Join Leon van den Heever for an in-depth discussion in this video Sides, part of Modeling a Cabinet with SOLIDWORKS.
- Next we're going to create the sides for our cabinet. So let's head on over to SOLIDWORKS. All right, let's go into edit mode for the bottom component and just note quickly we've got some fixing up to do. We've got the overlap on that bottom base section so I'm just going to show all the planes and let's just make a few adjustments to fix that.
So selecting the base width, let's activate the dimension. It's currently 42, we'll change it to 34 millimeters and we will have to rebuild this so that the changes can take effect. So a quick control Q and if we now look at this right corner, that is looking much better. All right, I'm going to also just change the profile a little bit. It's a little bit extreme. So let's take the 20 mil down to 10 mil on that arc and that looks much better like that.
So a quick isometric view and back into the skeleton component. Edit that component. And let's take the following planes and hide them. All right, I think we'll need the bottom plane still. So make sure that that is visible and then from the plane in the graphics view, use our control method and we will establish the sides or the height for the sides.
All right and then from that plane drag another one downward and that will be our top thickness. And then down the bottom you'll notice this on the profile that we've cut, we are going to need another plane coming inwards. So I'm going to take this left-hand plane that we've got visible. Drag this in slightly and we will deal with the positioning exactly in a minute but from it, let's create another plane and this will be our side thickness.
So let's look at this from a top view and determine the sizing that we need for the inner plane of the sides. So I'm just going to use the instant 3D and we'll just drag that until we find more or less where we think it will be suitable to our design. So I'm going to go with six millimeters over here, so I double click on that to edit. Change that to six and then the distance then for the thickness we can make this 20 millimeters.
All right, that's looking good. So the height then let's activate our dimension. Change this to 740 millimeters and then for our top thickness we are going to make this 30 millimeters. Excellent. All right, taking the base front plane, let's drag in then the front of the sides and this dimension we can set in at 50 millimeters.
And let's start renaming this. So the very top plane that we created, this will be our top plane. The one that we derived from it, let's make this the top thickness. All right, then for the side plane that we had for where we had the profile.
Let's call this base edge width. And make sure that you did get the right plane for that. And then the next plane, this will be our side thickness. And then lastly this plane is going to be our side front.
All right, this should be all that is needed for us to get our sides in place. So I'm going to exit and rebuild. Or let's hide the base front and base width planes just so that they are not laddering our space. Head on over let's insert a new component, so new path selected. Let's name this sides.
And select the front plane and then obviously exit our sketch. Go to the edge width, right click on that plane. Let's start a new sketch. Grabbing my corner rectangle, sketch out our rectangle and taking the top edge to the thickness plane. Let's make them co-linear. The left edges, make them co-linear and then the back edge to the back plane, sorry, make that co-linear.
And then we'll put this bottom line onto the top plane. All right, and we fully defined. That's good, let's head on over to features. Let's do an extrude. We will go up to surface. The surface will be our thickness, our side thickness plane. Right click to complete the command and starting a new sketch then on this inside face. We're going to need a little cutout here for our back cover for later, so just a simple rectangle.
Let's define the width of this to five millimeters and then we will constrain the bottom edge to the bottom edge of the extrusion that we've just created. All right and we fully defined. So features, simply extrude a cut for this one and we're going to go in here for a depth of five millimeters as well. Okay to complete the command and that should be fine for now.
So let's go over to features and simply we will mirror this side to the other side. Now make sure that we are mirroring the bodies. So the plane that we will mirror back is the right plane of the active component and then go to mirrors, select if from the graphics view. We can see the result on the right. Obviously these cannot be merged. I'll turn that off from the properties and go ahead and say okay to that.
All right, that is mirrored across just fine. Notice that we have two bodies. That is exactly what we will want especially for when we get to the detailing of our designs but with that let's exit the edit component mode. Let's do a quick rebuild again, so control Q for that. And I'm going to go ahead and save this. So save all, you probably have turned off the flag for that but with that, that's our sides done and I will see you in the next session.
- Setting up the model and adding components
- Creating the main structure of the cabinet
- Modeling the door
- Building the drawer
- Testing the model