Fixture design

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In this video, we'll look at fixture design.

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After completing this step, you'll be able to create a sketch and create a feature.

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In fusion 360, we're going to carry on with our gear housing, front cover only.

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We're going to start by going back and activating the top level of the design, if front cover is still active.

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We want to start by creating a fixture to hold this part while we're machining.

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It's important to note that when designing or creating fixtures,

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there are a lot of different reasons or nuances in why you would make certain decisions.

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What we're looking for with this design is something that bolts to these five different bolt holes that we added,

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and has parallel sides so it can easily be held in a vise but is also smaller than the outside shape of our part.

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We want to be able to completely machine the outside shape while it's raised above of ice but held insecurely.

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So these are the criteria and remember that everything critical as machine from one side.

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So we don't have to worry as much about orientation with these bolts.

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But again, if that is a critical component,

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then your fixture should probably include tapered pins or something to positively locate it aside from the bolts.

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So what we're going to do at this point is we're going to start a new component.

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So from the assembled drop down, we're going to select new component.

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This will be standard and I'm going to go ahead and name it while we're here and this is going to be front cover fixture.

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It's going to be active and then we're going to simply start sketching, one thing that's also important is the location of the origin.

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When we take a look at this, the origin is already centered at the main bearing or the main boss.

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This is where the input and output shafts will be on this design.

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So I'm happy with that location but note that it's actually off from the cover.

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So if we want the origin of the part to match the origin of the fixture, then we want to go ahead and move this before we start designing.

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We can do that by going to move copy and selecting the option to move components,

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the components that we're going to move our front cover but there's no geometry there yet.

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So what we need to do is we need to select a point on its origin and we can use the point to point method.

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Then we can simply select the center point of the back of our part and then that's going to be our target point.

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So the origin and the target points are going to be a to and from.

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But we also have other options such as .2 position and we can simply do a free movie.

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So revisiting this, we are going to move our component which is our front cover fixture.

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And again we don't have any geometry, so I simply selected its origin but you could also select it from the browser.

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The origin point is going to be the point that we're going from which is going to be the origin of our fixture.

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And the target point is where we're going to which is going to be the point on our front cover.

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Once we're happy with that, we're going to capture its position and we're going to say, okay.

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Capturing that position simply tells Fusion 360 that we know exactly where this thing is.

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Now we don't really need to see the origin anymore because we're going to start sketching on the face of our front cover.

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Keep in mind that this is parametric, its history based.

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So if anything were to move before this point in time such as the origin,

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then the sketches, everything that we're going to do is going to update but nothing is going to move because we don't want it to move.

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So at this point we're simply going to start our new sketch noting that it's automatically going to bring this entire face.

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So if we wanted, we could hide the front cover noting that we still have that entire profile there.

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I'm going to keep the front cover visible,

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because it just helps when we're talking about visual representation and then we're going to begin designing the fixture.

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So remember that what we want is something that's offset but bolts to all these holes and allows us to machine all the geometry.

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This means that we need to be offset from these holes that are going to be the main bolting holes for the housing,

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and we also need to be offset from this outside edge.

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The amount that were offset doesn't necessarily matter, but we just want to make sure that we have enough clearance.

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So I'm going to start by drawing a circle and I'm going to snap it to the outside diameter.

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Just gives me a nice reference without having to add any dimensions,

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let me snap there and gives I believe it's a half inch circle, roughly half inch.

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So this gives us a starting point.

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Next I'm going to go to offset but first I'm going to turn off chain selection because I don't want to offset the entire housing.

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Going to bring this edge in distance of minus

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I'm going to repeat that by using my right click marking menu. Then it's like this edge down here and again minus .125.

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If we want to relate those two, we can always double click on this dimension and then select the first dimension and then hit enter.

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When we do this, what we're doing is we're creating a dimensional reference between the two.

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I'm going to enter that minus .125 value,

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because it does get a little tricky whenever we're talking about dealing with positives and negatives and offsets.

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But keep in mind putting that intelligence and your sketches can often be something that really helps when you have to update these designs.

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The next thing I'm going to do is create a two point rectangle.

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Going to start from the center of this whole and I'm just going to begin dragging this out and I don't really have an end location in mind.

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I'm just going to make it a little bit bigger than it needs to.

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Then I'm going to use my coincident constraint for this endpoint to the center of that whole last, that leaves us the overall dimension.

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So we can determine whether or not we wanted to snap to something else, or we can just give it a dimension.

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In this case, I'll use the dimension option from the center point to this edge. And we'll give it a value of 2.25.

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The reason that we have this is because it gives us a good idea of what the overall size of our stock is going to be,

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and it looks like a little bit over 3.25.

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So if we had a 3.5 inch piece of stock that we were starting with, we'd have plenty of material to use.

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At this point, we could go through and we could trim off some of this excess, but fusion 360 automatically knows that this is a close profile.

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And because really all we need is the inside this is going to be very easy for me to select to create our extrude.

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So from here, let's go ahead and finish the sketch and turn this into a solid body, we're going to use extrude.

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It's already selected so I'm going to bring it out a distance of a half inch.

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Keeping in mind that this is a new body inside of our front cover picture.

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This component means that it's not going to automatically try to join the two together.

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Once we say, okay, well notice that we have a problem.

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This bolt hole right here is not inside of the actual part.

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It's causing a problem because we've got that small amount of overlap.

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Now, if this is something that we need to deal with, then we can always go back to the sketch. And we can modify this offset value.

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Maybe a smaller value like .06 will give us enough material. I'm going to say okay.

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And you can see that it gave us a little bit back,

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but honestly that is probably not much that tells me that likely I want to go ahead and I want to move that bolt hole,

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because its location is not going to be okay for me.

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Maybe I can put it back here somewhere.

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But again, the great news is that we can do that by going to that other component.

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I can go back to the sketch that was used to create it,

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I can find that sketch and then I can determine whether or not or where I want those points to be.

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If we go back to a front view and we take a look at our whole feature and we take a look at the sketch points that were used to create it.

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We simply need to right click and edit that sketch.

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At this point, we can't see through the other elements because we did that with the display setting.

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So I'm going to go back to shaded with hidden edges and I'm going to change this to one inch.

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And then I'm going to push it out a bit farther .75 and then I'm gonna finish the sketch,

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notice that this automatically updates for me and everything looks fine.

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Now I'm going to go back to my shaded with visible edges, noting that I can use control or command and the number four or five on the keyboard.

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So let's go back and let's modify our front cover fixture and let's edit this extrude.

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The reason I want to edit this extruded because I don't need that hole in the center,

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so I'm going to hold down control or command, select that geometry and then allow it to fill itself back in.

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So at this point it's probably a good idea for us to go through and fill it or round off these corners.

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And at this point we also need to keep in mind that this whole is actually the size for a quarter 20 tap and not a quarter 20 passing hole.

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You see that it's .202 diameter.

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So that means we have a little bit more that we still need to do.

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So let's go ahead and just add a few fillets and around these corners off because anytime you're dealing with a fixture,

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you don't want to have these sharp corners.

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This is going to be something that people are going to be handling putting in and out of the machine.

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If we use a quarter inch fill it.

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It makes it nice and smooth and really we could just cut the corner off here but we're just gonna leave that geometry for now.

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And lastly we want to increase the sizes of these holes.

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So if I use press pull and I select these holes and I want to increase their size.

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We can just modify that value. We know we're at

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So that tells me that I need to go minus .048 and that should take us right out to quarter inch.

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If I select it, you can see that we're a little bit larger, which means that I added that to the diameter and not the radius.

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So I need to divide that by two. So I can do that directly in here.

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Just divide it by two and say okay, and then we can measure one more time. And that gives us a quarter inch hole.

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So now that we have these holes, you might also consider doing a counter bore or some sort of taper champ for a counter sink screw.

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But for the purposes of our fixture right now, I'm going to go ahead and leave them as is,

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I'm going to activate the top level and go back to a home view and then make sure I save this before moving on.