Transcript
00:02
Use symmetry and construction geometry.
00:06
In this video, we’ll convert sketch entities to construction, create a sketch mirror and add a symmetry constraint.
00:14
In Fusion 360, we want to carry on with our gear reduction housing.
00:18
We're going to get started by creating a new sketch once again on the front plane.
00:24
From here, we need to make sure that we can reference some of the values that we've already created.
00:30
We still have our layout sketch shown, but we're going to use the option to create or project them as construction geometry in our current sketch.
00:39
So we're going to select Project or P on the keyboard.
00:42
We're going to select each of these items.
00:45
Once we have them all selected we’ll say, OK, and then we're going to hide our layout sketch.
00:51
You'll notice that they're displayed in a different color.
00:54
They are still able to be used for things like extrudes solid geometry.
00:59
But what we've done is we've created them as a projection into our current sketch.
01:04
If we want to turn them into a reference only type of geometry, we can select them all and use the line type construction.
01:13
When we left click, you can see now that they're dashed and they’re projected but only as construction references.
01:20
This means we can no longer select their close profiles for things like extrudes.
01:25
This is a great way for us to bring specific sketch entities from other sketches or even solid geometry into our current sketch.
01:33
This way we can begin to create the layout of our housing assembly.
01:38
We're going to get started by using our center diameter circle.
01:41
Starting from the origin, we're going to begin dragging this out slightly larger than our projected reference.
01:48
We're going to draw a secondary one larger than that.
01:51
We're going to begin again by going to the origin and drawing a circle that comes to about 70 mm,
02:00
and we're going to draw one at the outside of our last or a third idler gear.
02:06
We're going to drag this one out and it's going to roughly go through the center of the second idler gear,
02:11
but we want to make sure that we don't actually snap to any geometry.
02:15
So this is going to be about 37 mm.
02:19
From here, let's go ahead and use our Line tool to go between these two sketch entities.
02:25
Once again, I'll zoom in to make sure that we're not creating any additional references.
02:31
And then if you accidentally select, you can right click and hit Cancel and restart your Line tool.
02:39
But we want to make sure that we're creating tangent references between these two outside circles.
02:45
We can add that as a constraint by selecting the line entities in the circles and we'll go ahead and do this for the bottom one as well.
02:55
This is going to be a portion of our housing that encloses the idler gears as well as our driven gear on the front side of our housing.
03:03
So in order to make it as aesthetic as possible, we're going to use these tapered lines,
03:09
and make sure that we can include enough geometry to encompass all of the various idler gears.
03:16
Now that we've got some of this laid out, let's go ahead and add some dimensions.
03:21
To get started I want to add a dimension to this inside circle here.
03:26
I'm going to left click to place the dimension and then I need to define what this is.
03:31
In order to do this, I'm going to start by having an open bracket,
03:35
and I'm going to start to type in my gear list so I can start to see what I have inside of my parameters.
03:43
So remember that we're dealing with the drive gear in this case, which is the largest gear.
03:48
So I'm going to select my Drive_Gear_Dia, which is 96 mm and I need to add to that.
03:56
So in this case, we have a parameter called gear clearance diameter.
04:01
That gear clearance diameter is 4 mm and that 4 mm allows us to have just enough clearance for the outside edge of the teeth of our gear.
04:12
Now, just enough is not going to be good for us.
04:14
We want to make sure that we have a little space, especially if this housing has grease or there's any additional components that go in here,
04:21
we want to make sure that we have enough clearance.
04:24
So instead of just simply adding that 4 mm we're going to say plus and add more brackets,
04:31
and this is going to be our gear clearance diameter value, which is 4.
04:36
And I'm going to multiply that by 2 and then I need two brackets to close this off.
04:42
Gonna hit Enter and this should give us a value of 104 mm.
04:47
So once again, we're using that gear diameter, which we know is 96 mm and we're adding two of our gear clearance diameters to it.
04:57
The next thing that we want to do is we want to define the size of this geometry here.
05:03
Now when we do that there is a couple different ways we can do it.
05:06
Once again, we can define it as a diameter or we can define it as a relationship to something else.
05:13
So in this case, I'm going to create it as an offset and this is going to be my gear clearance diameter value, which is 4,
05:21
but I'm going to multiply that once again, times 2.
05:24
What this does is it gives us an offset value of 8 mm between the radius of the circles.
05:31
So this gives us an overall difference of 16 mm, which is different than the 8 mm that we had for this value.
05:39
So now that we have those two defined, let's go around and let's add a few more.
05:46
This value here is something that we don't really have a parameter for,
05:50
we're just going to have to use some of the other parameters to help define it.
05:54
So we're going to start on the right hand side, go between these two.
05:58
Once again, I want to use the gear clearance diameter.
06:01
I'm going to multiply that by 2 giving me 8 mm.
06:05
Since I know that's not going to work on this side,
06:08
I'm going to use that same value, that gear clearance diameter but I'm going to multiply it times 4.
06:14
Once again, I don't really have a value for this because we're just creating a sketch that has enough geometry to encompass our idler gears.
06:23
So basing it still off of that original value means that any ratios that we adjust, if we modify the diameter of our large gear, our drive gear,
06:34
that means all these other values are going to update accordingly.
06:37
So that's why I want to make sure that I use a relationship to that gear clearance diameter.
06:43
Now that we have these set, let's go ahead and use our center diameter circle tool and let's add some center diameter circles.
06:51
I know that I want my input and output shafts to be 10 mm so I'm going to manually enter that value.
06:57
But then I want to place some more center diameter circles and these are going to be using our idle gear shaft values.
07:04
That's going to be an 8 mm value.
07:07
And again, we're going to just go ahead and place and click to place that.
07:12
And again, if you forget, you can always go back to your sketch dimensions, apply that dimension and then simply select the correct user parameter,
07:20
and hit Enter on the keyboard.
07:23
Now that we have our center diameter, the clearance for our shaft and then we have the shaft clearances for the various idle gears,
07:33
what we need to do is we need to create the mounting point locations.
07:38
In order to do this, we're going to use a center diameter circle and I'm simply going to place one in the bottom right,
07:45
and I'm going to place two at the exact same location.
07:48
I'm going to do this over here as well.
07:51
I'm going to place two at the same location, making sure that they are concentric.
07:55
And then I'm going to hit Escape on the keyboard.
07:58
In order to find the location of those, I'm going to use a line from the origin to the center point and I'm going to do the same thing over here.
08:07
I'll hit Escape and then I'll convert those lines to construction.
08:11
These are only going to be references for adding dimensions.
08:14
So I want to make sure that I create these references.
08:17
In this case, I'll add a vertical line.
08:21
We’ll OK, we'll hit Escape and then we'll convert this to construction as well.
08:26
So now we have a vertical reference and we have this angular reference here.
08:31
Since we left this under constrained, we can move it around if we want.
08:36
But in the end, it's not really going to matter where that line is because what we're going to be doing is creating a dimension from it.
08:43
So using our dimension tool going from our vertical line to this line here, we're going to drag it down and add a 45 degree value.
08:53
We're going to do the same thing even though these two are offset adding that same 45 degree value.
08:59
Another thing that we can do if we want to keep this as a relationship instead of manually entering it,
09:04
we can select the original 45 and hit Enter and this will create a link between the two values.
09:11
This means if I change this to 50 degrees, both of them are going to change.
09:15
Once again, using this type of modeling approach is helpful, especially if you want to maintain this parametric link.
09:23
Now we need to define what the diameters are going to be.
09:28
In this case, I'm going to select the inside and these are going to be our mounting bolts.
09:34
So we'll hit M on the keyboard and this is mount bolt and I can hit Enter for that and I'll do the same thing over here.
09:42
Mount bolts and we'll hit Enter for that.
09:46
Now we need to figure out the offset that we need,
09:50
because this is going to be the center of the bolt going through and we need to figure out how big the rest of this is going to be.
09:57
Well, we don't really know at this point, we haven't picked out hardware.
10:01
So I'm going to manually enter a value of 2 mm and I'm going to do the same thing over here but I'm going to select that original 2 mm.
10:09
So once again I only have to change it in one place.
10:13
So I'm going to hit Escape to get off my dimension tool and take a look at what I have so far.
10:18
Now that I've added a few different things,
10:20
I'm going to show a few more tools that can be extremely helpful when we're creating these parametric sketches.
10:26
I'm going to add a couple more sketch circles over here.
10:29
I'm going to hit Escape.
10:31
Then I'm going to take a look at my symmetry constraint.
10:34
When we have a symmetry constraint, we need to select our entities.
10:38
First, we're going to go our first entity, our second entity.
10:42
And then we need to select a mirror line and we don't have one in this case.
10:46
But if I select this vertical line, notice that it moves it all the way over here.
10:51
We do the same thing to the inside ones and then we select that vertical line.
10:55
What we've done is we've added symmetry across that line.
10:60
Let's hit Escape on the keyboard.
11:01
Let's create one more line and this time it's going to be horizontal.
11:05
We're gonna select it, convert it to construction and then we're gonna use the mirror tool.
11:11
This will allow me to select all of the different elements that I want to mirror.
11:16
And then I select my mirror line and say OK.
11:20
And now I've created all of those fully constrained and fully defined sketch elements that are parametrically linked,
11:27
meaning if I change this value to 4 mm, all of them are going to increase.
11:31
If I change it to 2, they're all going to decrease.
11:34
Let's make sure that we finish this sketch and take a look at what we've done.
11:38
We've added a lot of references, we've added a lot of parametric relationships,
11:43
which means that we can always go back to Modify, Change Parameters and we can make adjustments to any of our values.
11:50
Let's go ahead and minimize this so we can see.
11:54
If we take a look at our Drive_Gear_Teeth and I change this to 60, everything updates.
12:00
But you'll notice that there are some issues because of the tangency between our idle gears.
12:07
If I change it back to 48, notice that it doesn't go back to the original location but it does satisfy everything that we've done.
12:14
So making those adjustments can update our sketches but we do have to model in a specific way to make sure that all the updates take place.
12:25
Because the drive and driven gears have that 1:3 relationship, they'll update just fine.
12:30
But our idle gear was manually entered and that value does not change based on any of the other parameters.
12:37
So if we wanted to make a true updatable fully constrained parametric type assembly,
12:43
we would need to figure out some sort of relationship to get that 10 tooth gear in there based on the distance between two points or diameters.
12:53
I'm going to use Control Z to undo and put this thing back on the right hand side, how we designed it, and I'm going to save this before moving on.
00:02
Use symmetry and construction geometry.
00:06
In this video, we’ll convert sketch entities to construction, create a sketch mirror and add a symmetry constraint.
00:14
In Fusion 360, we want to carry on with our gear reduction housing.
00:18
We're going to get started by creating a new sketch once again on the front plane.
00:24
From here, we need to make sure that we can reference some of the values that we've already created.
00:30
We still have our layout sketch shown, but we're going to use the option to create or project them as construction geometry in our current sketch.
00:39
So we're going to select Project or P on the keyboard.
00:42
We're going to select each of these items.
00:45
Once we have them all selected we’ll say, OK, and then we're going to hide our layout sketch.
00:51
You'll notice that they're displayed in a different color.
00:54
They are still able to be used for things like extrudes solid geometry.
00:59
But what we've done is we've created them as a projection into our current sketch.
01:04
If we want to turn them into a reference only type of geometry, we can select them all and use the line type construction.
01:13
When we left click, you can see now that they're dashed and they’re projected but only as construction references.
01:20
This means we can no longer select their close profiles for things like extrudes.
01:25
This is a great way for us to bring specific sketch entities from other sketches or even solid geometry into our current sketch.
01:33
This way we can begin to create the layout of our housing assembly.
01:38
We're going to get started by using our center diameter circle.
01:41
Starting from the origin, we're going to begin dragging this out slightly larger than our projected reference.
01:48
We're going to draw a secondary one larger than that.
01:51
We're going to begin again by going to the origin and drawing a circle that comes to about 70 mm,
02:00
and we're going to draw one at the outside of our last or a third idler gear.
02:06
We're going to drag this one out and it's going to roughly go through the center of the second idler gear,
02:11
but we want to make sure that we don't actually snap to any geometry.
02:15
So this is going to be about 37 mm.
02:19
From here, let's go ahead and use our Line tool to go between these two sketch entities.
02:25
Once again, I'll zoom in to make sure that we're not creating any additional references.
02:31
And then if you accidentally select, you can right click and hit Cancel and restart your Line tool.
02:39
But we want to make sure that we're creating tangent references between these two outside circles.
02:45
We can add that as a constraint by selecting the line entities in the circles and we'll go ahead and do this for the bottom one as well.
02:55
This is going to be a portion of our housing that encloses the idler gears as well as our driven gear on the front side of our housing.
03:03
So in order to make it as aesthetic as possible, we're going to use these tapered lines,
03:09
and make sure that we can include enough geometry to encompass all of the various idler gears.
03:16
Now that we've got some of this laid out, let's go ahead and add some dimensions.
03:21
To get started I want to add a dimension to this inside circle here.
03:26
I'm going to left click to place the dimension and then I need to define what this is.
03:31
In order to do this, I'm going to start by having an open bracket,
03:35
and I'm going to start to type in my gear list so I can start to see what I have inside of my parameters.
03:43
So remember that we're dealing with the drive gear in this case, which is the largest gear.
03:48
So I'm going to select my Drive_Gear_Dia, which is 96 mm and I need to add to that.
03:56
So in this case, we have a parameter called gear clearance diameter.
04:01
That gear clearance diameter is 4 mm and that 4 mm allows us to have just enough clearance for the outside edge of the teeth of our gear.
04:12
Now, just enough is not going to be good for us.
04:14
We want to make sure that we have a little space, especially if this housing has grease or there's any additional components that go in here,
04:21
we want to make sure that we have enough clearance.
04:24
So instead of just simply adding that 4 mm we're going to say plus and add more brackets,
04:31
and this is going to be our gear clearance diameter value, which is 4.
04:36
And I'm going to multiply that by 2 and then I need two brackets to close this off.
04:42
Gonna hit Enter and this should give us a value of 104 mm.
04:47
So once again, we're using that gear diameter, which we know is 96 mm and we're adding two of our gear clearance diameters to it.
04:57
The next thing that we want to do is we want to define the size of this geometry here.
05:03
Now when we do that there is a couple different ways we can do it.
05:06
Once again, we can define it as a diameter or we can define it as a relationship to something else.
05:13
So in this case, I'm going to create it as an offset and this is going to be my gear clearance diameter value, which is 4,
05:21
but I'm going to multiply that once again, times 2.
05:24
What this does is it gives us an offset value of 8 mm between the radius of the circles.
05:31
So this gives us an overall difference of 16 mm, which is different than the 8 mm that we had for this value.
05:39
So now that we have those two defined, let's go around and let's add a few more.
05:46
This value here is something that we don't really have a parameter for,
05:50
we're just going to have to use some of the other parameters to help define it.
05:54
So we're going to start on the right hand side, go between these two.
05:58
Once again, I want to use the gear clearance diameter.
06:01
I'm going to multiply that by 2 giving me 8 mm.
06:05
Since I know that's not going to work on this side,
06:08
I'm going to use that same value, that gear clearance diameter but I'm going to multiply it times 4.
06:14
Once again, I don't really have a value for this because we're just creating a sketch that has enough geometry to encompass our idler gears.
06:23
So basing it still off of that original value means that any ratios that we adjust, if we modify the diameter of our large gear, our drive gear,
06:34
that means all these other values are going to update accordingly.
06:37
So that's why I want to make sure that I use a relationship to that gear clearance diameter.
06:43
Now that we have these set, let's go ahead and use our center diameter circle tool and let's add some center diameter circles.
06:51
I know that I want my input and output shafts to be 10 mm so I'm going to manually enter that value.
06:57
But then I want to place some more center diameter circles and these are going to be using our idle gear shaft values.
07:04
That's going to be an 8 mm value.
07:07
And again, we're going to just go ahead and place and click to place that.
07:12
And again, if you forget, you can always go back to your sketch dimensions, apply that dimension and then simply select the correct user parameter,
07:20
and hit Enter on the keyboard.
07:23
Now that we have our center diameter, the clearance for our shaft and then we have the shaft clearances for the various idle gears,
07:33
what we need to do is we need to create the mounting point locations.
07:38
In order to do this, we're going to use a center diameter circle and I'm simply going to place one in the bottom right,
07:45
and I'm going to place two at the exact same location.
07:48
I'm going to do this over here as well.
07:51
I'm going to place two at the same location, making sure that they are concentric.
07:55
And then I'm going to hit Escape on the keyboard.
07:58
In order to find the location of those, I'm going to use a line from the origin to the center point and I'm going to do the same thing over here.
08:07
I'll hit Escape and then I'll convert those lines to construction.
08:11
These are only going to be references for adding dimensions.
08:14
So I want to make sure that I create these references.
08:17
In this case, I'll add a vertical line.
08:21
We’ll OK, we'll hit Escape and then we'll convert this to construction as well.
08:26
So now we have a vertical reference and we have this angular reference here.
08:31
Since we left this under constrained, we can move it around if we want.
08:36
But in the end, it's not really going to matter where that line is because what we're going to be doing is creating a dimension from it.
08:43
So using our dimension tool going from our vertical line to this line here, we're going to drag it down and add a 45 degree value.
08:53
We're going to do the same thing even though these two are offset adding that same 45 degree value.
08:59
Another thing that we can do if we want to keep this as a relationship instead of manually entering it,
09:04
we can select the original 45 and hit Enter and this will create a link between the two values.
09:11
This means if I change this to 50 degrees, both of them are going to change.
09:15
Once again, using this type of modeling approach is helpful, especially if you want to maintain this parametric link.
09:23
Now we need to define what the diameters are going to be.
09:28
In this case, I'm going to select the inside and these are going to be our mounting bolts.
09:34
So we'll hit M on the keyboard and this is mount bolt and I can hit Enter for that and I'll do the same thing over here.
09:42
Mount bolts and we'll hit Enter for that.
09:46
Now we need to figure out the offset that we need,
09:50
because this is going to be the center of the bolt going through and we need to figure out how big the rest of this is going to be.
09:57
Well, we don't really know at this point, we haven't picked out hardware.
10:01
So I'm going to manually enter a value of 2 mm and I'm going to do the same thing over here but I'm going to select that original 2 mm.
10:09
So once again I only have to change it in one place.
10:13
So I'm going to hit Escape to get off my dimension tool and take a look at what I have so far.
10:18
Now that I've added a few different things,
10:20
I'm going to show a few more tools that can be extremely helpful when we're creating these parametric sketches.
10:26
I'm going to add a couple more sketch circles over here.
10:29
I'm going to hit Escape.
10:31
Then I'm going to take a look at my symmetry constraint.
10:34
When we have a symmetry constraint, we need to select our entities.
10:38
First, we're going to go our first entity, our second entity.
10:42
And then we need to select a mirror line and we don't have one in this case.
10:46
But if I select this vertical line, notice that it moves it all the way over here.
10:51
We do the same thing to the inside ones and then we select that vertical line.
10:55
What we've done is we've added symmetry across that line.
10:60
Let's hit Escape on the keyboard.
11:01
Let's create one more line and this time it's going to be horizontal.
11:05
We're gonna select it, convert it to construction and then we're gonna use the mirror tool.
11:11
This will allow me to select all of the different elements that I want to mirror.
11:16
And then I select my mirror line and say OK.
11:20
And now I've created all of those fully constrained and fully defined sketch elements that are parametrically linked,
11:27
meaning if I change this value to 4 mm, all of them are going to increase.
11:31
If I change it to 2, they're all going to decrease.
11:34
Let's make sure that we finish this sketch and take a look at what we've done.
11:38
We've added a lot of references, we've added a lot of parametric relationships,
11:43
which means that we can always go back to Modify, Change Parameters and we can make adjustments to any of our values.
11:50
Let's go ahead and minimize this so we can see.
11:54
If we take a look at our Drive_Gear_Teeth and I change this to 60, everything updates.
12:00
But you'll notice that there are some issues because of the tangency between our idle gears.
12:07
If I change it back to 48, notice that it doesn't go back to the original location but it does satisfy everything that we've done.
12:14
So making those adjustments can update our sketches but we do have to model in a specific way to make sure that all the updates take place.
12:25
Because the drive and driven gears have that 1:3 relationship, they'll update just fine.
12:30
But our idle gear was manually entered and that value does not change based on any of the other parameters.
12:37
So if we wanted to make a true updatable fully constrained parametric type assembly,
12:43
we would need to figure out some sort of relationship to get that 10 tooth gear in there based on the distance between two points or diameters.
12:53
I'm going to use Control Z to undo and put this thing back on the right hand side, how we designed it, and I'm going to save this before moving on.
Step-by-step guide
