Test you SOLIDWORKS knowledge. This sample exam question asks you to build a swept surface or fill surface in SOLIDWORKS.
- [Instructor] In question number one of the sample exam, we're asked to open this part right here and to create a surface over here on the left-hand side of the part. Let's jump over to the question and take a look. First thing we want to do is create a swept surface or a surface fill on that edge. So, we add the option of either one of those. And we know that we need to make it the first thing here is surface should be flush with the X, Z plane or the top plane. So, that means it's going to be along that bottom surface. Should start with a profile that is angled three degrees from the vertical.
So, we have to make sure we're incorporating that. And then, it looks like we have to create a sketch along the footprint of the part so we can use that as our bottom profile, which is found in this Sketch 123. After creating the part, we need to then measure the surface area. If I scroll up here, we can see that this is the surface we're going to be creating. You can see it's a vertical line right over here. And, we've got about three degrees from the top surface down that we need to create that surface with. They're not telling us if it has to be a spline or regular line or what, but I'm going to go ahead and try to use a spline.
So, let's jump back over to the part. So, the first thing I know is that I need a plane right about at the end of this point here. So, right here I have a right plane. If I hold down control, I can drag that out a little bit, and I can choose that point right over here and snap to there to create that point. Okay. And once I have that, I know that's going to kind of be the end of my spline, then come down here to the top plane and let's go ahead and create a spline. But instead of a regular spline, I'm going to go ahead and use the style spline.
I'm going to snap right down here at the end and then I'm just going to drop a couple points out here to create that spline. At the very end, I'm just going to just kind of put a little ways away from the end. Now I know that this point or the end of this spline right here, needs to basically be coincident with that plane. So, I'm just going to bring that over and create a coincident relationship. Now, if I look at the top I can then kind of bring that in. Just looking just about over to where that line might be. Now, I can drag this control polygon around a little bit to create this shape and have this spline kind of follow this surface as best as I can.
So, I can kind of move it in a little bit. And, you might have to play with this a little bit to get it to do what you're looking for, right? So, I can just kind of start moving things around until I'm getting the shape that I'm looking for, at least something fairly close to what this bottom surface is. Obviously, there's a little bit of user error involved in this because we're just trying to copy an imported sketch, and it's never going to be exactly perfect. So, then again, just do the best you can. I can see here this is looking pretty good. Still sticking out just a little bit over there, so let's go ahead and drag that back.
And right there it looks pretty good to me. So, we've got a pretty good style spline set up, and let's go ahead and exit out of the sketch. So, now we have a lower line, we have the upper profile, and now all we have to do is connect the dots. So, let's go ahead over here and start a sketch on plane number one. I'm going to spin it around so I'm looking at the other side. And, I'm going to go ahead and use the center line command. So, I'm going to start with the center line going perfectly vertical. I'm going to make one more over here, and I'm going to set the angle at three degrees.
So, there's three degrees. And then, I'm going to start a regular spline right at this point here, and I'm going to snap that right down there to my new line, which happens to be right there. Hit escape and get out of that. And then, make sure that we say that this line right here and that spline are tangent to each other. That way it's coming out at that three degrees and then connecting down to that lower sketch. If you have a hard time seeing that lower sketch, you can also just get rid of the sketch itself so you can see it connecting the dots between the two.
Alright. Exit out of that sketch. Now, you can see we have one enclosed boundary. I'm going to go ahead and hide this plane, make it a little easier to see what's going on. And now, we have two different options. One is we can sweep this profile, or two we can patch it. So, let's go over here and click on surfaces and let's go ahead and do a fill surface. My patch boundary here is going to be this upper surface here, this lower surface there, and this one right over here. And, you can see just by easily choosing those three lines, we automatically get what we're looking for.
Click on okay and there should be the answer. Let's go ahead and measure that. Alright, my measurement here is 2220.26. Let's jump back over to the sample exam. Let's spin down here to the bottom of the exam and see what the answer is. So, it's 2220.93, seven millimeters, so we're not exactly what they have, but we are within the seven. Because there is some variability based upon how we create that lower spline, there will be a little bit of variation, but we are within the values so we are all set.
Let's jump back over to SOLIDWORKS and also jump out of the measure command, and let's go ahead and just create that one more time. So, because we already have that surface fill, I'm going to go ahead and just hide it for right now. And then, I'm going to go ahead and show the two sketches that we created. And, I'm going to go ahead and create it as a sweep as well. So, here's our surfaces command, swept surface. The profile, or the sketch profile, I want to use this one here. The path is this upper profile here and my guide curve can be this lower profile there.
So, that's one other way to create that shape. Click okay. And, go ahead and measure this one. And you can see, this one actually is a little bit bigger. It's 2229.65. So, there's a couple things of variability in this the way you're going to create it. So, I think probably the first option, the surface fill, would be a better bet, but a couple different ways you can create a shape similar to that, couple different options and they both work pretty good. I think the first, the surface fill, might be a better choice in this situation.
- Exam-taking techniques
- Surfacing tools
- Creating splines and 3D curves
- Building a boundary surface
- Extending and untrimming surfaces
- Knitting surfaces together
- Creating surface fillets
- Using the Thicken tool