be pretty dangerous.
05:04
We have options that we can turn on and off.
05:07
For example, if your machine has an auger, you can include a code inside of the N. C.
05:12
Program that's going to automatically turn that on for you.
05:15
We have optional stops pre load tool programmable coolant.
05:20
There are many different options that you want to
05:22
look through based on your specific machine and controller.
05:25
We're gonna move on to the next tab which is operations And here
05:29
is where we're going to select either individual tool paths or entire setups.
05:33
Note that multiple setups can be included but there will be some issues
05:37
if you're trying to post with the same work offset for multiple operations.
05:42
So just keep in mind that there might
05:43
be some limitations depending on your machine and configuration
05:47
from here.
05:48
What we're going to do is we're going to post everything and notice that there
05:51
is a check mark up here that we can reorder to minimize tool changes.
05:55
Now I would strongly suggest that you don't use
05:57
this check box at least as you're getting started,
06:00
make sure that you understand the order of operations and
06:03
how you programmed everything because you probably had a good reason
06:07
from here. We can post it or we can simply say OK or cancel for this example.
06:12
We're going to say okay
06:14
and note that N C program one has been created.
06:16
What I'm gonna do is I'm going to call this O P one N C P for N C program.
06:22
I'm going to repeat the process again. Going to set up create NC. Program.
06:27
Notice that
06:28
pre NGC is here.
06:30
We're going to create 1000 to comment is going to be O P two engine case.
06:38
It's going to go to the same folder location and we're going to use the same options.
06:43
Next we're going to go to operations and this
06:45
time I'm going to select opt to and say okay
06:49
I'm going to rename this Opie to NCP for
06:52
NC program and repeat the process two more times.
06:55
Once again we need to adjust things like the program number and the comment.
07:00
This is going to be O. P three
07:02
and again we're going to do engine case,
07:06
Move on to our operations and do
07:08
up three.
07:11
Want to Rename This 10 p three and NCP.
07:15
And lastly,
07:16
we'll create one more and once again we're gonna modify this one more time.
07:21
O. P four
07:23
engine case
07:25
operations will be everything inside of O P four.
07:29
Note that this is using the same work offset as op three and that's okay.
07:34
And then we want to rename the N. C program.
07:38
There are a couple of other things that we
07:40
can consider when we're talking about NC programs.
07:44
Let's just hop into one more NC program that we're going to
07:47
cancel when we take a look at the machine and post.
07:51
We select we do have an option to select things like operation sheets
07:55
or set up sheets or tool lists directly from the post processor list.
08:01
This means that instead of posting code to a specific machine,
08:04
what we're actually doing is creating a setup sheet for that operation.
08:08
There are other ways that we can do this as well.
08:10
Once we have our different NC programs created for up
08:18
We can select set up sheet or we can select post process for this example.
08:23
I'm only going to be taking a look at one of these.
08:25
And in this case let's go ahead and take a look at op three.
08:29
I'm going to right click and select post process
08:32
when we post process, it's going to take all of our settings that we used,
08:36
the machine that we selected for our post processor
08:38
and it's going to create our NC program again.
08:41
This is going to be saved in a specific location.
08:44
You can see here that we've got our two D adaptive tool path.
08:48
And as we scroll down we have other information and other tool paths that we can find.
08:53
Let's go ahead and cancel out of this and let's try O. P.
08:56
One NCP and select post process
08:59
now
08:60
one NCP does have some renamed tool paths. So you can see here this is called face top.
09:06
And if we scroll down we've got contour outside profile.
09:10
So renaming the tool path not only helps when we're viewing it in
09:13
the browser but it also does help when you're viewing the code.
09:16
We can verify that we are using G 54
09:20
you can see that we have a spindle speed that's above our 7500 limit.
09:24
So if our machine is fixed at 7500 we would want
09:27
to make sure we go back and adjust the tool parameters.
09:31
If we want to create a set up sheet for a single operation
09:34
or set up we can right click and select set up sheet.
09:38
So we're going to say this in the location in our data panel where our file is.
09:43
Once we say okay, a setup sheet will populate,
09:46
you can see that we see are part inside of the
09:48
Vice we have information about things like the maximum spindle speed,
09:52
the tools that are used.
09:53
We have a tool list. These can be compressed to make it a little bit easier to see.
09:58
We have a graphic showing our setup,
09:60
you can see the coordinate system is shown here and the
10:03
note Typical Vice 1.75 inch tall jaw with 1.375 parallels.
10:09
So again, this helps us understand the operations, the tools and the setup.
10:14
We also have configuration options where we can show only the tools used.
10:19
We can also show a compact version which reduces some of the screenshots
10:23
that are used and then we can show things like summary image only.
10:26
So there are no tool images here.
10:30
So with these configurations we can then print this out as a pdf or an
10:34
actual paper copy or if you have anybody that is working directly in your project,
10:40
they will have access to it inside of your data panel.
10:42
You can see it's listed here as 1001 dot F S S D If I double click on that,
10:48
it's going to open up in a web browser.
10:52
So from here we now are able to create our setup sheets and r
10:56
n C programs which allow us to translate that G code to something.
10:60
Our machines can read.
11:01
There are additional things that we can do.
11:04
For example, we can create a set up sheet for all of the operations at the same time.
11:08
And we can do this by either selecting all the operations,
11:12
right clicking and selecting setup sheet.
11:14
Or we can also go in and do things like create an NC program.
11:19
And when we create a new NC program,
11:21
we simply need to select all of the various operations and we can use either
11:26
a setup sheet for the post option or we can right click on that N.
11:31
C. Program and select setup sheet.
11:33
When we do this.
11:34
This setup sheet is going to include all of the various operations and tool paths.
11:39
And you can see here as we scroll down through this,
11:42
that we now have all the tools and we have the various orientations.
11:46
You will notice that there are some problems
11:48
associated doing it this way because now the
11:50
vice is shown as the same vice from op one and it's obscuring our part.
11:55
So we do need to think about these things and plan ahead.
11:58
When we do decide to create our documentation
12:01
at this point,
12:02
make sure that everything is saved and we can go ahead and move on to the next step
Video transcript
00:02
create cam documentation
00:06
in this video. We'll create an NC. Program and will create a setup sheet.
00:12
Infusion 3 60. Let's carry on with our engine case, Rh ready to program.
00:17
Now in this case we've created four operations.
00:21
We've got op one, op two, op three and up four.
00:25
Each of these are machines at different times
00:27
in the same vice using different sized parallels.
00:30
So a couple things that we need to do is we need to account
00:33
for notes that need to be displayed in what's called a setup sheet.
00:37
The easiest way for us to do this is to
00:39
create notes in individual operations or the tool paths themselves.
00:44
So first let's go ahead and take a look at op one.
00:48
The first thing to note about op one is that we use a specific size parallel a 1.375.
00:55
So I want to make sure that that notes included in our setup sheet.
00:58
So I'm going to right click on op one and I'm gonna select edit notes inside of here.
01:04
We're gonna say T. Y. P. For typical vice. 1.75 inch tall jaw
01:13
With our 1.375" parallels.
01:19
Once we say okay we're going to have a note icon that displays and
01:23
when we hover the cursor over it we can see what that note is.
01:26
More importantly that note gets displayed on our setup sheet.
01:30
Now you can do the same thing with any of the operations as well.
01:34
For example if we look down through here and we have a spot we
01:38
can right click and we can select edit notes for the spot drill.
01:43
We want to make sure not to go too deep.
01:46
So we're gonna say don't spot drill too deep.
01:51
So the notes can be very specific about the setup,
01:54
for example using a certain size parallel or it can be notes of
01:58
caution or maybe adjustments that could be made to the tool path.
02:02
Now these are going to be at the operation or
02:05
set up level and the individual tool path level.
02:08
We can go through and we can make notes on every tool path and every operation.
02:13
But I think this gets the point across from here.
02:16
The next thing that we want to do is we want to create something called an NC program.
02:21
When we go to the set up drop down. We have create N. C. Program
02:25
and
02:26
programs are a way for us to group tool
02:28
paths together in multiple setups into a combined program.
02:32
Now,
02:32
while we do have the ability to combine them together doesn't necessarily mean
02:37
that we have to we can still use them for individual operations.
02:40
So let's start taking a look at creating an NC program.
02:43
First notice that the post is selected here at the very top.
02:48
If we had selected a machine configuration inside of our setup
02:52
we could use that option to bring in the post.
02:54
Specifically
02:55
machine configurations can also be used for machine simulation.
02:59
We didn't really talk about machine simulation during verification but it
03:03
is a great way to not only verify the tool paths,
03:06
but also the motion inside of a specific machine
03:09
from here. We do want to make sure that we select a very specific post.
03:14
This is going to communicate or translate everything that we've
03:17
done here in Fusion 3 60 to a machine.
03:20
Now for me, what I want to do is select the
03:22
next gen control.
03:24
You can do this by going to choose from library and then you can
03:28
use the option to search by vendor and we can also search by capability.
03:34
For example, in the vendor we're going to select HaAS automation.
03:37
Notice that there are a lot of very specific machines,
03:40
we've got some turning machines,
03:41
we've gotta try onion a UMC 7 50 multi axis machine and
03:46
we've got this one at the bottom called Hoss pre NGC.
03:49
So I'm going to select the Hoss pre NGC as
03:52
my post and again that's going to communicate everything.
03:55
Notice that the file name and number has come in
03:58
as 1001 but the comment has not come in and
04:01
that's because an NC program gives us the ability to
04:05
not just take information from one setup but from multiples.
04:08
So in this case I'm going to add a comment O. P one engine case.
04:13
It's the same comment that we placed directly inside of our current setup.
04:18
Also note that we have the ability to post this to fusion team.
04:22
So if you want to save your N. C. Programs, Infusion team as well as locally.
04:26
You do have that option by default,
04:28
the output folder will be listed inside of your user documents for fusion 3 60 cam
04:34
you can open that folder location or you can specify a new location for me.
04:39
I'm going to specify a new location
04:42
inside of the folder where my data sets are saved.
04:44
I'm going to create a new folder and I'm going to call this N. C. Programs
04:49
inside of this folder. This is where I'm going to place all of the code.
04:53
So now all of those are going to be placed in there.
04:56
Also notice that inside of here we've got post properties rather than going
05:00
in and manually modifying a post processor which can be pretty dangerous.
05:04
We have options that we can turn on and off.
05:07
For example, if your machine has an auger, you can include a code inside of the N. C.
05:12
Program that's going to automatically turn that on for you.
05:15
We have optional stops pre load tool programmable coolant.
05:20
There are many different options that you want to
05:22
look through based on your specific machine and controller.
05:25
We're gonna move on to the next tab which is operations And here
05:29
is where we're going to select either individual tool paths or entire setups.
05:33
Note that multiple setups can be included but there will be some issues
05:37
if you're trying to post with the same work offset for multiple operations.
05:42
So just keep in mind that there might
05:43
be some limitations depending on your machine and configuration
05:47
from here.
05:48
What we're going to do is we're going to post everything and notice that there
05:51
is a check mark up here that we can reorder to minimize tool changes.
05:55
Now I would strongly suggest that you don't use
05:57
this check box at least as you're getting started,
06:00
make sure that you understand the order of operations and
06:03
how you programmed everything because you probably had a good reason
06:07
from here. We can post it or we can simply say OK or cancel for this example.
06:12
We're going to say okay
06:14
and note that N C program one has been created.
06:16
What I'm gonna do is I'm going to call this O P one N C P for N C program.
06:22
I'm going to repeat the process again. Going to set up create NC. Program.
06:27
Notice that
06:28
pre NGC is here.
06:30
We're going to create 1000 to comment is going to be O P two engine case.
06:38
It's going to go to the same folder location and we're going to use the same options.
06:43
Next we're going to go to operations and this
06:45
time I'm going to select opt to and say okay
06:49
I'm going to rename this Opie to NCP for
06:52
NC program and repeat the process two more times.
06:55
Once again we need to adjust things like the program number and the comment.
07:00
This is going to be O. P three
07:02
and again we're going to do engine case,
07:06
Move on to our operations and do
07:08
up three.
07:11
Want to Rename This 10 p three and NCP.
07:15
And lastly,
07:16
we'll create one more and once again we're gonna modify this one more time.
07:21
O. P four
07:23
engine case
07:25
operations will be everything inside of O P four.
07:29
Note that this is using the same work offset as op three and that's okay.
07:34
And then we want to rename the N. C program.
07:38
There are a couple of other things that we
07:40
can consider when we're talking about NC programs.
07:44
Let's just hop into one more NC program that we're going to
07:47
cancel when we take a look at the machine and post.
07:51
We select we do have an option to select things like operation sheets
07:55
or set up sheets or tool lists directly from the post processor list.
08:01
This means that instead of posting code to a specific machine,
08:04
what we're actually doing is creating a setup sheet for that operation.
08:08
There are other ways that we can do this as well.
08:10
Once we have our different NC programs created for up
08:18
We can select set up sheet or we can select post process for this example.
08:23
I'm only going to be taking a look at one of these.
08:25
And in this case let's go ahead and take a look at op three.
08:29
I'm going to right click and select post process
08:32
when we post process, it's going to take all of our settings that we used,
08:36
the machine that we selected for our post processor
08:38
and it's going to create our NC program again.
08:41
This is going to be saved in a specific location.
08:44
You can see here that we've got our two D adaptive tool path.
08:48
And as we scroll down we have other information and other tool paths that we can find.
08:53
Let's go ahead and cancel out of this and let's try O. P.
08:56
One NCP and select post process
08:59
now
08:60
one NCP does have some renamed tool paths. So you can see here this is called face top.
09:06
And if we scroll down we've got contour outside profile.
09:10
So renaming the tool path not only helps when we're viewing it in
09:13
the browser but it also does help when you're viewing the code.
09:16
We can verify that we are using G 54
09:20
you can see that we have a spindle speed that's above our 7500 limit.
09:24
So if our machine is fixed at 7500 we would want
09:27
to make sure we go back and adjust the tool parameters.
09:31
If we want to create a set up sheet for a single operation
09:34
or set up we can right click and select set up sheet.
09:38
So we're going to say this in the location in our data panel where our file is.
09:43
Once we say okay, a setup sheet will populate,
09:46
you can see that we see are part inside of the
09:48
Vice we have information about things like the maximum spindle speed,
09:52
the tools that are used.
09:53
We have a tool list. These can be compressed to make it a little bit easier to see.
09:58
We have a graphic showing our setup,
09:60
you can see the coordinate system is shown here and the
10:03
note Typical Vice 1.75 inch tall jaw with 1.375 parallels.
10:09
So again, this helps us understand the operations, the tools and the setup.
10:14
We also have configuration options where we can show only the tools used.
10:19
We can also show a compact version which reduces some of the screenshots
10:23
that are used and then we can show things like summary image only.
10:26
So there are no tool images here.
10:30
So with these configurations we can then print this out as a pdf or an
10:34
actual paper copy or if you have anybody that is working directly in your project,
10:40
they will have access to it inside of your data panel.
10:42
You can see it's listed here as 1001 dot F S S D If I double click on that,
10:48
it's going to open up in a web browser.
10:52
So from here we now are able to create our setup sheets and r
10:56
n C programs which allow us to translate that G code to something.
10:60
Our machines can read.
11:01
There are additional things that we can do.
11:04
For example, we can create a set up sheet for all of the operations at the same time.
11:08
And we can do this by either selecting all the operations,
11:12
right clicking and selecting setup sheet.
11:14
Or we can also go in and do things like create an NC program.
11:19
And when we create a new NC program,
11:21
we simply need to select all of the various operations and we can use either
11:26
a setup sheet for the post option or we can right click on that N.
11:31
C. Program and select setup sheet.
11:33
When we do this.
11:34
This setup sheet is going to include all of the various operations and tool paths.
11:39
And you can see here as we scroll down through this,
11:42
that we now have all the tools and we have the various orientations.
11:46
You will notice that there are some problems
11:48
associated doing it this way because now the
11:50
vice is shown as the same vice from op one and it's obscuring our part.
11:55
So we do need to think about these things and plan ahead.
11:58
When we do decide to create our documentation
12:01
at this point,
12:02
make sure that everything is saved and we can go ahead and move on to the next step
Step-by-step guide
How to buy
Privacy | Do not sell or share my personal information | Cookie preferences | Report noncompliance | Terms of use | Legal | © 2025 Autodesk Inc. All rights reserved
Sign in to start learning
Sign in for unlimited free access to all learning content.Save your progress
Take assessments
Receive personalized recommendations
May we collect and use your data?
Learn more about the Third Party Services we use and our Privacy Statement.May we collect and use your data to tailor your experience?
Explore the benefits of a customized experience by managing your privacy settings for this site or visit our Privacy Statement to learn more about your options.