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SolidWorks Relations

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Today I want to show you a few things that will be helpful on your second day of SolidWorks. The first thing that I wanna show you is how to change the units of a part or a drawing. So I'm gonna go back up to that 'Options' that I used to change the drafting standards. I'm gonna go to 'Document Properties' I'm going to change my drafting standards to ANSI like we talked about before I'm going to go down to 'Units' and I am going to choose the units system that I want I, in this case, want millimeter, gram, second system, you may want inch, pound, second; you may want centimeter, gram, second; it's up to you. But whatever units system I choose, if I have a dimension of 1 then it'll either be 1 millimeter, 1 centimeter, 1 meter, or 1 inch. Now I want to go over a few things with relations, which are also known as constraints, you may hear them referred to as either one. So what I'm gonna start by doing is creating a couple of rectangles. I already have a sketch open. I had that open when the video started. So I'm going to create a couple of rectangles in a plus sign. I'm going to click the green check mark to indicate that I'm finished with rectangles. And now let's say that instead of a plus sign I wanted it to be an upside down T. One of the options I have for doing that is using relations. So I would go to the 'Display/Delete Relations' button I'd click the little drop down arrow and I'd choose 'Add Relation'. Now because I already had a rectangle selected All of the elements of that rectangle show up in this 'Selected Entities' box. And I don't want all of those right now, the selected entities are the things I'm going to apply the constraints to And I don't want that. So I'm going to choose each of these and hit the delete key over in the 'Selected Entities' box and it unselects them. Now I'm going to choose the two lines that I actually want by clicking directly on them. So I'm going to click on this line and I'm going to click on this other line, and now I have a list of relations that has popped up that tells me the different relations that I can try to apply to these lines. Not all of these will work all of the time. So some of these, depending on what constraints I have going on in my model will interact with other constraints or interfere with other constraints and cause problems. So I need to think about what relations I'm adding. I'm going to add a co-linear relation in this case and it takes two line segments and puts them on the same line. So now I have this upside-down T. But let's say that I've decided instead of an upside-down T I wanted an L. I'm going to unselect my entities again by clicking on the entity and choosing delete. And now I'm going to click on two points I'm going to click on this point and I'm going to click on this point. Now I'm going to see a new list of relations And I am going to choose the 'Merge' relation which puts the two points at the same place. So now I have this upside-down L. And I can leave the Relations menu and I can move things around but those constraints that I've put in place will stay. Now let's look at another relation. So what I'm going to do is create a circle somewhere here in the middle of this L. And let's say that I want this circle to actually be tangent to both of these lines and to appear up here as an arc. So I'm going to close my circle dialog, and I'm going to go back to 'Add Relations', and I already have the circle selected, that's 'Arc 3' And I'm going to select this line over here and I am going to add a Tangent constraint. So now the circle is tangent to this line here on the left. I'm going to deselect that line, which can also just be done by clicking on it if its already selected, I'm going to select the other line, and I am going to add another Tangent constraint. So now both of those lines are tangent to the circle. Now what I want to do is to move the circle up. And there are a few different ways I can do that, you're actually going to use a different way in the tutorial, But let's add another relation, I'm going to deselect the arc, and the line and I'm going to select the point in the middle of the circle, and I'm going to select the point at the top of the line, and I am going to choose the horizontal constraint. So now those two points will always be horizontal from one another. Now let's say I don't want all of these lines here in the middle of my profile. I can use something called the 'Trim Entities' command. So there are a few different options here. The 'Power Trim' is pretty powerful, all I do is drag my cursor over the lines that I want to go away while holding it down, and I release and I am left with just the profile that I want. Then I hit the 'Undo' button. Instead I can do a different trim command which is 'Trim to Closest' and I can choose one line at a time. So really either one works. I also have something called the 'Extend' command, So let's say that I did actually want to create a line across here, for some reason, so I'm going to add a line that goes to there, and I'm going to end my chain. Now my line only goes half the way across. If I want it to go the rest of the way across, I'm going to choose 'Extend Entities' and I'm going to click on that line, and it extends the line to the next line. So that's Trim and Extend. Now we talked about relations for geometry, so tangent and merge and horizontal and co-linear, I suggest that you do look up the other ones in your book. There is another way to work with your sketch so that it retains certain properties even as dimensions in other areas are changed. So let's say I want this top leg of the L to be the same width as the bottom leg of the L. What I'm going to do is go to 'Smart Dimension' and I am going to start by dimensioning between these two lines, and creating a dimension there, and I will hit the check mark I will create a second dimension down here and I'm again going to go between lines, and I am going to place my dimension. Now if I want these two dimensions to be linked, I'm going to go to 'Tools', 'Equations', I'm going to make sure the 'Automatically Rebuild' button is checked, and I am going to add an equation here. So I'm going to say that I want the second dimension to be equal to the first dimension so I click on the second dimension first. It automatically populates the equal sign, I click on the second dimension and now the two are linked, so when I click 'Okay' it rebuilds my sketch, it actually exits the sketch when it rebuilds and now the two widths of my L are the same size. So now if I go in and edit my sketch and I modify this dimension here to maybe be 30 and I hit my check mark then both of my dimensions update to be 30. Now let's say I want the other end of my L to also have an arc on the end. There is a feature built into SolidWorks that allows me to do this really easily without having to look for the Arc Sketch tool. So I go to my Line tool, I click on the corner where I want to start my arc, and I start out drawing a line. If I come back to the origin, and start drawing again it actually changes it into an arc. So then I click on my second point and I've created an arc on the second end. Note that these tangent constraints showed up automatically. So I don't need to go back and add tangent constraints because they're already there. So I'm about done with this sketch. One thing that I am going to do is to get rid of a couple of extra lines here. Just because it makes things easier when I go to extrude so I'm going to delete that line and I'm going to delete this line. I could have also done that using the Trim command. So now that I have my sketch I am going to go to 'Features', 'Extruded Boss Base', I am going to click on the profile I want to extrude, 10 millimeters is fine, and I'm going to click the check mark. So now my object has been extruded. Let's say that I want to add a fillet a couple of places here so I'm gonna add a fillet to this joint here and a fillet down here on this sharp corner. So I'm going to go to the 'FIllet' command, I'm going to leave it at 10 millimeters, and I am going to choose the corners that I want to have filleted so I'm going to choose that corner and I'm going to choose that corner and I'm going to hit 'Okay' and they both now have a 10 millimeter fillet on them. The last thing that we didn't go over in the last video is how to make an extruded cut. So I am going right-click on this front face and add a sketch. So I have a sketch there now. I'm going to draw a circle and I am going to click 'Okay', then I am going to go to 'Display/Delete Relations' and I'm going to add a relation between that arc and this arc and say that I want them to be concentric, so this lines up my arcs well. And then I will hit 'Okay'. I will go to 'Features' and now instead of 'Extruded Boss Base' I am going to choose 'Extruded Cut', I am going to say that I want it to cut 'Through All', though, I could just choose a distance, and I'm going to click 'Okay' and now it is going to create a cut that is the shape of that circle all the way through my object. So those are the things I wanted to show you today Hopefully they will be helpful on your tutorial and your homework.

Video Details

Duration: 10 minutes and 52 seconds
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Language: English
License: Dotsub - Standard License
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Posted by: raghadkod on Sep 2, 2019

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