From the course: SOLIDWORKS 2017 Essential Training

Working with planes - SOLIDWORKS Tutorial

From the course: SOLIDWORKS 2017 Essential Training

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Working with planes

- When we first open new part inside of SOLIDWORKS we have the three fundamental planes, the front plane, the top plane, and the right plane, and generally we're going to use one of those to get started building our model. What happens if you want to create a hole, maybe to have some funny angle through a part or what if you want to create a feature that's not on one of those planes or we don't have a face to start on? That's when we need to start creating our own planes. Now there's a bunch of different ways to do this. I'm going to go through all of them. First things, go over to "Features" and come up here to "Reference geometry." Click on the drop-down and click on "Plane." Now the most basic type of plane is just going to be an offset plane, so I'm going to choose one of my existing planes, so maybe the top plane, or the front plane and then just type in an offset value. It's going to take the plane I started from and I'm just going to type in how far I want to offset that plane to create a brand new one. I also have the option to flip it to the other side or create multiple planes at the same time, which might be very helpful if you're going to be creating a lofted feature or some other complex geometry. I'm going to go ahead and take that all the way back down to just one additional plane, and then click on "OK." I also have the option to choose two different faces so under "Reference geometry" go to "plane." I'm going to choose maybe this face here, and then maybe this face over here and it's going to put a plane directly between the two faces that I chose. Two references, we're leaving the third one out because we just don't need it. Click "OK" and there it is. Now, as you choose entities, faces and planes go infinitely in all directions, so it's easy to use one of those as a reference. A line has two end points so I actually need a secondary reference to use a line. If I'm choosing only points, I need to choose three points. So click on "Reference geometry." Click on "plane" and I'll give you an example. So if I choose just a face itself, it allows me to just give a value and click on "OK." I only need one other reference. If I, instead, choose just a line itself, it's going to need not only a line but it also needs a secondary reference to determine where this plane is going to be in space. So if I click on a line and maybe a face, you'll say, "Okay, I want to have a perpendicular line "or a parallel plane or maybe set up some type "of an angle around that line." You can see I can rotate that plane around that line just by holding down the angle or typing in the value. If, instead of either one of those, if I turn both of those off, if I only choose maybe a point, or a point down here at the bottom, I need to actually choose three of those. So I choose a point here, I choose a point there. That's basically the same as a line, and then maybe a third point, and now it has the ability to put a plane there between those three points. So if using a point, you need to use three of them. If you're using a line and a point, you only need just the one line and a point or if you're using a face or a plane you only need to select that. If you also have to rotate around something that's not there, you might need to go ahead and create a sketch, so I'm going to go ahead and accept that one and then create one more plane. This time, I'm going to choose this sketch that I drew here and if you need to adjust the sketch, you can. I'm going to rotate around this line here and then define how much of an angle I want to rotate based upon this other sketch here. You can see here, I accidentally added too many so I'm going to get rid of this one here. I'm going to get rid of this plane right here. I'm going to choose this plane instead and then define the angle that I want to rotate around there. So instead of 90 degrees, I'm going to change this one so it rotates all the way around to the other side. Which will allow me to create a hole at an angle through this part. So you can see as I go all the way around here, plane gets in position and you can see then looking through this plane here, I'll be able to cut a hole at that angle through this part. Click on "OK." There's my reference. I can then choose any one of these planes, start a sketch, start a hole or any other sketch geometry, and then I'm going to create that right on my part, do a feature extruded cut, and I'm going to be cutting from that plane into my part and I can click on "through all" and it's going to cut right through my part at that angle. That's a great way to create some more complex geometry. If you get too many planes in your design and you want to hide them, you can always go up here to "View" and instead of displaying the planes, you can just turn them off. Same thing with sketch. "View, show/hide," and we're going to hide sketches. Sketch planes, I can go "view, show/hide "sketches." I also have these options right under here under my View palette. There it is, that's creating reference geometry and creating reference planes and multiple different ways for doing so.

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