Build a Parametric Clamp with Driving Sketches

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Welcome to another Shapr3D tutorial. My name is Andrew Cameradella. I'm an industrial design consultant and adjunct professor at DePaul University. In this tutorial, we're going to focus on creating a set of well-defined and constrained sketches that allow us to drive a set of features and bodies in order to create parametric relationships between components within the workspace. In other CAD software, assemblies are traditionally used to create the relationship between components.

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And we'll create those mechanical relationships within Shapr3D using a set of parametric sketches called driving sketches. Sometimes these are also called skeleton sketches. While there aren't any explicit assembly features inside of Shapr3D, we'll use these driving sketches alongside the unique mix of direct modeling and feature history to create a mechanical assembly that we can move around and preview within the workspace. For this tutorial, we're going to recreate a mechanical screw clamp

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where we'll primarily use sketches and alignment features within Shapr3D to create a movable model that maintains the relationship between all the components. Let's dive in. We're going to start off with a blank project here, and I'm just going to quickly rename this to Skeleton Sketch. And I'm going to import a drawing here so that we can take a look at what we're working with with this mechanical screw clamp. So I'm going to click on Image.

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I'm bring in that clamp and I'm going to make sure that this is scaled roughly. So there's 10 blocks on the side here, which are half inch blocks. So I'm just going to say 25.4 times five inches. And there we go. And we get our clamp scaled roughly to the correct dimension.

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I'm also going to line up this center pivot point here with the origin of the workspace. And I'm going to click done. I'm also going to turn this opacity down to about 50%. That looks pretty good there. And I'm going to start sketching. So the first thing I want to do is start to sketch out these pivot points. So we have our central pivot point here, and that's going to

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be a circle there. I'm also going to bring out this other pivot point here, along with this other pivot point here. And as I create geometry here, I'm going to also make sure that I'm setting constraints and geometry that's going to help drive the sketch here. So I am going to create some additional construction geometry here. And I'm just going to use that to help me define some of these other

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And I have these two circles here, for example, are equivalent. So we're just going to say equal. And the other thing I'm to do here is I'm going to set this to five millimeters. And you'll notice that when I have a fully constrained sketch entity, it's going to turn green. So this circle here is now centered on the origin and has a five millimeter diameter, whereas these other elements of the sketch here are still floating around. I can

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click and drag on those elements to kind of see how things are moving. And right now I want to make sure that these two circles move symmetrically along a center line here. So I'm going to add another line here and I'm going to click on the center of that circle there. I'm just going to drag and connect it to this bottom line. You can see I get my coincident constraint. I'm going to click on that endpoint and this line. And I'm also going to make this a midpoint. And the reason for that is I'd really like to get it so that again, these

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two circles move symmetrically along that center line. I'm going to also make this a vertical line. And you can see that now we're getting a little bit of more symmetrical movement there. And I'm going to make sure that this is horizontal. I'm going to click the horizontal constraint. Again, like now we're starting to get some more symmetrical movement. And then finally, I'm going to make sure that this is a set distance. I'm just going to set that to 25. And now

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If I move this around, this circle is moving along an arc that's 25 millimeters long. And I now have a pretty clean movement and actually reduce this to be 24. Just like that. That looks pretty good. We're just kind of roughing it in. not going to worry too much about matching up with the drawing, but this gives us a good idea of what's happening. Now that I have the basic motion for these two clamp halves represented in this sketch.

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I'm going to hide the sketch we're working on, and I'm going to create a new sketch on this surface. I'm going to start working out what the overall clamp shape is. And I'm just going to assume that the profile for both of these clamps is roughly symmetrical. There's some differences between the two halves, and we'll get to that in a little bit. So if I click on this line here, I can start to create this overall shape.

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do some more drawing like this. And then the last thing I'm to do here is add a little arc between these two. Perfect. Now that we have the sketch laid out, I'm going to focus on making sure that the relationships between all the lines stays consistent. And one of the things I'm going to do to help me out with that is adding an extra line here. And we're going to add a vertical constraint. This will make more sense in a second. Once we create all of the relationships,

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But I'm going to just make sure that we're keying to this line right here. I'm to make this parallel. I'm also going to make these two perpendicular.

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like that. I'm to make this set of lines here perpendicular.

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And I'm going to make this line here perpendicular, just like that. You can see that this sketch is now snapping better into the world space. I'm going add a couple of dimensions here. So we're going to make this 13. And as we fully constrain certain elements, those parts are going to turn green. Let's set this to 8.

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going to set an angle here, 140.

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goal here is to try to get all of the line segments to be constrained in length and angle without locking it to the world space.

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And here I'm just going around again, adding dimensions wherever I can, trying to get those sketch entities to turn green.

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going to be 16.5. I'll make it 17.

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Make this 32.

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going to make this tangent just like that. And I can click and drag certain parts of the sketch and see what's moving around. So I can see that this needs a dimension. We'll turn this to 18.5.

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Turn this to 30.

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Make this a 10 millimeter radius.

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14.5.

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So now this entire sketch is green, which means that it's locked in place. And what I'd like to be able to do now is make sure that when I unlock this sketch, I will rotate around this center pivot point. So everything's keyed to this vertical line here. I'm just going to delete that line. Everything turns blue. And now I can rotate this sketch. And you can see that we're getting some constraints here that are not behaving the way we'd like to.

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And the reason is that this is actually a coincident constraint with the very top of the circle. And what I'd like to do is delete that and have it be able to rotate around like this. And I'm going to make sure that this is a tangent here, tangent like that. This is, there's also the same problem down here on this, on this bottom point. So I'm going to make sure that this is also tangent like that. And

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We're going to make sure that this is coincident on the circle. So now if I rotate this, this sketch should move correctly by rotating around that central pivot point. At this point, we're ready to connect our sketch here that's defining our clamp jaw back to our original skeleton sketch. So I'm going to turn on our skeleton sketch. I'm going to type

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P for project and I bring back this circle here and I'm going to turn off our skeleton sketch and you can see that we have this purple element here and that is our projected circle that came from our original sketch. So this this circle here is locked in place. We can't move it around, but I'm going to use it to create a new circle and I'm going to turn that into a construction circle and I'm just going to make this tangent to each of the sides of the jaw here.

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It's going to be a tangent here, tangent here. And really, I'm just trying to make sure that mechanically I have the same distance between the face of the jaw here and the face of the jaw here for strength purposes. So you saw that everything turned green. And what that means to us now is that this sketch is fully constrained. So I can't move this around. But if I turn on our sketch two here, when I move our skeleton sketch,

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that jaw now moves. So we have a complete sketch and we can start now making a three-dimensional model. So I'm going to turn off our sketch one and right now I'm going to create our first body. And I'm noticing here that we're also missing our pivot point. So I'm going to turn on our sketch one and I can click on that.

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can click into sketch 2. I can type P again and project our pivot point. And those things are now locked in place. And if I turn off sketch 1, I can now type E for extrude. And I can select these two elements here. And I'm going to make this a 21 millimeter extrusion. I'm going to also make it symmetric so that it's

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coming from both sides. And I actually want to do this half the distance. So divide by two, just like that. And that is the first jaw or this clamp. So if I click done here, I can actually turn on our sketch one and I can keep moving that three-dimensional part now. So that's looking pretty good there.

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The other thing I can do here is I can also create a mirror of this part. So I'm to do Mirror. I'm just going to mirror it off of our center plane here.

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I'm going to click Done. And we have our two bodies now. And again, if I move our sketch one, both of those jaws move in unison. And that's starting to look a lot like our clamp. Now that we've completed both sections of the clamp, we're going to do some more detailing on this central screw. And what we can do is start by creating a new sketch.

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on the vertical plane here. And we're going to take advantage of this horizontal axis that we created as part of our skeleton sketch.

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And I'm going to dimension this circle. I'm going to say that's 6 millimeters. And I'm also going to extrude this out.

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just like I did before. And there's a few options that I'm going to choose. I'm going to create a new body. And I can go into the history tree and adjust and say that this is going to be symmetric. And I'm just going to round this up to be 35. And that looks pretty good right there. And that's done there. I'm going to take this end cap here. And instead of creating a bunch of different

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extrusions, I'm actually going to create a new sketch altogether.

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put it on the front surface, and I'm going to project this edge here back down to that sketch, and I'm going to use that to create a handle that we can revolve.

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This is on the midpoint, and I'm going to make this vertical.

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like that. I'm going to make these two parallel. Same with this parallel.

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And you can see that I'm wiggling the sketch around to kind of see where things are not connected.

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I'm going to make this parallel here.

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And I'm going to give it some dimensions. So we're going to make this eight, make this dimension here six, and we'll make this dimension here two, four. Perfect. That's looking good there. I can exit out of that. And now we can do a revolve. Click the axis, click check.

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And this revolution here is creating a separate body. So I want to union that together. Click Union. Click Done.

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you'll see that everything moves together.

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So lastly, if I go back into our sketch 4.

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I can create a hole for this other barrel, and I'm just going to put it right on this sketch here.

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I'm going to say that that's seven millimeters, just like that. We're going to temporarily hide this body. And I'm just going to select this area here. I'm going to extrude this out. I'm going to bring that body back. And from that extrusion there, create through all.

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I can do symmetric and it's a subtraction. So now we have a hole and now we can work on creating this little handle that fits through that hole. I think the simplest way to accomplish this is by creating a new sketch and we're going to do it on this vertical plane again. And I'm just going to draw a series of lines here and we're just going to make

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a quarter of this bar because we're going to revolve it and then mirror it. So I have a little bit of a wonky shape here. I'm going to make those parallel. I'm going to make these perpendicular. Same with this perpendicular. And again, this is just like a bunch of relationships. They're going to help us keep everything nice and aligned. Perpendicular.

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I can even make this vertical. And there we go. So this shape is now pretty well defined. I'm just going to give it a few dimensions. We're going to give that three millimeters. We're going to say that this is two millimeters.

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And we're going to say that this is 31 millimeters, just like that. So now this shape is pretty well defined, like I mentioned before. Give it one more dimension here. We're going to give this nine. And now if I move this sketch around, it's pretty consistent. From there, we can exit out of that sketch, click that area.

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We're going to do a revolve, click the axis. There we go. Now we have our nice cylindrical shape. And it doesn't really matter where this is because we're going to use an align tool in order to get that to fit together.

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I can now double click on the body and I'm just going to make a mirror along that face there. I have both sides of that now and I can do a union. Now that the union is complete, I can click once on that surface. I get my align tool. That align tool now allows me to take that surface and align it to any other surface so I can select faces and edges and do things to get those shapes to align.

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So I'm going to select this inner surface here and it automatically centers and aligns those two cylinders collinearly. I can click done. And there we go. So now if I look again at our driving sketch, I can move that sketch around and everything moves together. It's looking really good right there. Perfect. The other thing I can do here is since these parts are being driven,

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can rotate these off axis, for example, and it still works. So if I click on this driven sketch here, I can still move these around. There we go. Everything still works great. I'm going to just undo to get this back to its original location. The last features I'm going to create are these pivot points. So I can just hide everything that I don't need for this, including all the bodies.

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And I'm going to bring back my jaw sketch here. And I'm just going to also hide this body. I can extrude this shape out like that. And I'd like for this to be a symmetric object. And I'd also like for this to be a total of 21.

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And I'm to do the same thing with this pivot point up here.

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I'm going to extrude that.

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I'm going to make it symmetric, and I'm going to make it 21 millimeters, just like that.

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The other thing I need to do is create a hole for the screw that runs across. So I am going to bring back our Sketch 3.

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And I'm also going to extrude this through like that. So we get our hole and that's looking pretty good right there. So at this point, I have all of our pins. I can bring back our bodies and I need to make another pin that's on this side. So what I can do here is I can copy this shape and I'm going to keep it linked. I'm going to move it over.

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And I'm just going to do another align. So I'm click align and align that shape to there. Perfect. So let's bring back our various bodies here.

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I'm going to also bring back our driving sketch and we can double check and make sure that everything's working as we expect. All the pins are staying in their correct location and moving around as we would expect. After a quick undo, you can see that everything maintains its location and is well aligned. And really the rest of the work here is just some cleanup. So it's really creating chamfers and fillets.

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It's creating offsets so that parts don't bind. And we can take advantage of the insert breakpoint feature here to be able to go back into the history and adjust the parts as we see fit. And really all of those changes are going to continue to carry forward and they're going to continue to be driven by that original skeleton sketch. But otherwise this tutorial is complete. We've been able to demonstrate that by creating a skeleton sketch.

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We can drive a bunch of geometry and from there develop a model that allows us to preview a mechanism within Shapr3D. Thanks for watching. See you next time.