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3D Printed Molds Part 2 – Fusion 360 Mold Design

3D Printed Molds Part 2 - Fusion 360 Mold Design 1


Hey guys! In part two of my mold making series we're going to get down and dirty in Fusion 360 to show you exactly how to create these molds and then print them out. This process normally takes me five to ten minutes. There’s time stamps in the description and you'll see them in the bar below the video. You can skip ahead to any portion you want to see. If I leave anything out if you have any questions about anything in particular, please leave me a comment and I will answer them in the next video where we're actually going to inject this mold and go test it out. Alright guys let's roll!

making the mold box using Fusion 360

Making the Box

So we have our lure here. We're going to go and create a sketch on this plane and I’m just going to create a two-point rectangle and the size at this point doesn't really matter because we can adjust it later. You want to be thinking about where you're going to make your sprue hole to inject your plastic through and give yourself enough space there. So this one I’m going to inject right here at the head of the lure so I want to make sure I have enough space in front to put my sprue hole in place. Then I want enough space on the sides. Again, it's not terribly critical where we are at this point, we can always adjust it later. I'm going to take my rectangular square tool and draw a box. The sides matter because we need to put in some bolts, or some poles for our bolts, and we want to make sure that we have enough room for them.

So I do the box then I hit escape and now I’m adjusting the box out. What I do from here is I’m going to extrude this sketch object into a box. I come up here, and hit extrude my box. The key point here is my direction, I want to be symmetrical which is going to move it the same distance up and down. The sweet spot I‘ve found no matter what size lure you have is 15 millimeters, so I get 30 millimeters in total height. If I do 15, it's going to go 15 up and 15 down giving me 30 total. I found with 30 millimeters total, you have enough around the edge of the sprue to hold it in place.

Now if you know Fusion 360 at all, you can see its turning red which means it wants you to cut. I don't want to cut, I want to change my operation to new body. That's going to create a new box for me. Having a 17 millimeters body and symmetrical are the main keys there so I click on ok. Now, if I come over here and look at my bodies drop down, my twirl ball is here and I have this body too. The first thing I like to do usually is change the opacity or the transparency of this mold so I can see what's going on. Right click opacity control and I’m going to choose 50 so you can see we have our lure in the middle.

rename, opacity and chamfer on Fusion 360

Rename, Opacity and Chamfer

The first things we're going to do here is prep the mold box before we actually make our Split. I’m going to go around and select these edges and I’m holding down the shift key as I’m selecting multiple edges. What I’m going to do is I’m going to add a chamfer, which is basically an angle to all of these edges. The reason I do that is it uses less resin and it makes it easier to get off the build plate when I print it. I’m going to print one of these edges flat to the build plate so I just go ahead and chamfer around everywhere to save a little resin. Now chamfer is different from Philip in that chamfer does a direct angle. I do two millimeters, which seems to work for me on smaller molds. You can figure out what works best for you. Now you can see I have these angles around there so again, I do this mostly for saving a little bit of resin and it'll be easier when I print to get under here and pop this mold off.

cutting the lure out of the mold in Fusion 360

Cutting the Lure out of the Mold

Now that I have my box and my chamfers, what I want to do is cut my lure out of the box which is pretty simple to do. We're going to use this tool in the modify area and we're going to hit the combine tool and it gives me two options, target body and tool bodies. I'm going to select my mold and I’m going to select my actual lure so I have target body and lure body. My operation is going to be a cut and I want to check this box keep tools that's going to keep my master mold around and I just click okay. Now you can see it doesn't look like anything actually happened but if I come over here and basically turn off my master in the view, you can now see I have my hole in here. Now I have a mold at this point but I have no way to get any plastic in there, so let's fix that problem.

making the sprue in Fusion 360

Making the Sprue

We're going to add a hole to the front, this is going to be your screw hole where you inject plastic. I click on the hole tool and then I’m going to click on this front face here, make sure you click on the actual face. We want to line it up roughly in the center, make sure you're looking straight on so you're not getting weird angles. It should snap into place and then there’s two way you can do this. One, you can make the diameter you want the front where your injector is going to go which is roughly 16.2 millimeters. That's what I’ve been using and it's working really well so that's going to make this whole area here 16.2 millimeters and then my drill point I set to an angle and that way I can control how much penetration I get into my cavity. So if you look at the front here, that's going to shoot straight down there and I have a little opening and I have a little bit of an edge here.

So you can do it that way or the second way you can do it is you can set a counter bore and set that width to 16.2 and I can sit my main width to maybe 10 and you can see how it changes. Now my counter bore is where my injector is going to go and then this 10 millimeter gives me a slightly smaller sprue that I can pump all the way through there if I want to. It's really up to you, I haven't found that much of a difference and I tend to use just the straight through 16.2 on these smaller molds. I’ll use the counter bore and the smaller midsection there on multi-cavity molds, but on these little guys I like to keep it relatively simple. The main control here is this, I just pull it back and forth until we are into the cavity. I’m into the cavity but I’m not blowing up the face, if I go too far back I’ll blow up the face and I just eyeball it. Then as always, we want to click this edge here and we're going to add a fillet and let's make this fillet 1.5 millimeters. That's just going to add a little edge here and make it a little bit easier to pump it in there.

aligning bolts and holes on a mold in Fusion 360

Alignment/Bolt Holes

So now I have my sprue hole and my cavity so I can actually get plastisol into my mold. The next step I usually like to do now put in my holes for my bolts. What I’ve been using is M5 bolts. With M5 rivet nuts and the bolts you can do two things, you can use the bolts plus the rivet nuts to actually hold it together or you can use just the bolts without the nuts for alignment. Usually, I do a combination of the two. So I’ll put some bolts in with the rivet nuts to hold half of the mold in place and then I will put the bottom half with just the bolts into a vise. Now is when you need to decide where you're going to split and again we chose a round lure here so it doesn't really matter which direction. I’m going to split this one from top to bottom along the red plane. I’m going to use this plane right here to do my split so I’ll have a top and a bottom.

So what we want to do is then make sure our bolts go through that area. So I’m going to come over here and looking at the top now, I’m going to create a sketch. I’m going to create it on the top part of my mold so I click there and now what I want to do is create some circles and these circles are going to be five millimeters in diameter. M5 bolt is a 5 millimeter bolt, it doesn’t really matter at this point since you can do whatever size you want. By matching it to your bolt size you can get an idea of whether you have enough space or not, so five millimeter if you were using quarter 20s you'd want to do quarter inch.

Now I want to create a rectangular pattern and I’m going to select my circle. We’re going to go over here now I only need two of these so I change this number to two and then I push it down here and let's do five. The more holes we have here the more we'll save resin but obviously you don't want too many that would impact a lot of different stuff on your mold. Now hit enter and this is where all my holes are going to go and then we're going to finish sketch. We're going to use a different mode so I’m going to click hole I’m going to select that face that I just drew all those circles on and it's going to put a hole there but I want to come over to my hole tool and click sketch multiple holes. It's going to ask me to select the sketch points so I just come in here and click on all of these sketch points.

Now remember, I said I was using M5 bolts so there's a cool feature here in Fusion 360 that I can actually size these holes to the size of the bolt I’m using. The first thing I want to do is create a hole type.
I want a countersink because I have countersink bolts hole type. As soon as I hit clearance, this other area opens up down here and I have ANSI metric in profile which is metric and I have flathead machine screws which I bought. The size I select is M5 fit. I can do normal, I can do close, I can do loose normal. Loose normal usually works for me if you want to get picky you can go close. What you want to make sure you’re getting is enough depth so if I go to the right hand side I just want to pull these all the way through. Click ok.

venting the back of a mold in Fusion 360

Venting the Back

Now we have our holes we have our sprue and now we need to work on one of the vents. So I find the back and I’m going to put an air vent on this tail section. I find the air vent to be easier to do at this point than at the next point where we're going to be adding more air vents. So create a new sketch at the back and I’m going to select this back face. I’m going to draw a circle right in the center and I’m going to make it 0.5 millimeters and that's a size that has worked really well for me, it's always a balance between getting the air out and not letting the plastisol go through. One millimeter is too big you'll get lots of little tails and it doesn't hold the plastic. 0.5 millimeter seems to work best. I click finish sketch and I want to extrude this guy and just run it back in until you can see here. It turns into this circle that's going through that ball there. It doesn't matter which way you go through but you just want to make sure you go through and make sure it's set to cut and then click okay. Now I have a nice vent hole there.

splitting the mold in Fusion 360

Splitting the Mold

Now we're going to get to the fun part. I just clicked home, now we're going to split this in half and that's relatively simple. I just come up here and click split body. Body to split is my mold, my splitting tool this is where I’m going to select this plane in here but as you can see I can't get through there. I come over here and uncheck that eyeball and then come in here and select this plane. Come back in here turn that body back on and click ok. Now I have two parts, mold and mold 1. This is why I named it early on because it saves you a bunch of typing before now. What I do now is I come in here click on that bottom part, I’m just going to label it B for bottom and then when I put a T in there for top. This kind of organization helps me later when I’m coming through and making STL files.

venting the rest of the mold in Fusion 360

Venting the Rest of the Mold

Now we need to finish up the venting and this is a new trick I’ve learned that seems to work pretty well.
Especially when you have a curly or any master with a lot of detail like this, you don't want to come through and make little holes. So what we're going to do is make a small cut out around the edge of the cavity to absorb the air and then vent that cavity. So I’m going to go to the top view and I’m going to turn off my top mold so it doesn't really matter what side you do this. Now I want to create a sketch on this plane right here you can see I have halves now that I put this hole in here so I click that. Now we're going to use our old friend projects include we're just going to do project include and click project we're going to click here all right and say okay.

Now I have all of these lines in here and then I’m going to create an offset, so from the modify menu offset I can click on this line and it defaults to positive. I actually want negative and we're going to do negative 1.5 and that's why you can see my red line here. Now I have this line here and what I want to do now is I don't want to take this whole area down and I just want this area in here in order for Fusion 360 to work. I need to block that off so I come in here create a line and I’ll come to the back and just click here and come across.

What I’m doing here is I’m creating the borders of my edge and I think it'll make a lot more sense when we go to the next step. So I’m going to click there and go across to their. So now I’m going to hit the escape key so now you can see that I have just this section here. If I mouse over it, it highlights that so that means that's a fully enclosed section which is exactly what I want. I'm going to finish this sketch and I’m going to go do the same thing on the other side. Now you can see I have this little outline section and all we're going to do is extrude these down. So I click extrude and I come in here and I collect click this side and collect this side so I do both at the same time. Now I want to go down so I’m going to type in negative and I think you know -1.5 is probably too much. I'm going to get flashing all around. The typical vent hole is 0.5 and so we're going to stick with that. Now you can see I’ll click ok and that's going to cut this little section here around my mold and that's where my air can go. So again we're going to have hot plastisol shooting down here pushing down, this whole thing is filled with air and it's got to go somewhere so you can go out the back quickly and then it's going to follow into this cavity.

So the next thing we need to do is get this air out of this cavity. This again is the same thing we did last time. I’m going to turn back on my top here and we're going to come over and I’m going to create a sketch and put it on any of these outside areas here. I'm going to draw circles and we can come in now and I put them right on the center line. You can go below if you want to but I think they work just fine here and again 0.5 is my standard. I’m going to create another rectangular pattern and just pull it down and again you're just going to have to play with your mold to see how many of these you actually need. I probably need at least four here if I ended up with one right in the middle of the screw hole, it wouldn't matter too much because again that will vent air just as well as anything else but just line them up to where they're not running against anything you don't want to run them into.

I’m going to click on finish sketch. So now I click extrude and I have to select these profiles. You can see since I did it on the line I have two halves. A trick here is to select the bottom one first then the top one because if I select the top one sometimes the bottom one is hard to click. Select them all and we're just going to drag them all the way across. We click ok. Now again if you want to do more vent holes you can but I think what I have is pretty good but you can have too many. We are all set, all's left to do is export this to STL and print it.

exporting mold to STL and printing

Export to STL and Printing Tips

So to do that you just come over here to each mold part, right click save as STL. This little dialog pops up and I don't change anything in here. High is fine, I think you can get away with medium but I always choose high refinement. Click on ok and then it's going to ask you where you want to save that and you save it to wherever you want to save it and then we slice it and we go from there. Let's go do that real quick.

So this is lychee slicer, the slicer I use. You might use G2 box it's going to be pretty much the same for what we're doing here today. I’m just going to get my STL files that I saved on my desktop and bring them in. I’m selecting both of them and dragging them in here. There's two ways you can really print these molds- sideways or vertically. So I’m just using the rotate onto plate method here so if I print them sideways, this will be the shortest time to print. If I click estimate print time its two hours and 10 minutes but that's an estimate, it's realistically going to take more like four hours. You tend to have more print failures this way than if you rotate them vertically. You can position wherever you want to and you want to make sure you have enough vertical height here. For me, at least, this method produces the best prints but if I estimate print time it's seven, almost eight hours. That's the trade-off you run into.

If this is a prototype, and it's actually going to turn out like I want to I might print them sideways but really I’ve had a lot more failures that way. Again, it's a balance; do you want to try to print it quickly knowing that it might fail or print it this way and know that you're not only going to get the best results but you're going to get the highest success rate. The reason for that is when you print them sideways, you're actually putting a lot of pressure on the edge because there's so much volume when it's pulling away from the fat that it has a tendency to pull and separate from the build plate. There's different ways you can fix that, you can up your exposure time on your base layers but then the problem you run into is it becomes really difficult to get unhooked from the build plate. So this way, again, it takes the longest but it is the most success rate and the highest quality.




If you missed anything there are markers down below. Links to anything I talked about, the printers I use, the resin I use to make these molds, the M5 bolts and the rivet nuts I talked about are all down in the video description.

Have fun guys-tight lines.