Project #2 is started, based on the settings from Project #1. The profile is created and extruded and then cut is placed.
- [Instructor] Welcome back, this is the first video for project number two. So we're starting with the project one complete file, and we're going to be using this file as our starting point so that we can have all the same settings that we developed for the project one file. So let's go ahead and save this file one last time, just in case you just finished, and it's a good idea to do one final save, and then we'll do a save as. And then we're going to save this in our chapter three folder. And we're going to call this one project number two. And then underscore, 03, and then 01.
Okay. So now that we've saved this, we can go ahead and safely delete the project that we've created from project one, and now we're ready to start with project two. So let me switch over to the PDF version of the file. So let me just explain here the game plan for how we're going to develop this. So this is a little different than project one in that we have three views instead of one view. We also have an isometric view that we'll create at the end. After we've created the three dimensional solid we can set it up so that we can also reference in an isometric view as well.
So we're starting by developing a plan to create this solid, and I think the best method here, rather than start with a slab feature, which would be a rough feature of just a six sided cube type shape, instead what we're going to do is start with the profile of the outside edge of this front view. We're going to omit the rounded corner, so we're not going to fillet and round the corners first, or chamfer. We're going to use the feature modeling tools to do that instead. So this way we keep as many separate features as we can for the project.
So we're just going to start by drawing this profile, then we'll create a cut from the top edge of the part, and then we'll add in our holes, counterbore countersunk holes, through hole, and then finally the chamfer and the fillets and the rounds. Okay. So with that said, let's go ahead and start by drawing out the profile. So I'll go back to my tile view configuration. So we're going to be using the front view for the profile. So I'm going to go ahead and maximize the front view. And then we're not really concerned about where we're starting the project.
We just want to start drawing in the view, and then we'll go ahead and use our line tool. And we'll start with the base of the object. And we're using AccuDraw to do this. I'm going to draw straight across for a distance of 3.53. Now let's go ahead and zoom in a bit, so you can see this more clearly. And then I'll draw up, 1.02. And then back over, 1.22. And then over here on the left, I'll start here at the bottom left corner.
And I'll draw a line straight up at 1.51. So this is the overall height of the object. And then we'll come over to the right, a distance of .7. And then I'm just going to come down about an inch or so, maybe half an inch. We'll use the move parallel tool to figure out the base of the part here. So I'm just going to draw another short line segment here so I have something to trim to. And then I'll use move parallel. And then we'll go ahead and come up .59.
There we are. So now what you'll do is use the trim tool to trim the corners, and then just like we did in project one, we're going to be using the create complex shape tool to make a shape out of this. So I'm going to hit automatic. And then the max gap setting, I didn't really explain this before, the max gap setting is there if you have small gaps between the line segments. It'll jump the gap automatically. But since we've drawn this object with the lines touching, and they've been trimmed to the corner, there shouldn't be a problem with this max gap setting.
But if you are having an error message with the solid, or with the shape, then you may have to either adjust the max gap setting, or go back and retrim the corners just to make sure that everything is touching correctly. So we want to avoid any sort of overlaps or small gaps. So let's go ahead and use the complex shape tool. We'll click on one of the lines, and then just click an open space. And it should track around. And then you'll click one more time. You'll see the shape close message here. So let's click again. And now we have a completed shape.
So let's go ahead and tile the views again. And then I'll fit each of the four views. So now because we set this to a smooth shaded type display mode from last time, we can tell that this shape has been enclosed. So now we're ready to do the extrusion. So we have our profile. So we're going to go down to feature modeling. You're looking for the extrude feature command, which is in pallet A. And then we'll go ahead and extend this the width of the part, which is 1.54.
So now click in the top view, just anywhere on the shape is fine, and drag up. And then I'll fit the view again. So now we have the rough shape of the part. I always like to compare this to machining, so we're starting off with a machine part and we're going to be making progressively more detailed cuts and other features to the part to complete the model. So it is a lot like the machining process, I think. So let's go ahead and rotate around. So our next step is to place the shape for the cut.
So the dimensions for the cut, we can derive these from the dimensions of the part. The depth into the part is .59, and then the width of the cut is 2.15. Let me just switch over to the PDF file so I can illustrate this a little bit better. So here's the PDF file. So what I did is I took 3.53 and just subtracted 1.38, which gave me this distance. And then subtracted .95 from 1.54 to get .59 distance.
So we're looking for the shape and size of this cut. So we're just going to use like a rectangular shape to make this cut. Okay, so let's go ahead and find the shape tool. So that's in drawing. And then we'll go down here to place block. They call it block. We do have a shape tool but block'll work fine here. So now I'm going to snap here on this corner. And one thing you'll notice is as I add the shape, it's aligning itself to the view because that's how the AccuDraw compasses. So this is a major feature with Microstation in that if we're going to be drawing a new object, we want it to align to the AccuDraw compass.
So we have a shortcut that we can use to align the AccuDraw compass to the top orientation, which is the letter t. So we already have the AccuDraw compass activated, or focused, so we just hit t, and you can see how the AccuDraw compass has now oriented itself to the top view of the part. So now I'm just going to put my cursor out here in the rough location of where I want the cut to be. And then I'm going to type in the x-value, which is 2.15.
And then my y-value will be .59. So that'll give me the correct shape of the cut. So I'll click to accept the shape. So now I'm ready to place the cut on the part. So I'm going to go down here to feature modeling. And then, the create cut, or cut feature tool I should say. So the way the cut feature tool works is you can either go in both directions, one direction. We're going to choose the one direction option. So I'm going to uncheck both directions.
The Inside Profile method is what we use to create a cut that will remove material where the shape is. But you also have two other methods here. You can use Split Solid, which would just split where the shape is, or Outside Profile which is like a negative version of what we're doing here. But we're going to keep it at Inside Profile, and then we're going through all faces. You can also put in a draft angle if need be, we're not doing that, but if you want an angle to the cut, you can set this to a degree setting. And then thickness is for shell type surfaces, so we're not going to use that.
So I'm going to click on the solid first, and then the shape second. So now I'm moving my cursor up and down, and I can choose which direction to go with the arrow. So of course, I want to go downward. So I'm going to click down into the shape, and then click my mouse, and there's my cut. So I'm going to click one more time to accept, and now I've made my cut.
- Navigating the interface efficiently
- Creating 2D views from 3D solid geometry
- Creating a complex shape
- Creating dimension styles
- Creating a 2D view with title blocks
- Dimensioning and printing a drawing
- Beginning the 3D solid
- Drawing and dimensioning a plate, bracket, and more