Action camera mount

What you'll learn

Join Andrew Camardella, an industrial designer and adjunct faculty at DePaul University, as he explores advanced 3D sketching and modeling techniques to create a fully adjustable action camera mount. Follow along to get familiar with the following Shapr3D concepts:

  • Setting up sketches: Learn how to create editable sketches with center point rectangles and dimensional constraints to refine your model.
  • Using constraints: Discover how to apply vertical constraints, angles, and offset edges to maintain symmetry and ease future adjustments.
  • Extruding and mirroring: Understand the process of creating solid extrudes and using the Mirror tool to duplicate components efficiently.
  • Project tool: Utilize the newly added projection parameter in sketch history steps to modify projection components more seamlessly into your sketches.
  • Boolean operations: Combine multiple bodies into a single solid body using the Union and Subtract tools.
  • Creating variations: Use linked and unlinked copies to create and modify variations of your design and learn how to adjust parts of your project in History for quick prototyping.



Welcome to a Shapr3D tutorial. My name is Andrew Camardella. I'm an industrial design consultant and adjunct faculty at DePaul University. In this video, we're going to take a look at setting up sketches to create an ideal 3D model that allows us to adjust geometry as we improve our model. We're also going to take a look at a few tools that have been improved or added since Shapr3D's latest update. To cover the main topics in this video, we're going to be 3D modeling an action camera mount.


Let's get started. We're going to start up a new file here. So we're going to need to start making our first few sketches to help define the overall part. We're going to focus a lot on sketches in this tutorial. We're going to try to make something that is editable, and that's going to allow us to alter the design overall as we refine it and as we decide we want to make changes. The first thing I'm going to do here is start by creating a center point rectangle.


of the overall dimensions of our part. So I'm gonna just really quickly just rough out the overall dimensions. And these things are gonna get refined over time. So I don't need to be super specific at this point. We're just setting up an overall sketch here to give us some good bass models that we can start working from. The thing that we're working on is a two-piece camera mount. So there's a bass component and then there's a top component that clips into that.


I'm going to start building the base component first. And we have our overall dimension here. I'm also going to draw in a couple of other things, like our center line. And I'm going to make something that's symmetrical, and that's going to make it a lot easier for us to edit as we move along. That way, we only have to change dimensions in certain places when we're building this model out. So I'm just going to quickly rough in some dimensions here.


This dimension here is nine millimeters. As we move around, I'm adding dimensions. I'm also gonna start adding constraints. Shapr3D does a good job of automatically adding certain constraints in. It makes our lives a little bit easier. I'm gonna add a dimension here. We're gonna call this 4.5.


also going to click in here and this three.


One of the nice things about these new dimensions is that we can actually set which direction they're going in. So I want this to be a vertical dimension here. And that's just going to help keep things organized and in the correct orientation. One of the other things I want to do here is add some dimensional constraints for angles. So I'm going to make this 135.


And you can see with that I'm starting to get a little bit of skew here. So I'm going to just make sure that these dimensions are correctly located. I'm going to say that there's a vertical constraint here on this line.


I'm going to add a new vertical constraint here.


And I'm also going to move this back to our center point.


That right there is going to be 6 millimeters. And that completes that section of it. We're going to use our mirror tool once we create a solid to help us create this component. I'm going to also make another vertical line here, which the thing that we can do is create an offset line. So I'm just going to click in the more. I'm going to create an offset edge. And I'm just going to slide this over and call this 1.5 millimeters.


I want that dimension to stick around, so I'm just going to click and drag this here, hit enter.


So now that dimension sticks. And that gives us our basic layout of our part. So the very next thing I'm going to do here is start creating some solid extrudes. Now that I have these areas, I can click and drag them and move them around. So I want this height here to be a total of 11 millimeters.


And I'm going to just take this part and I'm going to make a duplicate of it by creating a mirror. I'm going to mirror along this face here. I'm going to click Done.


And I'm going to mirror that one more time to mirror it across the other side. I'm going to click on more, click on mirror, and I'm going to select this center plane right here in order to give myself some symmetry there. So now I have these four bodies and they actually are all going to be the same piece. So I'm going to hold off to give, make them a union until I get this bottom sections figured out.


So I'm going to make a bass plate that connects all those pieces together. I'm going to make that 4.7 millimeters.


You can see now that we have five pieces, we're going to end up connecting all of those things together.


The last thing I want to do here is also extrude another component. So I'm going to hide this last body that we made. And I'd like to make a little rib that goes through the middle of this component. I'm just going to lift this up here. I'm going to call that six millimeters total height. So what I've done is measured from the very bottom plane and extruded everything up. And that gives us our total height.


And what I'd like to do is also copy this and mirror this over. So I'm going to use our history tree here to move some things around. So I'm going to move this last extrusion before our mirror. So our mirror now is after the middle extrusion. I'm going to just add another, I'm going to add that extrusion to our target bodies. That way we get a nice symmetry with our components. That way, if we change anything about the sketch originally, everything updates automatically.


I'm going to bring our last extrusion back here, and that gives us our total design. So at this point, I can start bullioning everything together. I'm going to select everything. We have our top panel there that allows us to filter what it is we're selecting. I'm going to just tab over and select bodies. And now I'm going to union all of those pieces together. Now we have one single solid body. The other thing I want to do here is to cut


a little relief here that allows us to slide a clip in along this component. So I'm just going to really quickly create a new sketch on the end of this face.


And this is going to bring up one of the updated features of using the projection tool. I'm going to type P for the projection tool and that is going to allow us to include components into our sketches. And I'm just going to select these tall pieces here. It's going to give us some reference points for some of the geometry after cut.


So I'm going to click Done here. And you'll see that if we go into our sketch here, now we have our plane. We also have projected edges. And if we want to add more projected edges to the sketch, we can go back into Edit. We can include more edges into that.


So I'm going to use those projected edges now to create a subtraction. And I'm just going to...


Get back into our sketch. I'm going to go back to our rectangle. And this time, I'm just going to do a diagonal rectangle. I'm just going to click on this line and come all the way across to this edge here. We're going to add a dimension that goes from this edge here to this edge here. We're going to make that 2.5 millimeters. And with that, what we can do is click these areas here.


and use that as a way of cutting through this part. We're just going to subtract those areas there, and that's looking pretty good. But from here, what we can do is hide this body, and I'm going to start working on the new component that we're going to use to mate these two pieces together. And I know that the overall height of the part right now is 11 millimeters. That's going to work for us right there. I'm going to click OK. And


From here I can bring back the body that we've been working on and we can do a subtraction between this new component that we've made and the solid that we've created before. I'm going to do a subtraction like this and I'm going to make sure that I'm going to keep the bodies that have been removed from their original components. And that way we get a positive and negative piece that fit together. And we're just going to click OK.


Now we have these two pieces and we know that they're going to fit perfectly. So I'm going to hide this piece here because we no longer need it for our purposes. The next feature we're going to create is a slide release spring out of this component here, by removing some material. And the first thing I'm going to do here is start a sketch on the very top surface of this part. And I'm going to remove a long slit.


through the surface. So I'm just going to create that with a couple of lines.


And I'm also going to thin this material here by cutting away a little bit of this material here. And what I'm going to do is I'm going to first project up this surface here. So I'm going to click P and just click that surface. And then I'm going to also create a line here that just cuts away a little bit of this material. Just like that. And the rest is just creating constraints. So.


I'm going to select these two lines here. I'm going to make sure that I have a consistent angle. 45 degrees works. I'm also going to create a dimension here, make this four millimeters. I'm also going to make sure that this is a consistent distance away and I select these two edges here. I'm going to make this three millimeters. And I'm also going to make sure that


these edges are horizontal and perpendicular. I'm going to select horizontal and vertical. And there we go. So now I have some more areas that I can use to extrude away material. And I'm just going to select these two here and just extrude all the way through the object, just like that. So now we have a thin section here that should spring out of the way and allow us to create that slide buckle feature.


Another thing that we need to do is cut away a bit of this surface here so that it slides under the detent in this body. So if I hide this, we want that part to slide underneath of this detented area here. I'm going to bring that body back. And I'm going to cut away this by creating another sketch.


And I'm just going to draw a line vertically right here. I'm going to select this line here. I'm going to actually tilt this edge in a little bit, just so that we have some ability to connect these two pieces together. And this part will kind of ramp off that detent and slide underneath. I'm going to select this area here. And I'm going to just drag this down and make it minus 3 millimeters like that.


should be below this edge over here, which is kind of the maximum height of that detent. And that should work for us just like that.


I'm going to make a little bit of relief here by selecting these edges and putting some fillets on them just so that it slides past that detented area. I'm going to make this a 5mm fillet. I'm going to fillet this edge here. I'm going to make this 7mm.


And I'm going to also fillet this front edge here and make that 3 millimeters. So this is now a nice smooth curved area and that's going to slide underneath of that tooth that we have on the base plate. And we can sort of take a look at that in just a second. I'm going to duplicate this component using a mirror. I'm going to mirror that. Select my mirror surface, click check.


That's done. And then I'm going to double click both of these just to a simple union. So I have a single piece, just like that. And then we're going to check this against our bass plate. So I'm going to come over here and turn on the body that we have. And you can see that everything fits perfectly there. And I'm just going to slide this back so that we can double check a couple of things. But as this


As this circular tooth here engages this base plate tooth, this section will kind of spring out of the way and pass through this base plate. So now we have a finished action camera mount and I'm just going to undo to remove those movements that I just put in by sliding this part around.


And the remaining thing here is really just making variations and cleaning this up. The concept overall is complete. And so the thing that we just need to focus on now is cleaning up certain things like fillets and smoothing out corners that might otherwise be interfering and also giving a little bit of extra room for relief. And so one of the things that we can do is kind of save our progress here by using the new copy tool. So if I select both of these components.


And I'm going to make a copy of them. I'm going to unlink this copy. So at this point, this copy is going to be frozen. It's not going to update anymore if I change any of these dimensions. Likewise, if I was to double click all of these, I was to create another copy. This time, I'm going to leave it linked. What I can do is slide this over. And now I have a copy that's going to update with that original component. So I can start working on variations now and add, for example, different mounts or different types of.


connectors or variations of this original part and when I change this original body everything down the line is going to also update. So as an example I can come here I can create a sketch and I'm just going to create a simple mount for this connector. I'm going to draw a rectangle here. I'm going to make this upper dimension here three millimeters.


to make this 15 millimeters. And that way I have two dimensions there. I'm going to also add an extra line. So I'm going to type L, I'm going to select these two points.


And what I can do here is...


select this line, turn it into a construction line, and also make it vertical. Now I have a centered rectangle and I can use this area here to create part of my mount. So I'm going to select this area here. I'm going to type E for extrude. I'm going to bring this up to 17 millimeters.


just like that. I'm also gonna make sure that this is a new body. And the benefit here is I'm gonna be able to move this part around. I'm gonna create a copy. So I'm gonna move it six millimeters this way. And I'm also gonna create another copy and move it 12 millimeters this way, just like that. So now I have a new mount.


and I can do variations on that as well. But the benefit here is that once these are all connected...


I have a new body that I can move around and union those together.


And I can start making edits to that and building more features. So there's a few benefits to the linked and unlinked bodies. And the unlinked body is going to be over here. It's going to kind of be our history. And it's not going to change. The other thing I can do is I can come in here and I can start to modify this original component. So I'm going to hide this body. And I can select, for example, these surfaces here. And if I wanted to add a little bit of a relief, I can push and pull those surfaces.


to get a little bit of extra space for those components to fit together depending on the manufacturing process. So right now they're just very close together. So you're going to get a lot of binding in those elements. So I can just come here and add a little bit of relief. And I'm just going to give it 0.3 millimeters, just like that. And what I'm left with is a face offset right here. So that didn't update yet. But if I take this face offset and I move it


I made my copy, then everything down the line will update. So you see that I moved the face offset before my movement rotation. And now my update happens in the, in all the downstream models. And that my original unlinked copy still doesn't have any of those features added into it.


Likewise, another thing that we could do is we made these bosses here, and right now they're squared off. If I wanted to round them off, for example, I could also come in here and do something like round these corners over. And I'm just going to give them a fillet. I know that that's 15 millimeters. I could do 7.5 just like that. Again, I have a fillet that's here. If I bring it before my movement rotation, then all of the downstream items are going to update.


And finally, one of the most powerful features is that I can come in here and I can also change the original sketches. So if I change this to 32 millimeters, everything downstream is going to also update. It's a really useful tool to have access to. And you can see that our original model here hasn't updated at all. It's unlinked and we can continue to revise and make edits. And I can continue to make copies of this piece here and add different features as we go along.


At this point, these parts would be ready to make a quick prototype of, and using validation tools like 3D printing, we'd be able to see what changes we need to make in order to improve these parts.


Try it yourself

Action camera mount


About the instructor


Andrew Camardella has a diverse background stemming from his interest and understanding of "how stuff works". He has spent over 5 years working as an Industrial Designer and Digital Fabrication specialist, and he uses his knowledge of the product development process and various digital tools to translate 3D models between the physical and digital world. He uses 3D scanning, 3D modeling, and digital fabrication tools like 3D printers and CNC machines to help clients develop products and create prototypes and visualizations. Andrew currently lives and works in Chicago and does contract design and fabrication for clients ranging from startups and established companies, to artists and independent inventors. His work and experience spans a variety of industries from large scale art, digital imaging, environment design, green design, to consumer and commercial products.

Source: Pluralsight

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