Transcript
00:02
Working with a form as a BREP.
00:05
In this video, we'll use flatten and split body.
00:10
In Fusion 360, we want to carry on with our car hood.
00:13
We're going to begin working with it as a BREP.
00:16
But first let's take a look at a couple other tools that we have access to.
00:20
Under modify, there are many tools in here that can help us simplify the underlying geometry and potentially even create flattened sections.
00:29
For example, using the tool flatten.
00:31
It's important to look at and play around with all of these different tools to make sure that you understand their functionality.
00:37
In the case of the car hood, tools like smooth, pull, flatten and even straighten can be very handy.
00:45
Let's take a look at flatten.
00:47
Flatten allows us to fit, use a selected plane or make it parallel to a selected plane.
00:55
This allows us to make selections and create an average distance between them.
01:00
We can select a plane and pull geometry directly to it or we can be parallel to a plane.
01:07
When we do this, we can also use either control points or surface points.
01:12
The difference is the surface points will get pulled to the selected plane but the underlying geometry might be problematic.
01:19
Let's take a look at an example.
01:21
Let's use surface points first and we'll select the plane as our YZ plane.
01:27
When we start to select vertices, for example, inside of this grill area, notice how the geometry changes based on our selection.
01:37
If we change from surface points to control points, notice that we're actually getting closer to a flattened section inside of that area.
01:46
It's important to understand that the control points are creating the geometry or the underlying curvature based on their position.
01:55
But when we use the surface points, it can be problematic again because what we're really saying or what we're really doing here is,
02:03
we're taking the exact surface and we're moving it forward or parallel to a plane.
02:09
So it's a good idea to play around with these options and see if one works better than the other for your specific geometry.
02:16
If we needed to have a flat cooler or radiator mount here and we needed a flat section,
02:21
this could be a reason why we might want to flatten the grill opening.
02:25
If we don't like the way the grill opening actually ended up being created, we can select all these faces.
02:31
Use modify edit form and push it a little bit deeper into the car.
02:35
That way, that flattened section is a little bit farther back.
02:40
Now that we've played around with some more tools, let's finish the form.
02:43
Let's re show the body and take a look at the updates.
02:47
Everything looks pretty good from here.
02:49
Our crease on the edge is fine and we've got this flattened section even though it rolls back into those corners.
02:56
But now that we have this surface as a BREP, what can we do with it?
03:01
Let's begin by creating a sketch.
03:03
And in my case, I'm going to use the YZ plane and I'm going to start with a center point rectangle.
03:08
I'm going to make sure that I start below the origin and I'm going to place this about in the middle of my grill opening area.
03:16
I want to make sure that I have a vertical constraint between the center of that rectangle.
03:21
And then I want to begin using my sketch dimension tool to make sure its position is in this case 95 mm down.
03:29
I'm going to set its width 235 and I'm going to set its height to 30 mm.
03:38
Now that I have a sketch in relation to the grill opening, I could use that sketch to trim the surface.
03:45
I could use it to create an extrude that goes from or to a surface or I can use it to split the face of the surface.
03:53
In my case, I'm going to start by creating a solid extrude.
03:58
The solid extrude is going to come all the way through the geometry.
04:01
And the reason I'm doing this is because often times it's hard to find a good reference for where things need to be,
04:08
and you sometimes will create a reference such as this extrude that you can use as the basis for other features.
04:16
In my case, I'm going to go to my surface tools, go to create and select offset, select just this face.
04:24
I'm going to offset it forward 20 mm and say, OK.
04:28
When I offset at 20 mm, I'm then going to use the split body tool.
04:33
The body to split will be that rectangular extrude and the splitting tool will be that offset surface we just created.
04:40
This is going to leave me with that offset surface body and body 2.
04:46
And I can simply remove those.
04:49
The next thing that I might want to do is I might want to remove the geometry on the back side.
04:53
Once again I can use things like split body to get rid of that geometry.
04:58
Bodies to split will be this rectangular section and the splitting tool is going to be that surface.
05:06
Once again I could get rid of that body in this design but you'll note that this one didn't actually end up being split.
05:12
Sometimes working with these converted surfaces can be problematic and you might need to change your approach.
05:20
In this case, let's try split body one more time.
05:22
This is our body to split.
05:25
This is our split tool but we're going to turn off extend splitting tool and say OK and see if that allows us to split that solid body.
05:33
So turning off the extend split tool even though it didn't have to extend gave us the ability to actually split that body.
05:41
Now I can select all the other bodies inside of the browser.
05:45
I can right click and remove them leaving me with just this solid extrude that perfectly matches the underlying surface.
05:52
Any of this geometry can continue to be modified.
05:56
For example, if I want to add some small fillets to these corners,
06:02
or if I want to hide the surface all together and I want to shell this new body from the back side, giving it a 5 millimeter wall thickness.
06:10
I now know that that 5 millimeter wall thickness perfectly matches the underlying curvature.
06:16
So it's important to understand that because we had an open surface form body, it's now a surface body in Fusion 360s design workspace.
06:25
But that doesn't mean that we can't use it to help create the solid geometry.
06:30
At this point, I strongly urge you to continue playing around making adjustments to the model, adding new solid geometry,
06:37
and just seeing what you can do with it.
06:39
But from here we're going to save this design before moving on.
00:02
Working with a form as a BREP.
00:05
In this video, we'll use flatten and split body.
00:10
In Fusion 360, we want to carry on with our car hood.
00:13
We're going to begin working with it as a BREP.
00:16
But first let's take a look at a couple other tools that we have access to.
00:20
Under modify, there are many tools in here that can help us simplify the underlying geometry and potentially even create flattened sections.
00:29
For example, using the tool flatten.
00:31
It's important to look at and play around with all of these different tools to make sure that you understand their functionality.
00:37
In the case of the car hood, tools like smooth, pull, flatten and even straighten can be very handy.
00:45
Let's take a look at flatten.
00:47
Flatten allows us to fit, use a selected plane or make it parallel to a selected plane.
00:55
This allows us to make selections and create an average distance between them.
01:00
We can select a plane and pull geometry directly to it or we can be parallel to a plane.
01:07
When we do this, we can also use either control points or surface points.
01:12
The difference is the surface points will get pulled to the selected plane but the underlying geometry might be problematic.
01:19
Let's take a look at an example.
01:21
Let's use surface points first and we'll select the plane as our YZ plane.
01:27
When we start to select vertices, for example, inside of this grill area, notice how the geometry changes based on our selection.
01:37
If we change from surface points to control points, notice that we're actually getting closer to a flattened section inside of that area.
01:46
It's important to understand that the control points are creating the geometry or the underlying curvature based on their position.
01:55
But when we use the surface points, it can be problematic again because what we're really saying or what we're really doing here is,
02:03
we're taking the exact surface and we're moving it forward or parallel to a plane.
02:09
So it's a good idea to play around with these options and see if one works better than the other for your specific geometry.
02:16
If we needed to have a flat cooler or radiator mount here and we needed a flat section,
02:21
this could be a reason why we might want to flatten the grill opening.
02:25
If we don't like the way the grill opening actually ended up being created, we can select all these faces.
02:31
Use modify edit form and push it a little bit deeper into the car.
02:35
That way, that flattened section is a little bit farther back.
02:40
Now that we've played around with some more tools, let's finish the form.
02:43
Let's re show the body and take a look at the updates.
02:47
Everything looks pretty good from here.
02:49
Our crease on the edge is fine and we've got this flattened section even though it rolls back into those corners.
02:56
But now that we have this surface as a BREP, what can we do with it?
03:01
Let's begin by creating a sketch.
03:03
And in my case, I'm going to use the YZ plane and I'm going to start with a center point rectangle.
03:08
I'm going to make sure that I start below the origin and I'm going to place this about in the middle of my grill opening area.
03:16
I want to make sure that I have a vertical constraint between the center of that rectangle.
03:21
And then I want to begin using my sketch dimension tool to make sure its position is in this case 95 mm down.
03:29
I'm going to set its width 235 and I'm going to set its height to 30 mm.
03:38
Now that I have a sketch in relation to the grill opening, I could use that sketch to trim the surface.
03:45
I could use it to create an extrude that goes from or to a surface or I can use it to split the face of the surface.
03:53
In my case, I'm going to start by creating a solid extrude.
03:58
The solid extrude is going to come all the way through the geometry.
04:01
And the reason I'm doing this is because often times it's hard to find a good reference for where things need to be,
04:08
and you sometimes will create a reference such as this extrude that you can use as the basis for other features.
04:16
In my case, I'm going to go to my surface tools, go to create and select offset, select just this face.
04:24
I'm going to offset it forward 20 mm and say, OK.
04:28
When I offset at 20 mm, I'm then going to use the split body tool.
04:33
The body to split will be that rectangular extrude and the splitting tool will be that offset surface we just created.
04:40
This is going to leave me with that offset surface body and body 2.
04:46
And I can simply remove those.
04:49
The next thing that I might want to do is I might want to remove the geometry on the back side.
04:53
Once again I can use things like split body to get rid of that geometry.
04:58
Bodies to split will be this rectangular section and the splitting tool is going to be that surface.
05:06
Once again I could get rid of that body in this design but you'll note that this one didn't actually end up being split.
05:12
Sometimes working with these converted surfaces can be problematic and you might need to change your approach.
05:20
In this case, let's try split body one more time.
05:22
This is our body to split.
05:25
This is our split tool but we're going to turn off extend splitting tool and say OK and see if that allows us to split that solid body.
05:33
So turning off the extend split tool even though it didn't have to extend gave us the ability to actually split that body.
05:41
Now I can select all the other bodies inside of the browser.
05:45
I can right click and remove them leaving me with just this solid extrude that perfectly matches the underlying surface.
05:52
Any of this geometry can continue to be modified.
05:56
For example, if I want to add some small fillets to these corners,
06:02
or if I want to hide the surface all together and I want to shell this new body from the back side, giving it a 5 millimeter wall thickness.
06:10
I now know that that 5 millimeter wall thickness perfectly matches the underlying curvature.
06:16
So it's important to understand that because we had an open surface form body, it's now a surface body in Fusion 360s design workspace.
06:25
But that doesn't mean that we can't use it to help create the solid geometry.
06:30
At this point, I strongly urge you to continue playing around making adjustments to the model, adding new solid geometry,
06:37
and just seeing what you can do with it.
06:39
But from here we're going to save this design before moving on.
Step-by-step guide
