3D Printed Fittings for Silicone Tubing (Fusion 360)

I have a small hydroponic garden and recently changed some tubing to a different, more durable silicone tubing. My old fittings are now too small for the new tubing, so its time to design some new fittings for some tubes!

The goal of this Instructable is to hopefully pass on some knowledge on how I make 3D printable screws and barb fittings. All using Fusion 360 modeling software and Cura 4.13.1 for slicing .stl files.

We will be using ABS filament on a Lulzbot Taz5 printer with a .4mm nozzle. These instructions can be used with other printers and filaments however, a nozzle size no bigger than 0.5mm is recommended for the 3d printer since print layers will be 0.15mm and any bigger nozzle will struggle to print effectively for the detail we need.

Fusion 360

Cura (or similar slicer of preference)

ABS (or preferred filament)

3d Printer

Enthusiasm for creating!

So, as all projects begin, this one too starts with figuring out the specs of our materials. We need to know the inner diameter (ID) and the outer diameter (OD) of our tubing so we can build around those dimensions.

Mine happen to be 6mm ID and 8mm OD.

Continue!

Launch Fusion 360 and start the project by creating a new cylinder. Set the width of the cylinder to the OD - 1mm of your tube, so if your OD of your tube is 8mm set the diameter of the cylinder to 7mm. And set a length of 10mm.

You should have something that looks like this.

Now you have a basic cylinder, the goal is to make it into a surface that the silicone tube wants to grab onto and ideally become water tight when it does. A proven method for this fitting is known as "barbs".

Start by creating another cylinder right at the bottom, center (center of origin) of the one we created in Step 1. This time make the diameter 2mm wider and make the extrusion height ~1/3rd of your cylinder.

I made mine 9mm diameter and 3mm height.

Make sure that in the pop up menu on the right, you select "new body", BE CAREFUL not to select CUT or JOIN !! (This will prevent us from moving onto the next step.)

Next, we will click on the top surface of the cylinder we just created to select it, and once selected press "e" to extrude the surface.

Once we have started the extrusion, do the same we did with the first cylinder and make sure to choose the "new body" option. Set the height to the same as the one before and go on to the next one.

Now do the same process you did with the second small cylinder for the third one. You should have 3 separate bodies of the same cylinder stacked on top of each other. Like the images.

Finally for this step, we Chamfer the edges to give it the actual barb shape. Select the top edge of the top stacked cylinder by clicking on it. While selected, choose the command chamfer under the modify tab. And under "Type" select "Two distance". This will allow you to set a height and depth to the chamfer. The height will be our small cylinder heights and the depth should be 1mm in my case, but play around with these values to see what they do.

Now click OK and move on to the next body, the cylinder below. To select the top edge of this cylinder you may want to hide the one we just modified. From the component list on the left, click the eye icon to hide the cylinder we just chamfered.

Now you can easily select the edge and repeat the same chamfer process with the same values you used for height and depth.

Once you've done it for all three of the cylinders, unhide them from the component list. Select them all and click combine from the modify menu.

Done with the Barb!!

Since we are done with the barbs, we can now replicate that process for all of our fittings for the silicone tube, simple as that! But!! How do we make a screw (male) fitting for the barb you ask?! Follow along.

Now, hide the barb body from the components list by clicking the eye icon.

Next, we need a cylinder to use as the "male" part of our fitting. Simply make a new cylinder at the center of the XY plane, a diameter of 16mm is ideal. with a height of your preference, but I set the height to 18mm.

Put some threading on it by selecting the "thread" option under the "create" menu. Click the outside surface of the cylinder and click thread, or vice versa.

Now, in the thread menu on the right, make sure to check "modeled" to actually make the threading modeled on the cylinder. Also, uncheck full length and set the lengths on there so our threading starts 3mm from the top.(We will put a hex on the top to make it easier for screwing with a wrench.) Careful with the thread size.

IMPORTANT NOTE: When building threads to be 3d printed, make sure that the thread size is 1.5 or bigger because smaller threading may not print on most FDM printers due to layer height, tolerances, etc.

Next, we will offset the thread to give it some tolerance so it will fit into our 3d printed nut. For this we will select the thread's surface, and click "q" to initiate the offset command. We will offset it about (-0.15)mm this seems to work for my 3d printer but play with this value to find what works best for your printer. Do the same on the other face of the thread too.

Next, select the edge of the thread and do a 0.2mm fillet (select "fillet" from the modify menu) to make sure while the part is being printed, the sharp edges won't lead to unnecessary supports and cause your print to fail.

OK, now we have a barb and a screw looking thing. All we need is to combine them together, poke a hole through them and say goodbye to send off to the slicer, but first! We need a bolt (hex or whatever :/ ) to use while tightening the fitting to a hose or tank or anything else.

Select the upper surface of the screw we just made and click "create sketch". In this cool sketchy domain, we will sketch out the hex that we will then extrude. Firstly, click "create">"polygon">"circumscribed polygon" and then place it in the center of the top surface of the screw cylinder we have. Set the radius as the same as the cylinder underneath it and...phew. OK. Now select "Finish Sketch" and quit the sketching domain. You will see a blue polygon on your cylinder screw thing, click the inside of the polygon to select all the pieces(click and hold shift) and then hit "e" as you did before, to extrude. This time we will extrude down 3mm (remember from the previous step, we started the threading 3mm from the top). It should look something like in the images. Make sure to select "Join" here and not "cut" or "new body" from the extrude pop up on the right.

Now, all we have to do is hide the screw/hex/cylinder thing from bodies and unhide the barb body. Next, select the barb body and click "m" to move it. At this point, if you've built everything at origin center, you will only have to change the z value of the barb by the height of your cylinder/hex/screw thing.

If you've gone cowboy and have built the two things in different XY coordinates, no need to worry. Just select the barb body, hit "m" on your keyboard, choose move "point-to-point" in the move pop up menu on the right and click the center of the bottom face of the barb and the center of the top face of the hex/screw/cylinder thing. Voila! They should be centered and sitting on top of each other.

Now we can select both bodies and click "combine" from the modify menu.

We have a single piece thing that looks like this. We need to make a hole in it so water can pass through. Using the "hole" command under the create menu, select the top surface of the barb and make a hole in the center. The width of the hole should be so that there is about 2mm thickness to the lip of your barb and under the shape settings of the pop-up choose "extends">"all". This will hold up fine with ABS and other materials like PETG but anything more brittle might need a bit more thickness to it.

Finally fillet the edges of the barb to make it structurally sound, this should be pretty straight forward at this point. If not follow the images. I used a 0.5mm fillet, you can start here and try more or less fillet size depending on your preference. Make sure to not fillet too much though, otherwise the barb size will be smaller and smaller which might lead to your tubing slipping off the barb.

We have a finished male barb with a threaded male attachment. Now all we have to do is select this and save as an stl so we can send it to the slicer.

Right click on the body under the components list and choose "save as mesh". Make sure file type is .stl and we are set! Click save to file and open up your slicer to slice away.

Open up your slicer and slice away! Make sure layer height is set to 0.15mm or even 0.1mm if possible. And play around with the settings if you like.

This is it! If there are any questions or areas that you may think needs clarification or clearer instructions in this intractable feel free to email or comment and I will happily update the steps.