SolidWorks Feature Based

Today we're gonna talk about a few topics in feature-based modeling. So I'm gonna start by creating a new part and I am going to put a sketch on the front plane. And I'm going to create a part that is cylindrical in nature but has a complicated geometry and this is easier for me to do using revolution than extrusion. So the first thing I'm going to do is create a centerline that goes along the axis of the part that I'm trying to create. And I'm just going to put that along the x-axis. I'll finish my centerline. Then I'm going to use regular lines to sketch out the profile that I want to revolve. Now normally at this point I would apply all of my dimensions but I just wanted to show you a couple of dimensions because there's a trick to dimensioning when you're going to be revolving. So I'm going to open Smart Dimension and then I'm going to dimension between the line on my and the axis. Now if I stay between the part and the axis then I get the radial dimension. If I jump down below the centerline then I'm actually dimensioning the diameter that will exist once I've revolved the part. So I'll place another diameter here. And then the other dimensions that I'm going to wanna make will just be between the lines like before. So I'm not going to bother modifying these dimensions I would modify them to be the values that I want. I'll finish my sketch and now I want to revolve my profile. So I will go to 'Features', 'Revolved Boss Base', and and this time it automatically selected the profile for me. I may need to manually select the profile and the axis. This blank is where I select the axis and then I will also select the profile. So this looks like about what I want so I am going to click my check mark to say okay. And now I can see what I revolved. Now I want to create a hole patter on this face and before we've created holes by drawing a circle and using an extruded cut. This time we're going to use the hole wizard. So the hole wizard allows me to choose a wide variety of holes. I can choose what standard I'm using, whether the hole is threaded or not, and the size of the hole. I'm going to use a straight hole and I want it to be a quarter of an inch, and I'm going to make it a through hole. Now to choose my position I'm going to click on the 'Position' tab and I'm going to click on the face where I want to make the hole. and then it's going to ask me to position it on the face I'm going to place the around there. Now it puts me in the Sketch panel so that I can apply relations or dimensions to put the hole where I want it. So I'm going to add a relation after looking at my face between this point and this point that makes them vertical to one another. Then I'm going to dimension this distance and I'm going to make it a little bit bigger so maybe I'll make it 1.75 and that places my hole there. Once I'm finished dimensioning I can click 'Okay' for hole positioning and it will create my hole. So if I go back into isometric I can see my hole. Now I don't want just one hole, I want a pattern of holes. So now I'm going to use 'Circular Pattern' and I have to choose the feature I want to pattern and then I have to choose the circumference of something that indicates the circle I want to follow when I'm creating my circular pattern. So I'm going to choose this circumference right here and now you can see it creates a pattern of holes. This has six, I could move it up to seven or eight, I'm going to leave it at eight,and I'm going to click 'Okay'. Now suppose I wanted this to a long pipe with flanges on either end. One way that I could do that is to use the mirror function. So I am going to go 'Features', 'Mirror', and I am going to mirror this part around this plane and the 'Features to Mirror': it already chose this circular pattern for me but I also want to choose my first revolution. So I choose that and then I'm going to click 'Okay' and now I have a mirrored part. So this is my part Now I want to take this part and put it and put it in a drawing. So I will go to make a drawing from part assembly, it's going to make me save my part, again I'm going to have to browse for the drawing template and I will hit 'Okay', and now I'm in the OSU Title Block. Now when I go to place my view. This time I'm going to set down this left view as my front view. And the reason that I'm going to do that is to create a section view. So I'll place my left view down and then I'm going to add an isometric view and that is it for my projected views. And I don't like how big these are I think they need to be a little bigger on my page so I am going to use a custom scale, let's try 1:2 that's better. Now I want to create a section view based on this view so I will go to 'View Layout', 'Section View' now I want to draw my section line down the middle. So I'm going to hover over one of the parts that I know is in the middle and I'm going to go forward following the blue dotted line and I am going to draw my section line straight down and that will create my section view for me. Now I have forgotten to change it into ANSI so I'm going to do that. So let's go back to ANSI Alright. Now, not all my view have the right hidden lines. So this view should not have any hidden lines because it's an isometric and this view should not have any hidden lines because it is a section view and I don't show hidden lines on section views. Now I will need to add my centerlines to my views. So I'll click 'Okay' and I will go to 'Annotation'. My centermarks have already been taken care of except this centermark should extend all the way out past the edge of this outer circle. So I grab this little blue dot and I pull it along until it goes out all of the way that it needs to go and these lines would also come out although they are obscured by the section lines. Now I'm going to go to 'Centerline' and I need to put a centerline down the middle of this part, and I'm going to put centerlines for the circular holes. So now I have all my centerlines I have my views in place, I have a section view and I would go through and edit my title block, and set the page size and print.