SolidWorks LoftSweepExtract

Today we're going to talk about a few different ways to create new features. We're also going to talk about how to put an object into a drawing so that we can use it for machining or giving other people. I have already taken this document and put it in the ANSI drafting standard and I have chosen the units to be inches. The first feature that we're going to create is going to be a loft. And for a loft I want two shapes in space that I am going to connect with material. So the first thing I'm going to do is go to my right plane. And I am going to create a sketch on that plane. I will put a circle that has as its center the origin. I'll make it an arbitrary size, I would wanna choose a size for it if this were actually a part. I will finish that sketch, go back into my isometric view and now I need a second profile in space to connect this one to. And the best way to put it out into space is to use a 3D sketch. So what I will do is go back to the 'Sketch' tab, I will choose the right plane again, and I will create a plane in the 3D sketch. So I will click and I will tell it that I want it to be, maybe 3.5 inches away from my original plane. I will choose 'Okay' and now I have a plane that is 3.5 inches away from my first profile. I'm going to finish this and create a new sketch on this new plane. So I will click on the plane and I will create a new sketch. I will create a second circle that, again, is centered around the origin. And I'll make it a little bit bigger. It can be smaller, it doesn't matter. Now I am going to go back to 'Features', I'm going to exit out of my sketch and I will do a 'Lofted Boss Base'. Now it already chose my big circle so I'm gonna choose the little circle as the second profile for my loft. I don't want to hit 'Okay' yet because if you can see these lines that are going from one profile to the next are twisting around. And I don't want it to be twisted around. So the way to take care of this is to move these little green dots around so that they line up with one another and go straight from one circle to the other. This can be a little difficult to see and to get to the correct place. So I am going to use the 'Normal to' command and I am going to let that help me get these one right on top of the other. When I am successful with that I will no longer see all of those lines going between the profiles. Now I can click 'Okay'. I will put it back in isometric view and I have my loft. The next thing we're going to look at is the 'Dome' feature. So I will click on 'Dome' and then all I need to do is click on some sort of circular face and it will start creating the dome for me. I can change the radius of the dome from really big to small. I'll choose something somewhere in the middle. And then I will hit 'Okay' and and it's created a dome on the end of my loft. Alright, we're in a new document, still with the same settings. Now I want to show you the 'Sweep' function. So what I'm going to do is, again, create a sketch on one of my planes. We'll go ahead and do the front plane. Go to 'Sketch', create a sketch, and I am going to create an Allen wrench. So what I want is a hexagonal profile. And I will place the center of my hexagon and then I will decide how big I want my hexagon to be. I am going to choose to make it actually, only a quarter of an inch. And then I will hit 'Okay' and I have this little hexagon. I could've done a number of different polygons with any number of different sides. I will then hit 'Okay' and finish my sketch. Next I'm going to create a path along which SolidWorks is going to create this sweep. So what I'm going to do is, this time, click on the top plane and I'm going to create a sketch, and I'm going to make it so that I can see it by using the 'Normal to' function. And I am going to create the shape of my Allen wrench. So let's create it Something like this And then I will finish my chain. Now I am finished inserting lines but I don't want there to be this square turn here. So I want to make that a smoother turn and I am going to use a fillet for that. So I am going to click on my two lines And I am going to change my fillet parameter, I'm going to make it bigger. So maybe something like that. And then I'll hit 'Okay'. And now I am going to finish my sketch. Go to 'Features', 'Swept Boss Base' It already chose the path for me, I am going to choose the profile. It'll preview the sweep for me. And I will hit 'Okay'. And now I put this back into isometric And now I can see my Allen wrench. The last thing I wanna look at for features is how to create a linear pattern. So once more I'm going to create a sketch. And I'm just going to extrude a rectangle so I have a block. Now I am going to create a sketch on the face of this block. And I am going to put a rectangle on the block and I am going to use that rectangle to cut out a hole. Now if I want to repeat this rectangle so that I have more than one hole I can use the 'Linear Pattern' function. So I am going to leave my cut highlighted. And I am going to choose 'Linear Pattern'. Now I can choose up to two directions So I can do a linear pattern going along this axis and I can also do a linear pattern going along this axis. Now I am going to change the spacing. of my linear pattern so I am going to put each of these about 3 quarters of an inch apart. And I am going to create maybe nine of them. Now if I also want a pattern in the other direction I am going to, in this case, go one inch apart. And I am just going to make two of them. So this creates a linear pattern I am then going to hit 'Okay'. And now I have a pattern of holes in my block. Now what we're going to do is take this block and we are going to put it into a drawing. So I am going to save it because you have to save a block before you can put it into a drawing. And then I am going to go up to the 'New' menu and create a 'Drawing from Part/Assembly'. The first thing its going to ask me for is my sheet format and size. I will browse for this and I need to go into the Class Drive, go into FEH, 1282H, templates and I am going to choose the OSU Drawing Template. And I will open that and I'll leave everything else the same and I will hit 'Okay'. Now this 'View Palette' shows up on the right side and I can use that to insert my drawing. Or I can go over to the 'View Layout' menu I'm going to use the 'View Palette' this time. And so what I'm trying to do here is to create a set of orthographic views. I like what it's chosen for the front view and I am going to use that for the front view but I don't if I liked the top view better as the front view I could put that as the front view it all depends on how I modeled my part. So I'm going to drag my front view onto my sheet. And then as soon as I've done that it's going to allow me to drag out additional views. So I'm going to put a top view I'm going to put a right-side view and I'm going to put an isometric. Don't worry too much about exactly where it places it, you can move it later. Then I am going to hit 'Okay'. I"m going to move my isometric around. And this is — this is getting there. Now one problem I have here is that these three views all showed up with hidden lines, and I'm going to want to verify that. If they all show up with hidden lines then I'm in good shape If not I may need to add them in. This view over here showed up with hidden lines as well. And I don't want hidden lines in my isometric view because these are all through holes. So what I'm going to do is click on this isometric view And I'm going to un-check 'Use Parent Style', Then I'm going to look at these different views here and I'm going to choose the one that doesn't show hidden lines. It's called 'Hidden Lines Removed'. If for some reason one of my principal views showed up without hidden lines, I could do something similar I could instead click the button that says 'Hidden Lines Visible' but for my isometric views I don't want hidden lines And then I am going to close the dialog. These are filling up the page pretty well. Sometimes that won't be the case. So if that's not the case then I will click on this front view and I can change the scale to use a custom scale. So I can make it bigger, I can make it smaller. 1:2 is actually a pretty good scale for me so I'm going to use the sheet scale. Here in the drawing I'm going to want to go back up to 'Document Properties' and verify one more time that my drafting standard is put into ANSI. This is going to become extremely important when we start dimensioning these parts. Now I have all of my views on my sheet, and and the thing I have left is to change my title block. So I'm going to right-click on 'Sheet Format' and choose 'Edit Sheet Format'. Now my views are all going to disappear. And that's okay, don't panic when they disappear. Now what I'm gonna do is go down to each of these sets of X's and edit them. So I'm going to double-click on drawing title, and I'm going to give it a funny title. And I'm going to double-click on 'Drawn by' and I'm going to type in my name. The one thing that you're — that shows up on this title block that you are not gonna have is a seat number So you're just gonna double click on that and put in 'N/A' And anytime I'm done editing text I can either click the little check mark or I can just click out anywhere else on the sheet. So you would go through and fill in the rest of these X's with the relevant information Once I'm done I'm gonna go up to my upper right-hand corner and I am going to finish editing my sheet format, and all of my views will show up again. Before I print this I need to go to 'File' 'Page Setup' and make sure that I choose 'Scale to Fit'. This is going to make sure that my whole sheet shows up on the page when I print it. Then I'll hit 'Okay' and then when I'm ready to print my sheet I will just go up to 'File', 'Print', and print from there. Now, we have put this part here, on the drawing sheet. But this hasn't forced us to create any centermarks or centerlines. And we should do that. So I'm going to go back to my original part and I am going to add a hole that is a circle. So I'm going to put a circle somewhere here on the part. I'm going to close that dialog, exit the sketch. and create an extruded cut of that circle. Hit 'Okay'. And now if I save my drawing over here And I go back over to my drawing you can see that my hole has shown up. So now what I'm going to do is add in my centermarks and centerlines. I will go to 'Annotation' and I will go to centermark, and I am going to choose my circle here. Remember we don't put centermarks on isometrics. Once I have chosen all of the circles that need centermarks, I am also going to put on centerlines. And so the side view of this hole is over here, so I choose the two lines that are the extreme elements of the hole and I put the centerline between them. Up here its a little harder for me to see which ones are the hidden lines representing the circle. I believe its these two so I add a centerline there as well. So that is it for lofting, creating domes, sweeping, creating a linear pattern, and creating an annotated drawing.