Modern speaker

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Hey everyone, this is Daniel for Shapr3D. In this tutorial, we'll see how to create this modern speaker design with a lot of pattern features, linear pattern, radial patterns. We'll also take a look in how to use mirror features, and also we'll utilize the isolate mode quite a bit in this video. So I hope you're excited, and let's get started. OK, I'm here now in this new file. And the first thing, of course, is to name it accordingly.

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The next step is just to make sure that we have all our snapping tools and features on, because I like to work with them. Right, and also we are in the millimeter units. For our first step, let's just go ahead and create our sketch from the top view, and we'll create a center rectangle. So if you don't see center here, just double click or highlight and go down into this drop down menu.

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and then select the center rectangle from the menu. And then since we have snapping on, let's just go and highlight or hover over the center point roughly and then create our rectangle. And that makes sure that our center of the rectangle is also the center of the axis. And to make sure that it doesn't move whenever we add any dimensions to it, let's also click Lock in order to lock the rectangle in place.

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choose our dimensions. So let's highlight one of the lines and then type in our dimension. And that would be 150 millimeters in both directions. So we have a nice square. And that's it for our first sketch. So let's exit and then highlight this area and just pull it up. So it already understands that we want to extrude our rectangle. And with these arrows, we can just choose the direction. And then also we want to

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calculate how high we need to extrude it. So let's calculate 150, which is the width of the rectangle, plus half of the 150, 75, equals 225. So this calculator is very handy, and it will pop up any time you enter any dimension. So let's select that, and that's our first volume. So now we need to divide this volume into the different sections.

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So first thing is highlight the front face, go to Sketch, and then we'll create a rectangle again. And this time, let's double click again and click or select the diagonal rectangle. And then make sure that we can go from the left edge to the right edge and already constrain the rectangle to these edges. And if it doesn't constrain automatically, if you don't see those icons, go to Constraint Settings.

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and then activate auto-constraining. So now we just need to highlight those two edges and again, select our 150 millimeter distance to make sure that this equals a square. And then also, we can go down to the height of the rectangle and just put in a very tiny amount, 0.2 of distance. You can see that this is a very, very tiny rectangle, a flat rectangle. But.

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What we do is if we exit, we can select this and just push it through to the other side. And now basically divide our volume into two elements. So now if we go to the items, you can see that we now have two separate bodies. And that also creates a nice realistic look, because in reality also no two volumes or elements will touch with zero distance.

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it will already make it quite realistic. And then as the next step, we want to do the same thing with the lower part. So select the surface, go to Sketch, and again, we'll create a rectangle. But this time, I'm going with a center rectangle. And then go from this projected center here of our rectangle to one of these edges. I'm selecting the lower because it's easier to grab. And if you don't see these helping lines, make sure that they are on here and showing.

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guide points as well as snapping hints. And now the only dimension that we need will be the width of the rectangle. So again, point two. And it's already constrained into the center. We can make sure if we zoom in that the blue line, which is the center line or a set axis, is exactly in the center of these two edges. Now exit the sketch, highlight a rectangle, zoom out. I'll just move in 3D in order to see this.

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arrow and then just push it through all the way. We don't really need a dimension here or a constraint because we'll just push it through all the way. Then deselect and make sure that we now have three different and separate bodies. In order to not confuse any of them we can also rename them.

05:18

So now we have our volumes renamed accordingly. OK, let's start with our top volume and create the features for this one. And in order to make it easier to work with, we can click Isolate to basically hide everything that we don't need. So all the sketches, all the other volumes are now hidden, and we have entered this isolation mode. So now that we are in the isolate mode, we can select our front surface.

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and then start our sketch for the pattern. So let us move to where it's the left upper side and then create our first circle. So the circle, we just draw and select our diameter and we can change that later on. So let's just set it at eight. And also we want to constrain it to the top left side. So let's constrain the top dimension and also this distance.

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to 15 and now if we want to move the circle it is telling us it can't move because it's locked and constrained. So now we can start with our pattern. So it is selected. Let's go to the pattern tool and make sure it's linear. If it's not linear just open the drop down menu and then select the linear pattern from here. Now let's create the first direction with the arrow pointing to the right.

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And we have the decision between total distance and spacing distance. And I like to work with the spacing distance because then I can basically decide on the distance between the two circles. So spacing distance of 10 millimeters. And now we need to decide on the quantity. I know that 14 circles would make the whole row. So we need to duplicate it 13 times. And the same thing for the other dimension. So let's go with.

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10 millimeter here as well and a quantity of 13. And that will fill our whole area. So this could be our first pattern, but as you saw in the beginning, we had a little bit of a different pattern. We had the stacked circle pattern. So that means we would need to add another circle and another pattern here in the center between those four circles. And to do that, we also need to add a little bit more space. So.

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Let's change our diameter for the circle to 6. And then that would create a little bit more space for the new circle. Next, I'm going to highlight the circle and then go to Move and Rotate in order to move or copy this circle to the new position. For just one to move, it tells us, can't move it because it is constrained and locked. So that means we need to highlight Copy in order to create a new circle.

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copy of that first one and we'll actually create two. So basically one to the right and one to the bottom and our first copy we can actually delete. We don't need that one. So now we have our circle in this area in this free space. So it is a new circle and it has the six millimeter diameter but itself can move so we need to constrain it to something and let's constrain it to the first

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this 5 millimeter distance to the right and to the bottom. And to do that, we need to change the dimension from a direct dimension to a horizontal. So 5 millimeter horizontal, and then also 5 millimeter vertical. And that means now that our circle is locked and we can't move it. Another thing we can do is we can also relate the circle's diameter to the first circle. So let's.

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click on this lock icon. And now the diameter of the second circle is unlocked. Now we can highlight both of them and go to our constraint settings and set them to equal. That means I now just need to highlight and change this one diameter of our first circle in order to also change the second one. Now we are able to create our next or second pattern. So let's go to the linear pattern as well again and.

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Go to the right, 10 millimeter spacing, and a quantity of this time, 12, because we're missing one. So let's go 10 spacing. So the quantity of 12 would fill our row. And then the same thing with the other dimension, so spacing of 10 and quantity of 12. And that creates our complete pattern. So let's exit the sketch. And now we need to push.

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the pattern into our volume. But first, we want to change one thing. Currently, this volume is solid. And what I want to do is I want to have a core and an outer volume. So before we do anything, let's select our lower surface and then go to Shell. And then just select a 3 millimeter thickness. And that creates a hollow volume.

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that we now can basically push our pattern through. So in order to cut the pattern, it would be quite inefficient to select all of these areas separately and then do an extrusion. So what we can do is just move out, go to Tools, select our extrusion tool. If we go from the front, we can now click somewhere outside to the left, and then hold and drag.

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the selection rectangle over all of these circles. And since we go from the left to the right, this area selection selects only the things that are inside the rectangle. And since we are in the Extrusion tool, it also doesn't select any edges. It only selects those areas. So now when we go into 3D, you can see our handy arrow tool, and we can push the pattern into the center.

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Let's make sure that it's definitely pushing through. So minus 5 should do the trick. So this is our pattern done. But now our core is missing. So to do that, let's go and select these four edges. Then go to the offset edge and just offset this 2 millimeters to the center. And we'll just create a new volume in the inside.

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Make sure that it covers all of the holes. And let's, I think we can go for 145. Just make sure that it's not intersecting with our volume because if we do that, you can see it would push through and we don't want that. So let's make it small enough. So it's just in the center. And we can make sure if we go to the items that we have this center body, body four, now as a separate item.

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You can also just rename that core. All right, that's it for the pattern. We still are in our isolation mode. So let's quickly create our four screws that we had in the top. So select the top surface, go to Sketch, and we again go to one of the edges and one of the corners. I'll go to the left upper corner. And then we'll create a circle. And similar to what we did with the pattern, let's just create the circle.

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and select a diameter. What I also want to do is highlight the circle, create an offset. And that offset is, again, a very tiny one of 0.2 in order to just create the separation between the screw and the volume. Since we are in this sketch already, let's also create a hexagon. So go to Polygon and make sure we are at the hexagon. And create a hexagon from the center with a radius of 3.

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Now we can exit and zoom in to select this outer ring. And we can now push that in at least 3 millimeters, so minus 3, in order to separate. So we're going to push through the hallway and separate the housing from the screw. So deselect and make sure that in our items, we now have two volumes. So basically, this one is our new screw. And this is our top volume, the original one.

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So again, we can rename that screw. And as a detail, of course, we want to push in this hexagon about 2 millimeters. And that's our screw done. Of course, we want to mirror or make a pattern again with this screw in order to put it into all of the corners. In order to do that, let's unisolate everything for now, because then we can also get rid of all our sketches that we had. So all the sketches are now.

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hidden. So for the next part we go to Transform, Mirror, select our screw and also select the outer surface, so basically the cutting surface that we made. And now just zoom out where you can find this y-set plane. So it will mirror to one direction now. You can see if we zoom in that looks perfect. So it already cut out with our outside surface.

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and put in this new screw. And the same thing we need to do now a second time. So again, mirror with this first screw and also the outside surface and this screw and this surface. Just make sure that you don't select by mistake any plane. That would be the mirror plane. So select or unselect it again by clicking again. And make sure that we now select the right plane.

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That would be the XZ plane for the mirror plane. So that's done. We now have four identical screws mirrored to two directions. Now what if I wanted to add some details to the screw? Let's go to the history. And we have our extrusion, which is the last extrusion for our screw. Just click and hold and insert a breakpoint. So basically before our two mirrors. So we now are.

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in the history back to where we had our screw finished. What we can do is go to our screw, highlight it, and isolate that one. Go to our tools and find the Chamfer Fillet tool, and drag select all the edges of our screw. We'll just add a point to fillet to that screw to all the edges of that element. Sick, done.

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And now if we unisolate everything and also go down with the break point, either delete it or just move it down to the last part of the history, we can now see that all the screws, all the four screws that we had are filleted. So if I forgot to create any detail, you can always go back in history and the features will update accordingly. Perfect. So now for the next part of our design.

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we want to focus on the knob. So the left side, the left lower part. And again, we can go to items and find this bottom left part and then also click on isolate in order to make it a little bit easier for us to work with. So now we can select our front view and create a new sketch. And as I said, make sure to show the guide points and snapping hints in order to have those pink or magenta dots.

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And that will help us create a circle from the center. So you can already see it's centered and we can create our dimension. Let's go with 30 and that's it for our initial sketch. So let's exit and we need to extrude our knob. What I can do is I can extrude the knob but make sure to click on the small icon in order to select new body. So now the selection or the extrusion is not combined.

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not being combined with our original volume. So deselect everything. Now we can check if we have this new body. Yes we do. And keep it selected and just move it away from the body for one millimeter. So that's our initial volume for the knob. Now again we can unisolate, go to our items, select our body and isolate that. So now we can work on the details of the knob.

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without being distracted by everything else. So select the front face, we go into the sketch again, and we'll create a line from the center point, which is conveniently placed here, to the edge. Select the line and make it a construction line. Now let's zoom to the top and we'll create a new polygon, but this time double click and create a triangle. So from the center, go down along this edge.

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So now it's already constrained on the center and also on the edge. And we can select a radius of two millimeters, maybe even less depending on how deep you want these cuts to be. So now we have this triangle, which will be our cutting element. Before we cut anything, you sometimes see, or oftentimes you see knobs having chamfers on the edge in order to make them less sharp on the corners. So let's select those two corners and then draw.

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Inwards in order to make a chamfer so we can create a small one millimeter chamfer and click away to Confirm that now we want to zoom in and select both of those elements of the triangle Let's zoom in here and push that all the way down to cut the volume next We want to click on this center edge and just make them a little bit less sharp. So 0.23

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millimeter radius. So now we want to rotate this around the whole diameter. So let's go to the Transform Tools, go to Pattern, and then select the circular pattern. Now we want to highlight those three surfaces and move the center of the circular pattern into the center of one of these circles. So make sure that it's centered at least

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And now we can go and select our total angle.

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of 360 degrees and our quantity we can play with. So let's go with 30 and see if that's enough, maybe a little bit more, maybe 40. So let's go with 40 and hit done. So now we have our knurling pattern. And as before, we can go to the tools, go to Jamf Fulfill it and select all of these newly created edges that we have. And give them.

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0.2 millimeter radius in order to just make everything rounded over. So now that we're done with our knob we can unisolate everything and zoom out to see our creation. Right now that we have finished two of the three elements of our speaker we can move on to the next one and you might already know how we'll continue. We'll select this remaining part so we can

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Again, go to items and find our bottom right. Or we can also just double click and then go to isolate. And again, we'll create a new sketch. But this time, let's add a new sketching plane. So let's add a construction plane. And we'll just create a mid plane between those two elements. So we will make sure that the construction plane is in the center of our volume. Hit done. Now we can select our

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sketching plane and sketch on that one. So let's start with a line on our sketch and I need also my edge here. So let's project this edge, hit done and then click the starting point of our line and our edge and then select midpoint constraint. So now this line is in the center of our projected curve. Next we'll make it a construction and we'll just select this

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end point and make our line a little bit longer. Next, we want to just rough in our switch contour. So just create two circles and we'll connect the circles with a line. Make sure that the end of the line is also on the circle. And we'll also create a new line, which goes from one side of the circle to the other. So basically just crossing the whole sketch.

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and will not make this a construction line. Next, we want to make this line tangent to our circles, and hit Tangent. And here you can see that the circle that we created wasn't connected to the center line. So let's fix that, select the center point and our line, and hit the Coincident constraint. Now we need some measurements. So let us choose a appropriate diameter for those two circles.

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Let's go with 12 and this one can be also 12. And as I always say, you can choose to change it later on. So just when we're finished, we can go into the history, into our original sketch, and then change any of these dimensions. Next, we want to angle this line. So first of all, we can create a new dimension between the two circles. So let's make that a round number.

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And then we need to decide how steep this angle is. So let's select this line and then also our center line. And you'll see that we now can create a angle dimension. So let's go for 10 degrees. And now since we only need half of our switch, we can go to Trim and basically trim away everything that we don't need. So basically this is our contour. And last is to dimension where

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this will start. So what we need is basically this point to stick out of our volume for a few millimeters. So maybe two. All right, that's it. So we can exit our sketch. Now we're out of the sketch. Let's make sure that we create a new body. So we don't want to, since it's intersecting with this volume, it will combine these two volumes as soon as we

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revolve it. So let's go to the isolate mode and then select our sketch. That's the only one that we need right now. So isolate this one. And now we can revolve the whole part without combining any volumes. So we'll make sure that it's on part. Deselect everything. We can now go out of isolate. Now we want to make sure that this is a separate body. And as I said, you can always go in.

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into the history, into our sketch, and then play around with the dimensions. So if the whole thing is a little bit too big for you, you can change those dimensions, exit the sketch and now we're already updated. So now one more thing. We'll just put a fillet on this part on this edge and our switch is done. So what we can do is hide the sketch and also hide the plane.

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And one more step for the switch is to create a socket that the switch is in. So for that, let's select this front surface, create a new sketch. And as you can see, we already have this handy center point here because we'll create a circle and make that as big or small as you want. So let's go with 20. And this is all that we need. So let's exit and we'll select this area and extrude it out.

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Now make sure that it's going to be a new body. So it shouldn't intersect with anything. It should be its own body. And click somewhere to confirm. Now we'll select this front surface again and hit Shell. Our shell thickness should be 0.2. I think you might know where this is going. So now we have this piece, this element. What we can do is we'll move that backwards and basically use it as a.

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cutting object. So let's select this and this part and then go to Subtract. Hit Done. And you might be able to see that we now have created a solid piece here, a plug basically, that was created from our original volume. And the last step is to create some space for our switch. So what I'll do is double click our switch and then go and then use our Transform tool.

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hit copy, just move it up and down in order to basically end up at zero again. So now if we go into items, we'll have this body twice. So body 10, which is our switch, body 10, one, we can now hide the original one and just select this surface and just offset this face also 0.2 or 0.5. And that basically gives us

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a new solid that we can subtract with. So again double click this solid and this part and then go hit subtract and done. And now you can see that we created the socket for our original part.

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Now, original part is just that tiny amount smaller. And now it sits neatly in that cavity. What we can also do is select this edge and go inwards in order to create a small chamfer. And the last thing, if you want, is we can isolate our part and move the transformation origin to the center of this ball joint. And now.

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We can rotate around this ball joint. And we'll just move it 30 degrees to the up position, deselect, and exit the isolate view. And now you can see it's in the upper position. All right, so that's almost it. Let's put some final steps or final touches. We already have put some small radii on these details.

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part, so the rotary dial and then also our screws. But the rest still has some hard edges. So let's do the same thing. Isolate one of the parts. Then go to Tools, Chamfer Fillet, and then select every single edge. And we'll create a 0.2 radius or fillet onto all of these edges. So now when you zoom in, you can see

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Each one of those has their own soft edge. So hit Done. Now isolate off. We will do the same thing with this one. Isolate. Go to Jamf Refill It. Select all of these, 0.2. Isolate off. Isolate on.

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All right, so now you can zoom in and see that all of these edges have a nice radius or fillet. So now we are ready to put some materials on them and can make that quite fast. So I'll just choose a matte ABS material for these two. So let's make a black one and then also a colored one, as we had the orange color.

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anodized metal for these elements. Let's go with black. And I'll not just go with 100% black, because as you can see, the reflections are a bit nicer when it's not 100% black. And we'll just use this anodized material for these other parts as well. And I'll also use them for the screws.

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And then we'll go to plastic again and scroll down and find the matte transparent polypropylene, which has a really nice effect to it. So let's choose bright orange for that. And the last part is our core, basically where the speaker parts will be. So let's hide the top volume, which is the outer part. And then...

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We'll put a new ABS material on that and make it a brighter orange. So desaturate it. And now the top volume is not as dark. And if you zoom in, you can see these nice highlights because we put the soft edges everywhere and that makes everything look nice and realistic. So that's all for this tutorial. I hope you learned something.

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and enjoyed creating this modern speaker design in Shapr. So thanks for watching and we'll see you next time.