Parametric robotic arm using driving sketches

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Hi everyone, welcome to this Shapr3D tutorial. This time we talk about driving sketches. So driving sketches are sketches that we are using in order to inform other sketches or parts of the model. So in this case, we are going to use driving sketches on this robotic arm in order to inform the position, angles, and rotation

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of parts of the arm. Traditionally, you would use separate items of each part of the robotic arm and put them together in an assembly where you are then able to rotate and move around parts of the assembly. But we are using the advantage of driving sketches in order to have the same flexibility and same advantages as in an assembly, just in one easy file. So let me demonstrate what we can do.

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just go in this underlaying sketch, pick this point here at the end and then move this point around and you will see that the robotic arm moves accordingly. So what I'm using here is called an inverted kinematic. So basically a traditional setup of an arm with two linkages. Also, we can exit the sketch and we have another driving sketch here in the bottom with which we can rotate the whole arm.

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So now that we see how advantageous it is to use driving sketches, let's jump in and see how we can do it. So here I am in a new project. Let us name this project accordingly. And first off, let's set up the sketches properly. So in order to provide the rotation along the C axis, we first need to add a sketch.

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from the top view. Let's just add a line in a random position and give it a set length.

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I'm using millimeters as a unit for my model. Be sure that the starting point of our line is green and it's in the center point of our coordinate system. Now, when we click the second endpoint of our line, we can basically rotate the line around the center point. That's exactly what we want. And for good measure, also we can change the line to be a construction line. Now let's exit the sketch.

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And let's add our first construction plane. So go to the plus icon, set the construction plane to be along edge at an angle. So for the first part, let's select our newly created line, then click next. And we need to select a face or a plane in order to set the angle. So let's select the bottom XY plane, click next. And now we can

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select the angle in which we want our new plane to be. You will see it's not snapping in increments. We can change that by going onto the right upper hand side and click snap to grid. So hit done and this is our first construction plane. Now we can select it and we are going to create another sketch on this plane. So now let's create our driving sketch.

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This is going to be our linkage system. So I'll go to line and draw from the zero point upwards in the C axis. We can select our height and then we need two additional lines going to one side and then to the other. And we can select or choose our length.

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And we need one additional line going down from the endpoint.

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Now let's select all of our lines and make them construction lines. We can already see the only fully constrained line is going to be our vertical line going from the center point and the other lines only are constrained by their length. What that means is if I now select the last point in this linkage system, I can move this around and you will see

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that the rest of the linkages are following accordingly. Since the links are constrained, it can only change the angles between them. This we take to our advantage. So we're done with this sketch. We can now exit this one and we can test if our rotation system works. So let us select the endpoint of our first sketch and rotate this. And you will see that our linkage system rotates accordingly as well.

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All for the last part of our setup, we need to add additional planes along the linkages. So the same idea that we had in the beginning with our first plane, we are now adding additional planes along the linkage system. So click on add construction plane and the type should also be along edge at angle. So the first one will be our first horizontal line. Click next.

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The reference plane will be our rotated plane. Click next and then we'll just make it 90 degrees. Hit done and we repeat this for the last three parts of the linkage.

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So now that we created all these planes, we can tidy up a bit by going into the history and selecting the planes that we just made, going into the details and changing the size of each of them to be a little smaller. So now that it's a bit tidier, we can recheck if all our linkages work and the planes are following our driving sketch. Perfect. Now we are

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ready to create our first part of the arm. To do that, let's jump into this plane. And I like to just go out of the planar view in order to show you exactly what we are doing. The first thing we need to do is projecting our driving sketch onto this plane. So let's go to more project and select our first linkage line. Click done. Now we need a few lines. So one

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going perpendicular to our sketch line, one going down perpendicular to this one, and then one going back to the endpoint of our first line. Next, we want to round those edges. So I'll go and select the arc tool and create an arc between those two lines. Going to select the arc and this line, make them tangent, and then the same on the other side

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and we'll create another arc on the lower part. Also make them tangent on both ends. Now we can trim away these edges and create some dimensions. So I'll select the outer edge and the sketch line and make them be 60 millimeters apart. Next let's select the arc and make this 40 millimeters.

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Now we want to have both of these arcs be the same length and radius. So let's select both of them and just constrain them equal. Another thing we can do, since we are going to use this dimension a few times, let's go into this radius dimension and select this icon here. This will create a new variable, which we can then reference in other sketches. So.

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Let's select OK. And in the history, we can now see our variable called length 1, which is 40 millimeters. We can rename that to be radius 1. We can also do this with our offset of 60 millimeters. So select this icon and create a new variable. And then again, we can rename this to be distance 1. OK, we can now...

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Jump out of the sketch and we're going to create another sketch in order to create our first part. We'll select our rotated plane, create a sketch and we're going to create a sketch here at the end point of our arm sketch. So I'll select the circle and we'll just need a circle of 50 mil and make sure that the circle is green and constraint fully.

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Exit the sketch. Now we can select the area, go to more and sweep along our just created sketch. So now we have our first part of the arm. We can already check if it's doing what we want it to do. And that looks good. So now it's going to be a repetition of what we just did just on the other side on our second linkage. So select the plane, go to sketch.

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Now we want to reference this line. So go to More, Project, and project this line. And now we can use it to make our sketch perpendicular to this one. So I'll go to Line.

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and create our sketch. And if these references are not popping up automatically, go here to the constraint settings and then make sure that auto constraining is on. Sometimes you want it to be on just to make your drawings or your sketches quicker. And same thing, we want to create an arc between those two lines and select those, make them tangent.

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And the same thing on the other side.

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going to trim away these corners and now we need to set our dimensions and here we can take advantage of our variables. So we have distance one, which is 60 millimeters and we have our radius, radius one of 40 millimeters. Of course we can now either make both of them equal or again, go in and make this one.

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be the radius reference as well. So now that we have a fully constrained green sketch, we can exit, select the end surface of our first arm linkage and go to more, sweep and sweep along this sketch. OK, perfect. Again, we can recheck if everything works by going into our driving sketch and moving the end point around. So now let's finish up this model.

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with adding a few additional parts. So right now it doesn't have a beginning and an end. So let's change this. We'll go into our last part of the system of the linkage system into the plane and then hit sketch. And then we are going to do the same thing as we did before going to more project and use our driving sketch as a reference hit done. And now again, I'm going to use a line going

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parallel, excuse me, going perpendicular from that sketch and then creating a rectangle. Now we'll round the corners again with some arcs, making them tangent on both sides.

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as well as trimming those corners and making sure that the distances are correct. And again, we can use our reference distance of 60 millimeters and the same thing for the radius. Going to use the radius reference. Now I'm going to make those equal and we have a fully constrained sketch. So let's exit and again, use the end surface of the arm in order to go to sweep.

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and sweep along these edges. I'm going to stop after this curve here because we are going to add a grapple arm. So hit done. So let's click this end surface and then create a new sketch here. You will see that it turns around because it follows all these turns and angles that we did during the creation of the arm. So what we can do is again,

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use our project and use the vertical line of the first driving sketch in order to inform the vertical lines. So now that we have that, we can also project the edge of the surface. And now let's add some additional lines. I'm going to use the center point of the circle. I'm going to go perpendicular and then I'm going to end at

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the circle sketch and make this tangent as well. Now we can select the height or length of the grapple and also we can select the thickness in the end of the arm. So that's it for the grapple part and we are going now to select those and extrude them outwards. I'm going to use 40 millimeters because this is going to give me the same distance between

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the center planes. Also make sure that we are creating a new body and we're not using union in order to connect those two. So this is our new part. The last thing for the Scruple part is we're going to again go into this newly created surface, create a sketch. Now we want to reference this edge. So go to project, select the edge, create a new circle, make it a bit bigger.

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from the center point of this edge. In order to have an offset dimension between those two circles, we can create two lines going away tangent to those respective circles. So select both of them and make them tangent. Then we'll also make them a construction line and parallel to each other. What that gives us are two reference lines so that we can now set a distance

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for this circle. So let's go with one millimeter distance, exit the sketch, and we're now going to select this area and pushing inwards for the 20 millimeters that will give us the middle point of our part. So now to make it a bit nicer, we're going to give that a few rounded edges here and also on the bottom here.

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And since this is only the first element or first part of our grapple, we of course need to mirror it. So we're not going to mirror, but we're going to use rotate around axis. So let us double click in order to select the body. Next, we're going to select this reference edge. And then also we need to highlight copy and then we can