Sketch constraints and splines

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In this exercise, I'm going to show you how we can create all the sketches so we can 3D model those models you see. In this demonstration, I will show you how we can draw lines, arcs and splines, and then work with dimensions and constraints to stabilize the sketches. Ultimately, this will also take a look at what a fully constrained sketches

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like in green on the left side, and a fully unconstrained sketch in blue on the right side. And what this means when working inside a parametric modeling environment.

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Let's start with a new and empty file. I will go into front view, move the screen down a little bit. And to create our sketch, I will go to the toolbar, select Sketch. The line command is selected and I will start drawing my first line from the origin to the left side, along the X axis to the length of 30 millimeter. And I will snap to the grid as an easy helper. Click left mouse button and then

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right click to stop. I will zoom out a little bit, move the screen down, and then continue drawing my next line from the origin or the endpoint here. I click and then draw a line straight up. This line should be 200 millimeters. On the keyboard, I can simply type in 200, press Enter. It's a very long line. I zoom out a little bit more. And you see by writing down 200,

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and pressing Enter, I already gave a length dimension to this line and this can only rotate now. I would like this line to be vertically oriented and I can snap directly to the Z axis. And when I click, I am creating a Coincidence constraint of the sketch endpoint to that Z axis. So left mouse button click, we will zoom in so we can see 10 millimeters.

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left mouse button click, we will go down 30 millimeters click, and then we will stop, right click and exit the active drawing. At the bottom, we will just draw another line straight up to around 140 millimeters click and right click and one time right click, and then select, drop the line tool. We've now

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Command active, I can now select specific elements. Let's take a look at what we have. This line is 200 millimeters long. I will go to the Constraint Settings display and turn on, Always Show Dimensions and Always Show Constraints. So you can see now this line is 200 millimeters long. It has a thick green end point.

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and also a green endpoint at the top. This means that this line has a length, so it can't change it. And also it can't rotate because the endpoints are solid green. You see the other three lines are blue. And then also here, this line is green. So let's pay attention to what happens when we start clicking on those elements.

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And you see, we can change the length and we can change also the rotation of the line. This line is green and has one green endpoint. The other one is blue. So that means I cannot rotate it, but I can change the length. There's this constraint. I select it and then delete it, you see now this is blue. Now can also rotate it.

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To make the sketch more stable and not deform unexpectedly and also give dimensions, we can then use constraints. So this line should be horizontal. I give this a horizontal constraint. This line should be vertical constraint. I can also select both of these lines and hit horizontal vertical. This worked out.

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Then let's add dimensions. I click on the line. This then gives me the dimension. I can write in the value. And you see now all these lines pretty much are green. This is a nearly fully defined sketch. Only here, this point is blue, which means I can still move this. This does not have a length dimension. Let's draw in an arc.

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to there, we can rotate this arc a little bit. It's okay practice to roughly draw this in, right click, drop the Arc tool, because now we can think about how do we want this arc to be in relationship to the rest of the geometry. This arc should flow nicely into this line. So I selected both, and then we add a Tangent constraint.

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this arc to here, I would like to be 90 degrees.

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And now you see we have a really nice, perfect quarter arc. And everything, as you can see, is nice and green. We then go ahead and change some of these values. You see everything moves in a very predictive way. This is what happens when you have a fully constrained sketch. If elements would be blue, they might change unpredictably.

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We can try this out as an exercise. We can also remove constraints. I click on this lock icon. This is gone. I select the Tangent constraint and delete this. I select this and do that. And if we change this to 160, you see what happens. The rest stays and doesn't really follow with it.

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One more time, we will set this to be a horizontal. This should be Tangent, or I can also constrain this to 180 degrees. I would like this to be more a curve like this. So I will give this a 55 degree radius for the arc.

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Let's select everything, but double click, then we go to the Move and Rotate command, turn on the copy function, and we move this over along the grid somewhere else. Turn off the copy, and then I zoom a little bit more in to cleanly snap to the axis.

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Because I made a copy and I moved this to the side, you see this snap now to the X axis, but everything here can move. This point I will lock.

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this line is blue because it does not have a horizontal or vertical constraint. And there we have everything constrained again. Let's delete this arc. Then we move this down a little bit to 100. And we're going to draw in now a spline. With the spline,

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particularly the control version, I start drawing from one end, click. Here comes now the tangent point, click. I can click somewhere else. That is the second tangent point to this line and then click. This is the end point, right click and right click, Drops Line tool. In a similar way, how we created a Tangent constraint to

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make this spline flow softly into the line. We will make this spline flow softly into those lines, two times for each end. But this is still blue. Well, because these points can move around and these points, I can dimension the distance vertically. It's very easy. 30 and here also 30.

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and then you will see everything is perfectly constrained. I cannot add another dimension here in between because everything is already solved. When I lower this to 80 millimeters, you will see the distance between these points is changing.

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Beautiful. Very good.

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What we can do now is we can go to Exit Sketching. You see these dimensions, we will keep them on for the moment. I click into the sketch profile, shift click the axis and call the Revolve command. I will do the same on the right side, Revolve. And there you see now we have these two bodies.

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because everything is dimensioned and we see the dimensions outside the design. And again, because this is on each case, a fully defined sketch, we can adjust everything while being outside the sketch environment. If you do not want to see in the modeling environment, also the sketches, we can then go back into the sketch environment, go to constraints and simply...

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turn this off. Then we will not see those when nothing is selected. And also we will not see them outside the sketch environment where we model, but we can also not edit them in this environment.

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You see that I created two very basic representations of these bottles. They have nothing in terms of fine details or internal volumes. This is a very common approach that you block out the basic sketch and then later you start adding more details to it. So I will go into the sketch environment and each corner, I would like to have

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an arc position so I can fill it each corner. I do this here and I do this there. Then right click and drop the arc. will Tangent them so they really nicely flow into these lines. And I hope at this point you start getting an idea of what these constraints do. They're kind of like geometrical restrictions.

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Both arcs, I would like to be always the same. So there is an equal constraint. If one arc is being adjusted, you see the other one will follow it perfectly. We do not have any information about the bottle and the cap. We can continue drawing very basic elements in here.

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These lines will be horizontal and vertical. This will be horizontal and vertical. I will dimension this to 20 with a distance of 2 millimeters. And then I will do exactly the same on the right side. You notice I drew them a little bit different. was a mistake.

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This should have been horizontal and vertical because now lines which are the same, again, I will set to be equal and you see that also now created a fully constraint in this other bottle. Because when the cap and the neck is the same, I only have to create a sketch for that one time with dimensions. So this way, when I change...

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this dimension, you will see on the other side, this updates automatically with it.

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When I go into Exit Sketch and call the history line, you see everything is exactly the same. And that is because we did not really update these comments.

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I open the Revolution tab, then I click on Edit and Delete Face, and only select these two inner profiles. So I'm replacing the commands. I can do the same also here.

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When I click on this, you see then everything is gone. That is a different way. And now to create the caps, there we simply select the sketch profile, the axis called the Revolve command. And there we are. You see also how I structure everything very cleanly. The caps I will hide for the moment in the items list. Then I select both caps

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and call the Shell command. To make something nice and easy to see, I will use two millimeters for the thickness. You see now one command applied to two faces of two different bodies. Again, another nice example of how to work effectively and fast. Work smart, not hard. This is the beauty of history-based parametric modeling. When inside a sketch, you work with fully constrained sketches,

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but also in the object environment when you work with modeling features and you chain them together. We can take a look at the section view and there we see how beautifully everything was executed.