Discover the steps to add detailed designs to a 3D model of a fork using sketching and cutting techniques. Learn how to create triangles, apply mirroring, delete unnecessary lines, and give your sketches specific names for better organization.
Key Insights
- The article provides a detailed guide on how to add details to a 3D model, specifically a fork, by using sketching and cutting techniques. This involves creating a sketch, hiding the fork, using the sketch to create cuts, creating angle cuts, and projecting lines to provide a reference.
- One can create complex shapes like triangles by using the line command. The article also explains how to mirror these shapes across a line for symmetry. Unnecessary lines drawn for reference can be deleted once the shape is complete.
- Naming each sketch and giving it a specific profile is essential for better organization. The article outlines the process of extruding the sketch and selecting the profiles, changing the direction to symmetric and adjusting the distance to ensure a proper cut. Finally, fillets can be added to the edges for a smooth finish.
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Now let's add some details to our fork. Let's begin by expanding the Bodies folder and giving our body a name. It's going to be our fork.
Now it has a name, it's a body, it's called Fork, and we want to add some details and we'll do that by sketching. So first we'll click on nothing, everything's deselected, and now in our Create menu let's go for Create Sketch. We want to create the sketch at our construction plane called Fork Center, so we'll click on that, and we're looking directly at our fork.
Now our first step is to hide the fork. So with that Bodies folder still expanded, let's hide the fork itself and zoom into our Wheel Center. We're going to use the sketch to create some cuts in our fork.
The first cut we want to go ahead and go to Create and look for Center Diameter Circle. We'll click right in the center of our hub one time, pull that out, and we'll type in 5 for 5 millimeter. So that was pretty easy.
Now we can turn on our fork and we also want to create some angle cuts on both sides. This will be a little bit trickier because it can be hard to find exactly where this ends. We can see we're getting a couple of end points there, but let's go ahead and under Create we're going to find Project Include and select Project.
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Now we can click this line from our other sketch that goes right down the center. If we don't see that sketch we want to turn on that Fork Angle Sketch, make sure that's visible, and then select that line and click OK. So that gives us a purple line down the center to provide us with a reference.
We want to create two triangles. Let's start with one side and then we'll mirror it over. We'll find the line command.
We'll start right in the center of our hub. We'll click one time and go straight down. If we're going straight down we will get these little double lines that let us know that we're parallel to that original purple line.
We'll go down and let's go ahead and type 12. We'll go down 12. Now we'll click our line tool again.
We'll click right where we left off and we will go to the left and let's say this time we're going to go to the left about 10. Type in 10. There we go.
Let's continue on. We'll click right where we left off. Go straight to the left.
Make sure that we're drawing parallel. We'll get those double lines and this time we'll type in 12. Click our line tool again.
Click where we left off and go straight up. We're going to get that little constraint that lets us know we're moving at a 90 degree angle. That's what we want, 90 degrees.
We're going to go up almost to the wheel so it's going to be 80 millimeters. We'll type in 80. There we go.
Now we'll click our line command again right where we left off. We're going to go from that point all the way down to our point right here. We created a double line here 10 and then 12.
That point right in between. We'll click and there is our triangle. All that work just to get our triangle.
Now we can go ahead and mirror that triangle across our purple line. We'll find under the create menu, mirror. We will select every line of that triangle.
Find our mirror line and we'll click select there and click that purple line and it mirrors it across. Now we'll click okay and we're good to go. We have two triangles but let's go ahead and delete the lines we no longer need.
From that center circle we can delete the line going down. We can delete this 10 millimeter line. It was just there to find that corner.
We'll click and delete that. We don't need the purple line anymore. We'll select it and delete it and it's gone and that looks pretty good.
We have triangle, triangle and that center hub. Once it looks good we can click finish sketch. Let's go ahead and give that sketch a name.
Right now it has a generic name and we'll type in fork details. Enter locks that in. So let's go ahead and go to the create menu and look for extrude and we want to select our profiles first.
So select. We will select one of our triangles then the other triangle and then that circle can be hard to select. Sometimes holding control on the keyboard lets us select through items.
We can click on it or we might have to hide our fork body but control is working for now. We'll hold control and we have our three selected profiles. Now we want to change our direction from one side to symmetric.
I'm going to orbit my view to see what's going on a little easier. Starting in the center, pulling that out and eventually it starts to cut. We've got our center circle, the two triangles and it's cutting.
What is our distance? We just need to make sure we go far enough to cut everything. So let's go to 50 and objects to cut. We can uncheck everything except for our fork.
We don't want to cut any part of the wheel, just the fork and click ok. And there we go. That's looking pretty good.
Now we've got our sketch here. It's called sketch three. That's because it didn't take.
Sometimes you have to do it again. So fork details. Enter locks that out.
Hopefully it stays there now and we don't need to see the fork angle sketch anymore. We can hide that and we also no longer need to see the fork top. We'll hide that.
Just keep everything nice and clean. So there is our fork and last but not least we can add some fillets to make it look good here. So under modify we'll go to fillet and we'll click on these little edges at the bottom of our fork.
One, two, three, four. We might have to orbit around so we can see every edge and select all four. Once we have that we can visually drag the arrow in and or we can type in our dimension which in this case will be 10.
So 10 for 10 millimeters and then in our fillet menu once we have the 10 typed in we will click ok. And that's about it. That's our fork.
It's looking really good. I think we're all set with that. Now we can go ahead and create our pattern right from that.
So in the create menu we can select create flat pattern and we need to pick our stationary face. If we look up inside here at this face we can click the inside flat face right at the top of our fork. We'll click that and click ok.
Fusion is going to think for a moment and create that flat shape for us. Once we're happy with it which there's really nothing to do it looks good we can click the green check box and there it is. We're done.
Let's just double check everything here in our browser. We have our fork. We have our rules which is all for steel.
We have our flat pattern which we just created. We've got our bodies which is our fork, our sketches, three sketches, and our construction. If that all looks good we can minimize everything and mash that save button.
