Ceci est une ancienne révision du document !
Welcome back! Ok, I need you to create a new project, a new body, a new sketch, add a centered rectangle, and stop there in the Sketcher workbench. Let’s look at getting this piece locked in place and adding (or removing) some bits. If you look in the left panel, you’ll see a bit that says ‘2 DoF(s)’. This means two things aren’t locked in place. Not the end of the world, but it means items could move and mess things up later. You can click the ‘2 DoF(s)’ link and it’ll show you what’s not locked, but I can tell you that it’s all four corner points. In other words: we can move all four sides. The middle is locked in place as we did that by choosing to make the rectangle from the middle point outwards. So, left-click on the top edge of the rectangle and it’ll change to green. Now left-click the Constrain horizontal distance icon. This will give us a popup that’ll let us lock that size in place.
I’m going for 40mm. You’ll see that we now have a size on our drawing. Let’s do the same for the left or right side, but choose the vertical icon beside the horizontal and make it 30mm. Lovely. Now you’ll notice the whole thing is green. This is because it is locked in place and can’t be moved by accident. The left panel also says ‘fully constrained’. I’m not keen on the 30mm text being on the inside though. You can click and drag on it to move it outside the box. I prefer that. Now, you could close that and go back to the Part design workbench, and pad it, but let’s add some circles inside it. We’ll think of those as screw holes for now. Click the Create circle icon. Same as the rectangle, we'll need two clicks to draw the circle. One in the center and one on the outside edge. So, make two circles inside the rectangle. I’ll put one to- left and one bottom-right. Don’t forget to right-click (or Esc) to come out of creating circles mode.
If you need to move the circles, you click and drag on the center point. You can click and drag on the circle outline to resize it.
Let’s lock a size in for these circles. Click the outline and choose the Constrain arc or circle icon. This is currently set for diameter, but you can click the down-arrow and choose to make it a radius if you like. I’ll make it 6mm. I need the other one to be the same. So click the outline of the 6mm one we just did, hold down the CTRL key, and click the other circle. Now click the Constrain equal icon. It looks like a big red equals sign (. Voila! The two circles are the same.
If you double-click the 06mm label on the top-right one, you can change it, and it’ll change them both. Try it. Set the top-left circle to 5mm.
We need to constrain these to make sure they’re in the right place. Click on the center point for the circle top-left. Hold down CTRL. Click the top-left corner of the rectangle and choose the horizontal constraint (like we did with the rectangle sides). Let’s go with 8mm. Select the same two points and choose vertical constraints and choose 8mm again.
I’ll let you figure out how to do the other circle.
So now our drawing is green and all locked down. Again, like last time, click Close in the left panel. This time, though, look at the top icons in the Part design workbench. See the yellow and red ones? Well, yellow means add, red means remove. That first one with the yellow box is the pad icon. It does the exact same as we did last time. Click the pad icon and make it 2mm this time. If you want to marvel at your creation you can use the middle mouse button (or scroll wheel held down) to move the model about. Hold both middle and right buttons to rotate. On the left panel, click the right-arrow beside Pad. This will show a greyed out Sketch below it. Double-click the Sketch to go back into it. Feel free to add another two holes to either corner of the rectangle to give four holes. We’ll start with that four hole plate next time.