Create extruded cuts

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Create extruded cuts.

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In this video, we’ll create an extruded cut, project a sketch into a sketch, end an extrude at a face and use Combine to add bodies together.

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In Fusion 360, we want to carry on with our gear reduction housing solids.

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The first thing that we're going to do is we're going to roll back the last extrude cut that removed material from the front housing.

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I'm going to create another extrude by selecting extrude and selecting the front face.

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We're going to go to the Gear_Housing_Thickness.

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So when we take a look at this, you'll notice that as I type in the letter G, even though Housing_Wall_Thickness doesn't have a G in it,

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I can still navigate through all of those parameters.

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I also want to make sure that this is a new body as it will be a cover that gets bolted on.

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We expand our Bodies folder.

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Now we have a Body 3 and we can roll the end of the timeline back past that extrude cut.

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There are many other areas where we need to begin removing material.

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So I'm going to start by hiding Body 2.

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And I'm going to take a look at this face and begin removing some material.

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If we take a look at our sketches and our housing layout sketch, we already have a sketch in here that will allow us to remove some of this material,

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but it's not complete yet.

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So I'm going to get started by creating a new sketch on this face by selecting it, then right clicking and creating a sketch.

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Then I want to bring back my housing layout sketch and I'm going to use P on the keyboard to project some of these sketch entities.

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I'm going to bring in the outside diameter of the bolt hole locations.

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I want to bring in the diameter of the inside of this cut that we're going to remove.

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And I'm also going to bring in some of these outside diameters inside this small area and I'm going to bring in this edge as well.

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I'm gonna say, OK, and then I'm gonna come through and use offset to bring this edge in and it's going to come in a value of 4 mm.

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But I'm going to use the minus sign and I'm going to add the Gear_Gap parameter.

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The Gear_Gap parameter right now should give us enough offset inside of here.

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We can validate this by taking a look at the original layout sketch for the position and the size of the gears.

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Remember that these values are actually the pitch diameter so it's in between the teeth.

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We're not 100% sure if this is going to be enough room.

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We can always go back into change parameters even inside of the sketch, we can take a look at some of the values that we have.

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You'll notice that our Gear_Gap right now is 5 mm.

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And if we take a look at some of the other parameters that we have,

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you'll notice that our gear thicknesses in here at 8 mm and our housing wall thickness is 3 mm.

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So what I'd like to do is come back and modify this value and this is going to be our minus Housing_Wall_Thickness value,

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which will give us a little bit of a smaller offset.

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We're going to use that value for now, but note that we might have to come back and change it.

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We're going to go back hide the original layout sketch in the housing sketch to take a look at our results.

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What we want to do from here is finish our sketch and create our extrude cut.

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We're going to take this inside area as well as some of these other areas that we've created and begin dragging them backwards.

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As we do this, I'm going to enter minus and then we need to use our Gear_Thickness value.

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So the Gear_Thickness value should be 8 millimeters.

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And if we say OK, we can validate that by going to Inspect and taking a look at the depth from the top face to this bottom face,

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and noting that it is 8 millimeters.

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So everything there looks good.

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Obviously we will need to make some adjustments to the housing,

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but this is giving us a good start to make sure that we have enough room or clearance for those gears.

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Once we actually create our spur gears, we’ll be able to see a little bit better the different areas that we need.

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We can always go back into any of these sketches and make adjustments as necessary.

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For example, if I want to use project by hitting P on the keyboard and bring in this edge here and then offset that edge,

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making sure that Chain selection is turned off,

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I can bring this one in that same minus 3 millimeter distance and we're gonna use that Housing_Wall_Thickness value and say OK.

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Using my right click marking menu, I can repeat that.

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This is going to be a minus Housing_Wall_Thickness value on this side as well.

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And those lines can be extended out until they intersect this projected edge.

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They can do that by simply drawing a new line that is co linear.

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Depending on which constraint gets automatically applied, you might note that it's parallel or co linear,

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and you'll notice that it looks like it extended it for us.

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We're going to finish the sketch, modify our extrude cut,

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and we can come back and we can re select some of these areas that we also want to extend and remove.

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By hiding Sketch 5, you can see that looks a little bit cleaner and gives us that consistent wall thickness.

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We view this from the front and pull it to the center of our screen.

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We've now removed a large amount of material from the center of this back portion of our housing.

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If we bring back some of the other bodies,

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you'll notice that now we have room for gears on the front side of this which will be our driven and idle gears.

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Our long idle gear will go through the front of this housing all the way to the back housing.

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And this other piece is simply going to be a cover,

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and this will give us a position to have a counter bore for things like a shaft that runs through some of those gears.

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There are other areas that we need to remove.

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So let's hide Body 3 and show Body 2 and let's start a new sketch.

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We're going to use a center diameter circle and set this to 21 mm.

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I'm going to say extrude cut, I'm going to begin dragging it back, but I'm going to change this to go Through All.

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Objects to cut will be both of these bodies and we'll say, OK.

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Now I have space to mount the 21 mm bearing on the inside of that housing and some room on the back side of this housing.

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We will need to add some additional material because the bearing is thicker than the wall housing.

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If we bring back Body 3 and we right click on that feature that we just created, we can make it go symmetric or two sides.

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And the second side, we can drag it forward and set the distance to Through All, allowing it to cut through all three portions.

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Notice in the preview that it's not showing it cutting through.

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And that's because when we modify this feature, we need to make sure that we include Body 3 as one of the objects to cut.

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Because it was originally hidden for the first extrude, it's going to automatically be excluded.

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So you need to make sure that you toggle that option on if you want to include it in the extrude cut.

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Let's go ahead and add some additional geometry to the front of the housing to hold that 21 millimeter bearing.

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If you remember from the McMaster-Carr website, this 21 millimeter outside diameter bearing has a 5 millimeter thickness.

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If we take a look at inspect and we figure out the thickness of this housing, it should match 3 mm,

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which was the housing thickness value that we used.

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So we're going to start a new sketch on this front face.

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We're going to select Create Sketch and using our center diameter circle,

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we're going to create a center diameter circle that's larger than the housing based on the Housing_Wall_Thickness.

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We can do this by adding a dimension and begin to type H for Housing_Wall_Thickness.

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And now we have a 3 mm thick section.

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I'm also going to use a center diameter circle in the middle and this is going to have a 10 millimeter diameter.

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This is the size of the shaft that we need on the input and the output side.

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We're not necessarily going to use all of these in the same position, but we're going to make sure that it's all included in this one sketch.

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Remember that we have 3 mm of the wall thickness here and we actually need to have 5 mm for the bearing.

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So we're going to create an extrude.

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We're going to just take a look at this wall.

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We're going to extrude out a distance of 2 mm, which will give us the complete 5 mm for that bearing.

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I'm going to create a new body here and say OK, and bring back that last sketch.

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Next I'm going to create another extrude, which is going to include both of those regions.

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To include both of these regions, it might become problematic if you have other geometry.

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So sometimes you might have to hold control or command down in order to re select that geometry.

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What we're going to do from here instead of cutting is we're going to start at an object.

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So we want to start it at the end face that it's trying to remove.

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Notice that the extrude cut is automatically removing that face, so we need to reverse the direction.

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We're going to set it to a new body and then we're going to pull it out a distance of wall thickness.

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So using that Housing_Wall_Thickness and creating that new body then hiding the sketch,

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will give us these three separate body sections and now we can use Combine to join them together.

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These could have been done as a joint in the extrude, but sometimes it can be helpful to create them in their own sections.

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And that way we can go back and use Combine later on.

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I'm going to use Inspect and Section Analysis quickly.

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I'm going to hold down the left mouse button and select my YZ plane to quickly take a look at what we've done.

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I'm not going to save my section view but I want to note that we have a 5 millimeter section here, we have our 3 millimeter wall thickness.

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And this helps us include that 21 millimeter bearing and it has the 10 millimeter opening for our input and output shaft.

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So I'm going to say Cancel on the section view so that I'm not saving that analysis just yet.

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And I want to make sure that I do save this design before moving on to the next step.