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Dimensioning in SolidWorks

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Now that we have gone over the basics of dimensioning I would like to go over an example in SolidWorks where we're actually dimensioning an object. So here I already have my layout drawing with my three orthogonal views and my isometric pictorial. And so now I'm going to add dimensions to my orthogonal views. I'm going to start by placing the overall dimensions for my part. So I have overall width, overall depth, and overall height. To do that I'm going to click the 'Smart Dimension' button and I am going to click the line I want to dimension and drag the line away from the part. I could also dimension between lines just like i did when I was creating the part in the first place. Now I've placed these two dimensions the width and the depth in the top view because its really obvious in the top view that I am dimensioning a rectangle. If I look at the front view or the right-side view, its less obvious to me what the width and the depth refer to. Now when I place the height I am going to choose the front view mostly because the right view doesn't offer me any advantage over the front view. for now I can place these dimensions just about anywhere because I'll move them around later to make sure they're neat and aligned. Now that I've placed my overall dimensions I'm going to start giving sizes and locations for the features of my object. The first features I'm going to dimension are these holes that you can see around the base. I'm going to need to dimension their size and location. Now when I go to dimension their location I'm going to have to keep in mind the function of these holes. The holes are most likely going to mate with some sort of bolt pattern on the surface to which this object will be bolted. In order for that bolt pattern to match the bolt pattern that I have here on my object Its critical that these holes be properly located relative to one another. So to locate them the first thing I'm going to do is locate them between centerlines in both directions. Now that I have dimensioned between my holes I need to locate them on the object. If I were assuming symmetry I wouldn't need to do this but for now let's not assume symmetry and just place the necessary dimensions So I am going to locate to this corner. Now it might be tempting at this point to place another dimension right here, between this circle and this edge I won't want to do that though and the reason is I already know what that dimension is. If I know that it is 120 millimeters deep and I know this hole is placed 20 millimeters plus 80 millimeters away from this edge I know that this dimension over here has to be 20 millimeters. Now again, I've chosen this top view because I am dimensioning on these circles. When I go to actually create this part, to create these holes I'm going to look at this view, I'm going to locate these holes, and mark the center of the circle, and then get out my drill and drill out those holes. So I'm dimensioning my circles in the view where it's the most useful. N ow that I've dimensioned the location of my holes I also need to give their size. So I am going to click on my circle, and I am going to place the diameter. SolidWorks is usually smart enough to figure out that I am dimensioning a circle and so a diameter should be placed there. Now I have more than one circle here, I have four. So if I just wanna place one dimension instead of four I can do that, I just need to indicate that there is more than one of that feature. And to do that I'm gonna go over to the left to 'Dimension Text' and I am going to click all the way at the beginning of those variables there that stand for the dimensions of my part and I am going to type in 4 and a capital X. And that indicated that there are four of these 20 millimeter diameter holes. Now I'm going to want to give the location and size of this circular feature that goes through the object. To give the location I am going to place it relative to one of these holes. And again, that's because I know pretty precisely where the location of the hole's going to be bolted into the bolt pattern underneath it. So that gives me a better definition of where the central feature is going to end up. So I place the dimension there and now my circular feature is located. To give the size of the hole that goes through the circular feature I'm going to dimension it where is looks like a circle, though as a concentric cylinder it may be more accurate to dimension it in the longitudinal view. The overall cylinder is a positive cylinder so I'm going to dimension it down where it looks like a rectangle So I've located and dimensioned the size of my holes I've given the size and location of the central feature. The only dimensions I'm missing now are the location dimensions for this base feature relative to the top and bottom of my cylinder here. I'm going to do that in this front view down here because, again, there's no real advantage to using the right-side view and I'm going to choose to use datum dimensioning because I do not know exactly what is the critical dimension for this part. I'm not sure if the width of this base part is going to be important, or if the distance between the base and the bottom of the cylinder is going to be important, I don't know. So since I'm not sure, the safest thing for me to do minimize tolerance buildup. So now I have placed all of my dimensions, I'm going to wanna make sure that they're nice and neat. So I'll click out of dimension and I'm going to wanna keep them not too close together they also don't need to be spaced out quite this much. You can look in the book if you would like more precise definitions on how far apart the dimensions should be from one another. So at this point the dimensions are nice and neat, no dimensions are overlapping. I can tell which which dimension arrow each of these numbers is associated with. I'm going to wanna go back through and double-check all of my annotations, do I have all of my centerlines? So I do in this view. I do have my centerlines in this view. But if I look over here in my right-side view I'l notice that I'm missing centerlines for my holes. So I'm going to go back in and add those to make sure that I have all of the centerlines for my drawing. I would then check to make sure that I have dimensioned and located all of the features of my object as well as making sure that I can tell what the overall dimensions of my object are. Now looking back through, you can see that this cylindrical part is dimensioned in the horizontal direction but I don't have it located in the vertical direction. So I'm going to move my dimensions out a little bit to make room for it And then I am going to add that dimension. Now this part could also be dimensioned using the assumption of symmetry, that will be covered in the tutorial that you will do in class.

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Duration: 9 minutes and 5 seconds
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Language: English
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Posted by: raghadkod on Sep 2, 2019

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