Add the top tube - SOLIDWORKS Tutorial

- [Instructor] The next part that we're going to add to the assembly is the top tube, which as we know and as the name suggests, is the one that goes along the top of the bike. Open the assembly that you've been working on, and it should look something like this. We're going to follow a similar process to how we added the seat tube. So firstly, let's insert a new plane to sketch this new top tube on. Go to the assembly tab, and click on reference geometry and choose plane. And for the first reference, let's click on this top line, and for the second let's choose either end, I'm going to choose the front end. So now we're adding a new plane that's perpendicular to that line on the end of that line. Press okay to add it, and I'm going to rename that plane as top tube plane. Now let's insert a new part again. Go to assembly, insert components and click on the dropdown and choose new parts. Now, similar to the previous video depending on your settings, you might have to input a file name directly at this point, or you might just get directly to this stage where you've got this small green tank next to the cursor. If you're prompted to enter a file name then just call it something like top tube. And then we should be back in the assembly ready to select the plane for the new part. Select that latest plane that we just added, the top tube plane. So now we're sketching a new part on that new plane. Similar to the seat tube, this tube consists of two concentric circles started on the end of that line. So let's get the circle tool, and then zoom in, and just draw two circles at the start point in there. This top tube is a bit of a smaller diameter than the seat tube. So we'll get the smart dimension tool. This one is 25.4, so it's one inch in Imperial terms. And then the wall thickness is a little bit less as well. So grab this second circle, drag it inside the first one. And then for the wall thickness is 0.8 millimeters. So just select both circles and let's add in 0.8. Now let's extrude this profile by going to features, extruded boss/base, and let's extrude all the way down to the seat post here. So for the end condition here on the left, let's go to the dropdown and choose up to surface, and then just select that seat tube. So it should extrude all the way along to that seat tube. You might have to flip the direction by clicking this button here on the left. Let's press okay to add that new feature, and then exit editing this part by clicking up here in the top right. Now we've got this new part here, so we can rename it depending on your new part settings. So if you need to rename it, if it's called something like, part two, then you should right click on it, choose rename, and let's call this top tube. Then we can also save the assembly, and you might be prompted to save your file externally. If so, just click save externally and then click on top tube, press same as assembly and press okay. So now that top tube is added as a new external part. So now we can see the frame starting to come together quite nicely, but you might see an issue. If you can't see any problems, try going to the evaluate tab, clicking on interference detection, and then just press calculate. And we can see we've got a small problem here. The top tube is actually clashing with the head tube. That's because we didn't actually notch it at this end, we only notched it at this end. So like many problems in SolidWorks, there's a few different ways we could solve this. We could use a cavity feature and cut away that interfering section, or we could manually cut the notch. But actually the easiest thing to do is just close this interference detection tool, and then we can edit this part by clicking on it in the parts tree and press edit part. Then let's expand the part and edit that tube feature. So click on the feature, press edit feature. Now we can actually offset the start of this tube and we can use an up to surface end condition on this end as well. To do this, go over to the left and here where it says from, click on this dropdown and change it to offset. Then let's increase the offset, so we're no longer in the middle of that tube. Let's try 30 millimeters, maybe you need to go up to 40, that seems to work. You might need to flip the direction by clicking this button so we should be offset and in this direction. And then before you press okay, let's also activate direction too by putting a check in this box. And then for the end condition, let's choose up to surface, and then let's just select our head tube surface. So we should be going all the way up to the head tube like this. Press okay. And now that looks great at that end and at that end. So we can exit editing the part by clicking up here in the top right. Now if we do interference detection again by clicking on the tool and pressing calculate, you can see we've got no interferences, so that all looks correct. So then if you like, you can just open this part and have a double check in the part. So it looks good at this end and it's also notched correctly at this end. So if we go back to the assembly by pressing Control + Tab, by using those up to surface end conditions, we know that both of the ends are correctly notched. We know that we haven't accidentally cut the wrong angle by cutting it manually. This can be especially helpful because none of these angles are actually 90 degrees. So at this point you can just save your assembly and we'll continue on in the next video.