Transcript
00:09
This course will cover how to use Autodesk Inventor Professional to annotate and share your 3D models.
00:19
We'll start with an overview of the Autodesk Inventor 3D annotations environment and how to use it properly to define,
00:26
as well as tolerance your models before exporting them to share with others.
00:33
The Autodesk Inventor "Annotate" tab gives users the ability to add Dimensions,
00:39
Tolerances and Notes onto a three-dimensional model instead of a two-dimensional drawing.
00:44
This is typically easier to interpret and allows users to export this data inside of a three-dimensional PDF,
00:52
or a STEP 242 file for CNC and CMM machine integration.
00:59
The Inventor annotation environment also includes what's called the Tolerance Advisor which will provide messages,
01:06
warnings and other feedback to help users properly constrain orient and tolerance a model prior to sending it for manufacturing.
01:16
So this slide shows the general workflow that will be used when creating 3D annotations with Autodesk Inventor.
01:26
So once you've activated the "Annotation" tab,
01:29
you can then add dimensions manually or you can extract them from the 3D CAD model automatically.
01:36
Once the dimensions have been added,
01:38
you can then include specific hole and thread notes to define hole-thread sizing, as well as depth and counter bore options.
01:48
You can also edit these notes to include a size tolerance,
01:51
that can be used in combination with your geometric dimensioning and tolerancing later.
01:57
Next, you'll typically add your Notes.
01:60
These can just be general notes or overall profile notes.
02:03
This will replace the typical notes block or title block you would see on a two-dimensional drawing.
02:09
However, it will be shown at all times on the 3D graphics window when viewing the CAD model,
02:15
and these notes will also be included with the 3D PDF if you choose to export it that way.
02:22
Next, you'll jump into creating Tolerance Features.
02:26
This is where you will begin to define your datums -- datum A, B, C, etcetera,
02:32
and then create your Datum Reference Frame from that.
02:35
Once that's been established, you can add additional tolerance features referencing that datum reference frame,
02:41
and then you can continue to validate your GD&T using the Tolerance Advisor.
02:47
Once you have satisfied all the conditions and recommendations of the Tolerance Advisor,
02:51
you can then export your model as a 3D PDF or STEP file to share with others and to produce your manufacturing file.
03:03
So in the annotation environment,
03:05
you'll notice there's going to be two folders that are created as you add Dimensions,
03:09
Notes and Tolerance Features.
03:12
The first folder is your Annotations folder.
03:14
This will contain all of your dimensions as well as your hole notes, surface texture call outs and weld symbols.
03:21
You can right-click and edit any of these from the browser.
03:25
You can also select them in the browser to highlight them in the graphics window to confirm which one is which.
03:32
The other folder that's created is going to be your "Tolerance Features" folder.
03:35
This will include all of your datum reference frames, Tolerance Features and Notes included with the Tolerances.
03:46
So take a look at the first few steps in that workflow.
03:49
Anything you do to add Dimensions, Notes or general notes as well as Surface Texture call outs,
03:55
all of those items will be added to the "Annotations" folder and will show up there in the browser.
04:00
That folder will not be created until you add your first Dimension or Note.
04:04
And then you can find those items there later as you progress.
04:09
Anything that's created as a Tolerance Feature,
04:12
a datum feature or a datum reference frame will be added to the "Tolerance Features" folder in the browser,
04:19
and it can be edited and accessed from that area at any point in time.
04:28
So if you select dimension from the "Annotate" tab, that will activate the Dimension options.
04:34
Once you've selected a couple of faces, it will give you a preview of what that dimension will look like.
04:39
Now, the biggest difference between this and a sketch environment or a 2D drawing environment,
04:46
is that you have to choose a plane on which this annotation will lie and be visible in the 3D environment.
04:54
So you can toggle which plane the dimension will show up on, whether that's an XY or XZ plane.
05:01
Using the "Spacebar," you can toggle between the two.
05:05
If you hold the "Shift" button, you can then select a new face reference and your dimension will be placed on that plane.
05:14
Once the dimension is created, you can then edit the format,
05:18
you can edit how it is toleranced and what the size is going to be,
05:22
whether that's a symmetric plus/minus tolerance, or if you set a firm max/min limit.
05:30
Once you've defined all of that, you can then reference these dimensions later when you're adding in tolerance features.
05:35
But this will be the first step in any 3D annotation.
05:40
Hole and Thread Notes can also be added in the 3D annotation environment.
05:44
This is extremely helpful when you have something like a counter sync, counter bore,
05:50
or maybe threaded hole that you created in the part file.
05:53
It can bring in some of that information and data automatically, so that you do not have to type all that in and add those symbols.
06:00
Now, those symbols as well as the Precision and Tolerance can be adjusted Manually once that hole note has been created.
06:09
You can also type in custom notes and add an additional symbols where they are needed.
06:15
The check boxes will give you the ability to use Global Precision for your number of decimal places,
06:20
as well as whether or not to use the Part Tolerance for your Tolerance values.
06:25
The dropdown menu where you see "Default" allows you to change to a symmetric or a min/max type of size tolerance,
06:33
that can then be adjusted when you get to add a datum feature as well.
06:39
Your General Notes are going to replace your typical note block you would see on a two-dimensional drawing.
06:45
And this can also be used to automatically place your profile tolerances.
06:50
If you are applying a Global Profile Tolerance, you can do that here as well.
06:55
If you have a specific surface or edge on the model you want to call out, you may consider using leader text.
07:01
This gives you a little bit more control over call outs and notes on your three-dimensional model.
07:07
Again, this will all be included in the three-dimensional PDF as well.
07:15
The tolerance feature in the annotate environment is going to give you the ability to add in your datums as well as your tolerance features.
07:25
It is automatically going to choose a tolerance feature based off of your selection.
07:30
So for instance, if you choose a flat surface, it may choose flatness or profile.
07:35
Whereas if you choose a cylindrical hole feature,
07:38
it's likely to choose something like perpendicularity, cylindricity or maybe hole position.
07:45
So we'll intelligently try to recognize what is needed.
07:48
Now, the specific tolerance type and whether or not it's a datum identifier can be changed and manually updated.
07:56
However, some of the guess work is eliminated when you're using a smart tool like this.
08:03
If at any point, you need to add additional segments to the feature control frame, you can do that using "Add Segment,"
08:08
and you can then update your datum reference frame once enough datums have been created and use that to properly
08:15
constrain your model for inspection purposes.
08:21
So once you've established a datum A, B and C,
08:25
in your datum reference frame, you can choose which datums are primary, secondary and tertiary.
08:32
This datum reference frame can then be used later when you are locating holes or adding in things like Profile Tolerances.
08:41
You can also customize this as you go and the corresponding features will update automatically.
08:48
All of this will be included in the STEP file and the 3D PDF as well when you go to export.
08:57
After you create your first tolerance feature,
08:59
the Tolerance Advisor will automatically be activated and show up as a separate tab in the browser.
09:06
You can mostly ignore it until you've finished adding in your datums and features.
09:11
But it's important to keep track of what some of these messages are and how you can fix them.
09:16
If you right-click on any of the messages that come up and you select "More Information,"
09:20
it'll actually open up that specific page in the Help manual,
09:24
which typically will give you info on the message as well as a recommended solution to that problem.
09:33
You can also activate the Face Status Coloring at the bottom of the Tolerance Feature browser.
09:39
What this will do is it'll show you a legend and identify what surfaces are currently fully constrained,
09:45
partially constrained or unconstrained by the Geometric Dimension and Tolerancing that you have put in place.
09:56
The last step in the annotation process is typically going to be sharing your model-based definition file.
10:03
So to do this, you can export as a three-dimensional PDF that can be viewed with Adobe Acrobat.
10:09
This is really helpful when you are sharing with a vendor or a manufacturer, and they'd like to be able to rotate the model around,
10:17
and view your Dimensions and Tolerances without needing a CAD software,
10:24
or anything like that to actually view that data.
10:28
The other way you can export your model is using a STEP format or a CAD format.
10:32
If you are using a STEP file that you want to be read into your CMM software,
10:37
make sure to choose STEP 242 format in the "Options" when you go to save the file to your computer drive.
10:47
So I'll give you a quick overview of the annotate environment using this gear housing part file shown here.
10:53
Within Autodesk Inventor, if I'm on the "3D Model" tab, I'll just switch over to the "Annotate" tab,
10:58
and this is where you'll see your Geometric Tolerances as well as your General Annotations and Notes.
11:04
The export options are shown over to the right.
11:08
So if I were to start by just adding something like a simple dimension by selecting Dimension,
11:14
once I select two faces, so I'll choose a face on one side and then another face on the opposing,
11:22
you'll notice it automatically places this dimension and then it gives me a plane showing me,
11:27
how this is going to be shown on the 3D model and what plane it will rest on.
11:32
If I want to change this, I can just hit the "Spacebar" on my keyboard which will flip it to the next available plane.
11:39
So for this specific dimension, I have two plane options, this XY plane and then this XZ plane.
11:46
If you want it to lie on a specific face,
11:50
you can also hold the "Shift" button and then select that face,
11:54
and it will then place it on the plane that is corresponding to that selection.
12:00
So now if I were to select with my left-click, it'll place that dimension,
12:06
and then it'll open up the options here where I can choose things like Precision,
12:11
Tolerances and how this is going to be formatted.
12:15
So for instance, let's say instead of a "Default," it's actually going to have a specific "Symmetric" tolerance to it.
12:23
I'll change to "Symmetric" and you'll then see up here where I have a plus or minus 00,
12:29
I can double-click on that and I can change this to, for instance, 0.01, click the "Check Mark."
12:35
And then now my dimensions has been added to my three-dimensional model.
12:41
So let's say then I want to add in a hole note, I can simply go to the "Hole/Thread Note" option.
12:48
Once I've selected that, notice I can't choose a flat surface,
12:51
it will only let me choose a cylindrical face or edge. So if I choose this one here,
12:57
it then gives me the same options as before where I can toggle what plane I want this to lie on.
13:02
Once I've left-clicked to confirm, I can then once again change whether or not I want to use Global Precision, a Part Tolerance.
13:12
I can doubleclick on the value if I'd like to change the formatting or the precision of that call out.
13:19
If I click this little icon here where you see this "Edit Hole Note" button,
13:24
what that'll do is then open up a window where I can add in additional text and symbols,
13:29
things like counter sync, counter bore and diameter.
13:34
So I'll select "OK" to confirm that.
13:37
Click the "Check Mark" and now I have a Hole Note added in to this file.
13:42
If the Hole Note is something that is threaded -- so for instance, this time I choose a threaded hole,
13:47
what you'll notice about that is it pulls that information from the original CAD model.
13:51
So it'll say the actual size of the thread being used for that hole feature.
13:58
Now, if you have a note that is going to just be added as a Note Block, you can click on the "General Note" button and then type that in.
14:08
So I might say break all sharp edges...
14:18
Select "OK", and it'll be added into this corner.
14:21
This will show up regardless of what view you're currently looking at.
14:25
And you can also use this to add in general profile notes. So if I select that option from the panel,
14:32
I can choose which quadrant I want it to be in. I'm going to choose the same exact one. It just adds it to the next line,
14:38
and it'll then say the Profile Note and I can then adjust that Tolerance as well before clicking "OK."
14:46
And now this will be my note block that'll show in all views.
14:52
So now I'm ready to start adding in some Tolerance Features as well as a datum reference frame.
14:57
Now, in order to do that, I can go ahead and select Tolerance Feature from the top panel,
15:03
I can then choose this bottom face for instance and hit the "Check Mark."
15:08
Now, based off of this selection, it knows it's a flat planar face and it assumes that I want a flatness tolerance on it.
15:14
It also assumes that I'm going to be setting this as my datum A.
15:19
So I'll click to confirm.
15:21
I can then choose if I'd like to use this as a "Datum identifier" or not what the actual value for that datum will be.
15:29
And when I'm ready to confirm, I can hit the "Check Mark" and that will be added into the 3D window.
15:34
You'll notice the Tolerance Advisor shows up as soon as you add your first tolerance as well.
15:39
Again, keep in mind that this will continue to update as you add additional Tolerance Features.
15:44
So it is not a final list of messages.
15:47
So I'll add one more Tolerance Feature here to this hole going through the middle of the housing,
15:54
hit the "Check Mark." And once again, it identifies this as a hole feature.
15:58
It also assumes I want perpendicularity to datum A and it also assumes that I want this to be my datum B.
16:07
So I click to confirm.
16:09
Once again, I can add additional segments, I can adjust whether or not I want it to be a "Datum identifier" or not,
16:16
and what that value is going to be and hit the "Check Mark" to confirm.
16:20
And now I am ready to save this and export as a PDF or a STEP file.
16:28
So for this example, I will go ahead and select "CAD format."
16:32
When I do that, I can choose where I would like to save this file and what the type is going to be,
16:38
which in this case will be STEP format.
16:41
And then there's this "Options" option right here.
16:43
If I select that,
16:45
I can then choose 242 which is your MBD format,
16:51
which will be best if you are integrating with a CMM machine.
16:55
So I'll select "OK."
16:57
And then I can click "Save" to export this as a STEP file.
00:09
This course will cover how to use Autodesk Inventor Professional to annotate and share your 3D models.
00:19
We'll start with an overview of the Autodesk Inventor 3D annotations environment and how to use it properly to define,
00:26
as well as tolerance your models before exporting them to share with others.
00:33
The Autodesk Inventor "Annotate" tab gives users the ability to add Dimensions,
00:39
Tolerances and Notes onto a three-dimensional model instead of a two-dimensional drawing.
00:44
This is typically easier to interpret and allows users to export this data inside of a three-dimensional PDF,
00:52
or a STEP 242 file for CNC and CMM machine integration.
00:59
The Inventor annotation environment also includes what's called the Tolerance Advisor which will provide messages,
01:06
warnings and other feedback to help users properly constrain orient and tolerance a model prior to sending it for manufacturing.
01:16
So this slide shows the general workflow that will be used when creating 3D annotations with Autodesk Inventor.
01:26
So once you've activated the "Annotation" tab,
01:29
you can then add dimensions manually or you can extract them from the 3D CAD model automatically.
01:36
Once the dimensions have been added,
01:38
you can then include specific hole and thread notes to define hole-thread sizing, as well as depth and counter bore options.
01:48
You can also edit these notes to include a size tolerance,
01:51
that can be used in combination with your geometric dimensioning and tolerancing later.
01:57
Next, you'll typically add your Notes.
01:60
These can just be general notes or overall profile notes.
02:03
This will replace the typical notes block or title block you would see on a two-dimensional drawing.
02:09
However, it will be shown at all times on the 3D graphics window when viewing the CAD model,
02:15
and these notes will also be included with the 3D PDF if you choose to export it that way.
02:22
Next, you'll jump into creating Tolerance Features.
02:26
This is where you will begin to define your datums -- datum A, B, C, etcetera,
02:32
and then create your Datum Reference Frame from that.
02:35
Once that's been established, you can add additional tolerance features referencing that datum reference frame,
02:41
and then you can continue to validate your GD&T using the Tolerance Advisor.
02:47
Once you have satisfied all the conditions and recommendations of the Tolerance Advisor,
02:51
you can then export your model as a 3D PDF or STEP file to share with others and to produce your manufacturing file.
03:03
So in the annotation environment,
03:05
you'll notice there's going to be two folders that are created as you add Dimensions,
03:09
Notes and Tolerance Features.
03:12
The first folder is your Annotations folder.
03:14
This will contain all of your dimensions as well as your hole notes, surface texture call outs and weld symbols.
03:21
You can right-click and edit any of these from the browser.
03:25
You can also select them in the browser to highlight them in the graphics window to confirm which one is which.
03:32
The other folder that's created is going to be your "Tolerance Features" folder.
03:35
This will include all of your datum reference frames, Tolerance Features and Notes included with the Tolerances.
03:46
So take a look at the first few steps in that workflow.
03:49
Anything you do to add Dimensions, Notes or general notes as well as Surface Texture call outs,
03:55
all of those items will be added to the "Annotations" folder and will show up there in the browser.
04:00
That folder will not be created until you add your first Dimension or Note.
04:04
And then you can find those items there later as you progress.
04:09
Anything that's created as a Tolerance Feature,
04:12
a datum feature or a datum reference frame will be added to the "Tolerance Features" folder in the browser,
04:19
and it can be edited and accessed from that area at any point in time.
04:28
So if you select dimension from the "Annotate" tab, that will activate the Dimension options.
04:34
Once you've selected a couple of faces, it will give you a preview of what that dimension will look like.
04:39
Now, the biggest difference between this and a sketch environment or a 2D drawing environment,
04:46
is that you have to choose a plane on which this annotation will lie and be visible in the 3D environment.
04:54
So you can toggle which plane the dimension will show up on, whether that's an XY or XZ plane.
05:01
Using the "Spacebar," you can toggle between the two.
05:05
If you hold the "Shift" button, you can then select a new face reference and your dimension will be placed on that plane.
05:14
Once the dimension is created, you can then edit the format,
05:18
you can edit how it is toleranced and what the size is going to be,
05:22
whether that's a symmetric plus/minus tolerance, or if you set a firm max/min limit.
05:30
Once you've defined all of that, you can then reference these dimensions later when you're adding in tolerance features.
05:35
But this will be the first step in any 3D annotation.
05:40
Hole and Thread Notes can also be added in the 3D annotation environment.
05:44
This is extremely helpful when you have something like a counter sync, counter bore,
05:50
or maybe threaded hole that you created in the part file.
05:53
It can bring in some of that information and data automatically, so that you do not have to type all that in and add those symbols.
06:00
Now, those symbols as well as the Precision and Tolerance can be adjusted Manually once that hole note has been created.
06:09
You can also type in custom notes and add an additional symbols where they are needed.
06:15
The check boxes will give you the ability to use Global Precision for your number of decimal places,
06:20
as well as whether or not to use the Part Tolerance for your Tolerance values.
06:25
The dropdown menu where you see "Default" allows you to change to a symmetric or a min/max type of size tolerance,
06:33
that can then be adjusted when you get to add a datum feature as well.
06:39
Your General Notes are going to replace your typical note block you would see on a two-dimensional drawing.
06:45
And this can also be used to automatically place your profile tolerances.
06:50
If you are applying a Global Profile Tolerance, you can do that here as well.
06:55
If you have a specific surface or edge on the model you want to call out, you may consider using leader text.
07:01
This gives you a little bit more control over call outs and notes on your three-dimensional model.
07:07
Again, this will all be included in the three-dimensional PDF as well.
07:15
The tolerance feature in the annotate environment is going to give you the ability to add in your datums as well as your tolerance features.
07:25
It is automatically going to choose a tolerance feature based off of your selection.
07:30
So for instance, if you choose a flat surface, it may choose flatness or profile.
07:35
Whereas if you choose a cylindrical hole feature,
07:38
it's likely to choose something like perpendicularity, cylindricity or maybe hole position.
07:45
So we'll intelligently try to recognize what is needed.
07:48
Now, the specific tolerance type and whether or not it's a datum identifier can be changed and manually updated.
07:56
However, some of the guess work is eliminated when you're using a smart tool like this.
08:03
If at any point, you need to add additional segments to the feature control frame, you can do that using "Add Segment,"
08:08
and you can then update your datum reference frame once enough datums have been created and use that to properly
08:15
constrain your model for inspection purposes.
08:21
So once you've established a datum A, B and C,
08:25
in your datum reference frame, you can choose which datums are primary, secondary and tertiary.
08:32
This datum reference frame can then be used later when you are locating holes or adding in things like Profile Tolerances.
08:41
You can also customize this as you go and the corresponding features will update automatically.
08:48
All of this will be included in the STEP file and the 3D PDF as well when you go to export.
08:57
After you create your first tolerance feature,
08:59
the Tolerance Advisor will automatically be activated and show up as a separate tab in the browser.
09:06
You can mostly ignore it until you've finished adding in your datums and features.
09:11
But it's important to keep track of what some of these messages are and how you can fix them.
09:16
If you right-click on any of the messages that come up and you select "More Information,"
09:20
it'll actually open up that specific page in the Help manual,
09:24
which typically will give you info on the message as well as a recommended solution to that problem.
09:33
You can also activate the Face Status Coloring at the bottom of the Tolerance Feature browser.
09:39
What this will do is it'll show you a legend and identify what surfaces are currently fully constrained,
09:45
partially constrained or unconstrained by the Geometric Dimension and Tolerancing that you have put in place.
09:56
The last step in the annotation process is typically going to be sharing your model-based definition file.
10:03
So to do this, you can export as a three-dimensional PDF that can be viewed with Adobe Acrobat.
10:09
This is really helpful when you are sharing with a vendor or a manufacturer, and they'd like to be able to rotate the model around,
10:17
and view your Dimensions and Tolerances without needing a CAD software,
10:24
or anything like that to actually view that data.
10:28
The other way you can export your model is using a STEP format or a CAD format.
10:32
If you are using a STEP file that you want to be read into your CMM software,
10:37
make sure to choose STEP 242 format in the "Options" when you go to save the file to your computer drive.
10:47
So I'll give you a quick overview of the annotate environment using this gear housing part file shown here.
10:53
Within Autodesk Inventor, if I'm on the "3D Model" tab, I'll just switch over to the "Annotate" tab,
10:58
and this is where you'll see your Geometric Tolerances as well as your General Annotations and Notes.
11:04
The export options are shown over to the right.
11:08
So if I were to start by just adding something like a simple dimension by selecting Dimension,
11:14
once I select two faces, so I'll choose a face on one side and then another face on the opposing,
11:22
you'll notice it automatically places this dimension and then it gives me a plane showing me,
11:27
how this is going to be shown on the 3D model and what plane it will rest on.
11:32
If I want to change this, I can just hit the "Spacebar" on my keyboard which will flip it to the next available plane.
11:39
So for this specific dimension, I have two plane options, this XY plane and then this XZ plane.
11:46
If you want it to lie on a specific face,
11:50
you can also hold the "Shift" button and then select that face,
11:54
and it will then place it on the plane that is corresponding to that selection.
12:00
So now if I were to select with my left-click, it'll place that dimension,
12:06
and then it'll open up the options here where I can choose things like Precision,
12:11
Tolerances and how this is going to be formatted.
12:15
So for instance, let's say instead of a "Default," it's actually going to have a specific "Symmetric" tolerance to it.
12:23
I'll change to "Symmetric" and you'll then see up here where I have a plus or minus 00,
12:29
I can double-click on that and I can change this to, for instance, 0.01, click the "Check Mark."
12:35
And then now my dimensions has been added to my three-dimensional model.
12:41
So let's say then I want to add in a hole note, I can simply go to the "Hole/Thread Note" option.
12:48
Once I've selected that, notice I can't choose a flat surface,
12:51
it will only let me choose a cylindrical face or edge. So if I choose this one here,
12:57
it then gives me the same options as before where I can toggle what plane I want this to lie on.
13:02
Once I've left-clicked to confirm, I can then once again change whether or not I want to use Global Precision, a Part Tolerance.
13:12
I can doubleclick on the value if I'd like to change the formatting or the precision of that call out.
13:19
If I click this little icon here where you see this "Edit Hole Note" button,
13:24
what that'll do is then open up a window where I can add in additional text and symbols,
13:29
things like counter sync, counter bore and diameter.
13:34
So I'll select "OK" to confirm that.
13:37
Click the "Check Mark" and now I have a Hole Note added in to this file.
13:42
If the Hole Note is something that is threaded -- so for instance, this time I choose a threaded hole,
13:47
what you'll notice about that is it pulls that information from the original CAD model.
13:51
So it'll say the actual size of the thread being used for that hole feature.
13:58
Now, if you have a note that is going to just be added as a Note Block, you can click on the "General Note" button and then type that in.
14:08
So I might say break all sharp edges...
14:18
Select "OK", and it'll be added into this corner.
14:21
This will show up regardless of what view you're currently looking at.
14:25
And you can also use this to add in general profile notes. So if I select that option from the panel,
14:32
I can choose which quadrant I want it to be in. I'm going to choose the same exact one. It just adds it to the next line,
14:38
and it'll then say the Profile Note and I can then adjust that Tolerance as well before clicking "OK."
14:46
And now this will be my note block that'll show in all views.
14:52
So now I'm ready to start adding in some Tolerance Features as well as a datum reference frame.
14:57
Now, in order to do that, I can go ahead and select Tolerance Feature from the top panel,
15:03
I can then choose this bottom face for instance and hit the "Check Mark."
15:08
Now, based off of this selection, it knows it's a flat planar face and it assumes that I want a flatness tolerance on it.
15:14
It also assumes that I'm going to be setting this as my datum A.
15:19
So I'll click to confirm.
15:21
I can then choose if I'd like to use this as a "Datum identifier" or not what the actual value for that datum will be.
15:29
And when I'm ready to confirm, I can hit the "Check Mark" and that will be added into the 3D window.
15:34
You'll notice the Tolerance Advisor shows up as soon as you add your first tolerance as well.
15:39
Again, keep in mind that this will continue to update as you add additional Tolerance Features.
15:44
So it is not a final list of messages.
15:47
So I'll add one more Tolerance Feature here to this hole going through the middle of the housing,
15:54
hit the "Check Mark." And once again, it identifies this as a hole feature.
15:58
It also assumes I want perpendicularity to datum A and it also assumes that I want this to be my datum B.
16:07
So I click to confirm.
16:09
Once again, I can add additional segments, I can adjust whether or not I want it to be a "Datum identifier" or not,
16:16
and what that value is going to be and hit the "Check Mark" to confirm.
16:20
And now I am ready to save this and export as a PDF or a STEP file.
16:28
So for this example, I will go ahead and select "CAD format."
16:32
When I do that, I can choose where I would like to save this file and what the type is going to be,
16:38
which in this case will be STEP format.
16:41
And then there's this "Options" option right here.
16:43
If I select that,
16:45
I can then choose 242 which is your MBD format,
16:51
which will be best if you are integrating with a CMM machine.
16:55
So I'll select "OK."
16:57
And then I can click "Save" to export this as a STEP file.
