Skill Level Appropriate for all
- [Instructor] In this week's example, I'm gonna be showing you an easy way to create a fish-mouthed tube connection that looks like this. You can see here I've got two pieces of tubing coming together, and I've got a nice profile here that easily makes those two things blend together with no gaps so it's gonna be really easy to weld at whatever angle we specify. Or whatever sized tube or pipe that we are using. To do that, I'm gonna jump over here to this sketch I have, and it's basically just two lines intersecting. So let's go ahead and take a look at that sketch, just start her off so I have a 12 inch piece of tubing that's gonna be down here, an eight inch piece that's gonna be intersecting it at 60 degrees and I've just got it four inches from the edge.
Doesn't really matter here, we're just creating some type of angle here, to create the shape. We can always go back to this angle again and change it to create any types of different patterns for any different angle that we need, okay. Back to my sketch, now I'm gonna choose this line right here, I'm gonna go over here to features, come up here to reference geometry and choose plain and I'm gonna choose that line and then the point at the very end of it. So I'm gonna create a reference between that line, that point, and it's gonna put a plane right through at the end of that line. Click on okay, now let's go head and start a sketch on that plain, and I'm gonna spin this thing around so I'm looking kinda straight down on it and start a circle right there.
Now let's go head and specify a two inch diameter. I'm gonna then click on normal two and then zoom in on that sketch and then I'm gonna create a couple of center lines, so from the origin, I'm gonna draw a line directly up here to the circle. And then again making one more line over here. Now I'm gonna find about a one degree angle between the two, so one degree, and then I'm gonna go over here to my trim tool and just trim it away, and the reason I'm going that is I don't want one continuous circle, I want most of a circle, because I wanna turn this into a piece of sheet metal and I wanna roll it or unflatten it.
So if it was one continuous circle I wouldn't have that ability, I'd need to cut it and that's what this tiny little one degree angle is here. So I don't have one continuous shape, it's basically just a piece of rolled material. Click on okay, now let's go over here to Sheet Metal. Create a Base Flanger tab and you can see here I'm going this direction, instead of blind I want to go Up To Vertex, and I have this little point right there, click on okay and there is my piece of tubing. And you can see it's already got a cut in it, so you can see it's actually more like a piece of sheet metal that's been rolled around to create that shape.
Okay, the next thing I wanna do is I wanna cut away this other piece of pipe, so going here on the front plane, I'm gonna go head and start a sketch, and go head and just draw out a circle starting at the origin and draw it out, give it a dimension. I'm gonna type in 2.5 okay and then just go to features and extruded cut, alright and I'm gonna go Up To Vertex again just choose that point at the very end, so I'm gonna be cutting through here.
And notice we have a couple options. I have this option to do a Normal cut, so it's gonna be cutting this tubing here, this piece of sheet metal as if it was a Normal cut. Like it was flat pattern like on a laser and then cut around, so you have that option, or you can turn it off, so I'll show you the difference between the two so let's just go ahead and just leave it on for right now. Click on okay and you can see here that it has actually cut it away and you can see that's a Normal Cut. So you have a couple things that are kinda interesting here, whereas like these little transition points here and here, right in there and there. And just how it's kinda built, and I'm gonna show you what that actually means in one second here.
First what I wanna do is create from the front plane, right where we had that other sketch, right here, I'm gonna go ahead and create a surface, an extruded surface and we're gonna go blind up to that vertex. Now this actually is not doing anything for us, it's just allowing us to kinda see what's happening with this cope surface, so you can see that we've got a little bit of an edge here, you can see this little edge sticking up here and then it kinda blends as it moved to this other side, and that's what you would get if you maybe took a piece of sheet metal, laser cut it as a flat pattern and then rolled it up and that's a Normal cut, now if I were to change that.
So instead of this extruded cut here, I would change that to a Regular cut, not a Normal cut, click okay and now you get a completely different shape. You can see that one actually completely blends around there. So it really depends on how you're gonna be cutting or coping out this piece of tubing, whether you choose the Normal cut, or the regular cut like you see here. So the end result here is that I wanna create a flat pattern that I can then print out on a piece of heavy card stock and then fold or roll around a piece of tubing, then use a marker, draw out my shape, and then take it over to a saw and grinder.
Grind it and shape it to the size so that when I do mate these two pieces together, in the real world and get ready for welding, that they come together with a perfect angle, and there's no gaps so it makes a really nice weld and everything looks really good at the end of the day, so that's our plan. Alright so choose either you want the Normal cut, or the non-Normal cut, I'm gonna switch back to the, let's go ahead and edit that feature here. Back to the Normal cut, you can see it there. Alright, now I'm ready to create a flat pattern. So if I go over here, I can just choose this surface here or go over to Sheet Metal, and just say Flatten right? And there's my shape, that's what this thing's gonna look like at the end of the day.
Which is, you know a fairly complicated shape, it would be very difficult to figure that out on your own. Now I wanna be able to take this and kinda save this out as that 2D pattern, now to do that I'm gonna go head and right click and click on Export to DxF / DwG. I'm gonna go head and overwrite this flat pattern here. Click on save, and say Yes. Now it's gonna ask me a few questions here, over here I say well yes I'd like to export that face, and it's not required but you can align your output and in this case it's probably helpful to do that.
So click on the X axis, I'm gonna choose this line right here or this edge, the Y axis I'm gonna go head and choose this line right here and that's gonna get everything aligned perfectly. Then go head and click on Okay. And you can see there that's an example of what the flat pattern's gonna look like and this again is what we're gonna then save out, print it out on a piece of paper or a piece of heavy card stock and I can wrap that around my tubing, and it should show up exactly the right size, for when it wraps around and then take a marker. Draw that shape out and then you can take it over to a grinder or cutter, cut that shape exactly and when they mate together, when you're actually getting ready to weld it.
Everything should match up perfectly, and be good to go. Go head and click on Save, and there you have it. So that's a quick way for creating a very complicated pattern for fish-mouthing or coping out a tube to tube connection. Now, we can always go back, unflatten that shape here, go back to my original shape here, change the angle if I wanted to, everything automatically updates with the shape and I can continue to do the same thing. I can also go back and change the size of the different tubes, you get the different shapes and you can pretty much use this part here, that you've created as a universal pattern for any different size of tubing, or any different angles that you might be working with in the field.
Hopefully this helps out, with your next project. Thanks for watching, and check back next week.