Fusion 360 Snap Fit Cases | 3D-Printable Raspberry Pi Case

by the end of this tutorial you'll know how to create snap fit cases in fusion 360 we'll take a look at modeling the snap fit connections for a 3d printable Raspberry Pi case however these snap fit connections could be used in several projects be sure to stick around until the very end of this video where I'll show you a pro trick to make sure your plastic cases stay aligned while you snap them together to help model the case I'm going to use this pre-built CAD model of the Raspberry Pi that I found on grab CAD this is the fourth version of the Raspberry Pi so if you're modeling a case for a different version or for an Arduino then you'll want to make sure you modify it accordingly I'll put a link to the grabb CAD download on this tutorials resource page along with some other resources that can be found at product design online.com forward slash number 13 that's product design online.com forward slash 1-3 the grab Cadfael that i found is a step file and you'll see after importing the file there are several different components and parts that make up this file to simplify the design file for the 3d printable case I'm going to create a new file and then insert the imported file I'll simply click the new design plus symbol above the toolbar then before we can insert the design file we'll have to save the file as this is required otherwise you'll be prompted that you can't insert into the current design I'll simply click the Save button and then I'll type out Raspberry Pi number 4 and then case then I'll hit that blue Save button to save the file if I now toggle open the data panel you'll see that I'm able to right-click on the imported step file and I can select insert into current design this will then give us the option to rotate or alter the scale of the object I want this case to be sitting right side up so I'm going to drag the rotation slider until it snaps into place at 90 degrees then I'll click the ok' button to confirm the rotation change you'll now see that we have this linked sub assembly folder with all of the original components nested underneath now you could have simply created a new component and nested the Raspberry Pi files underneath however I like to keep design files separated as much as possible by using these linked instances this way if I use the file in other projects I only have to worry about updating the one master file I'll now create a new component for the plastic case and then we'll get started with modeling the case I'll select the assemble drop-down list and then I'll select new component I'll simply rename this plastic case before clicking the OK button before starting the main box shape we'll want to make sure the existing model is in the correct place looking at the front view of the model you'll see that the bottom of the Raspberry Pi model is slightly below our bottom origin plane we'll want to move this up leaving enough room for the thickness of our case I'm going to right-click on the Raspberry Pi component in the fusion 360 browser then I'll select the move slash copy option or you can always hit the keyboard shortcut letter M as in Mike if I type out two-and-a-half millimeters you'll see that puts the bottom flush with the origin plane however we want this to be moved in additional three to five millimeters factoring in the thickness of our box I'm going to make my case enclosure three and a half millimeters thick so I'll type out a total of six millimeters then I'll click the ok' button to confirm the results I'll now hit the keyboard shortcut letter R as in Romeo to activate the rectangle command before doing anything you'll see that I'm prompted with a question of whether I want to capture the current position of the model because I recently changed the position of the model which I would like to keep I'll select the capture position button should you ever accidentally move a component around you can hit the continue button which will place the component back in its original position now that the rectangle tool is activated we'll need to select an origin plane to start the sketch on I'm going to toggle open the origin folder and I'll select the bottom XY origin plane then before clicking anything I'll be sure to select the center rectangle and the sketch palette this will allow us to start the rectangle by clicking on the center origin point or the height I'll type out 64 millimeters followed by the tab key to lock the dimension in place then for the length I'll type out 93 millimeters then I'll hit the enter key on my keyboard to place the rectangle I'm now going to extrude this rectangle into a three dimensional box well then want to shell the box create the holes on the box and then we'll cut it in half followed by creating the snap fit joints I'll hit the keyboard shortcut letter e as an echo to activate the extrude command then I'll type out 30 millimeters for the height followed by clicking the OK button as we work with our plastic case we want to be aware of our inner parts therefore I'm going to lower the opacity of this case component I'll simply right click on the plastic case component and then I'll select the opacity flyout folder you'll then be able to select be 60% setting which allows us to work with the model while still being able to see the inside before shelling this box I'm going to apply fill it's to the outside so it has nice rounded edges I'll hit the keyboard shortcut letter F is in Foxtrot to activate the Phillip command I'll select the four vertical edges and I'll type out a fill it radius of five millimeters and I can look at this model from the top view to ensure that I'm not going too far in it looks good for now so I'm going to hit the plus symbol in the fill it dialogue box this will let us create some more fill it's on the remaining edges before selecting anything I'm going to look at the model from the home position then I'm going to click on the select drop down menu so I can select the selection priority flyout folder where I'll click on the option that says select edge priority this will let me select the top four in the bottom four edges without worrying about selecting any of the faces by accident I'm going to then type out a fill it radius of two and a half millimeters followed by clicking the OK button at this point we can hollow out this solid cube by using the shell command I'll activate the shell command from the modified drop-down list to ensure we shell only the inside without removing one of the faces we'll need to select the body of the plastic case if you're having trouble selecting just the body then you can always select it in the fusion 360 browser which will ensure there is no possibility of selecting the face after the body is selected I'll type out a shell thickness of three and a half millimeters which will represent the thickness of the walls of our case I'll make sure the direction is set to inside and then I'll click the ok' button looking at the model in its current state we can somewhat tell that a Raspberry Pi has enough room around it however we can always use the section analysis to take a better look I'll select the inspect drop-down list then I'll activate the section analysis I'll then select BYZ plane for the faces selection this will let us essentially cut the model in half to take a closer look at it it appears that everything fits within this plastic case from this perspective as the components on the ends here will end up having slots cut out for them I'm going to also check the section analysis in the other direction I'll turn off this first one by selecting its corresponding light bulb in the fusion 360 browser then I'll right-click and select repeat section analysis this time I'll select BYZ origin plane before clicking ok if I now look at the right side of the viewcube you'll see that this side of the model appears to be okay as well we see some other components that will need to create holes for lastly we may want to create a third section analysis for the top view we can then use all three of these as we continue to work on the model giving us the ability to quickly monitor our inside components I'm going to first turn off this section analysis then I'll rename it by selecting it in the fusion 360 browser and I'll click a second time which lets us rename it I'll name this one with and I'll quickly rename the first one length I'm going to hit the keyboard shortcut letter s for the shortcuts box and I'll type section which gives us the section analysis option at the top I'll simply click the enter key on my keyboard to select it then I'm going to select the top of the model and I'll just drag the blue single directional arrow down about five or six millimeters now the height doesn't matter as long as I can see into the inside of the case lastly I'll be sure to click the ok' button to confirm this section analysis i'll also rename this one top in the fusion 360 browser now that we can see through the top let's create some pegs that will run through the holes on the raspberry pi's board this will help keep the board in place as it sits in the case preventing it from moving around we're going to reference the circle cut outs on the imported model to do this we'll use the project command which will let us project the geometry into a two dimensional sketch I'll select the sketch drop-down list and then I'll find the project slash include folder near the bottom of the list then I'll select the top face of the bottom side of our plastic case you'll notice the body of my plastic case component is highlighting in the browser which confirms that I'm selecting the correct face now that I have the project command activated and I've chosen a sketch plane I can select the four inner circles followed by clicking the OK button you'll now see that we have purple sketch geometry which signifies that it's driven by something or in our case this original Raspberry Pi model we can now select the offset command from the sketch drop down list this time I'll select one of the projected circles then I'll type out an offset distance of negative zero point three millimeters which equals a tolerance of 0.6 millimeters since we're dealing with the diameter of a circle you'll want to make sure that you use the negative symbol in front of the value or you can use the flip button to ensure that the circle is on the inside then we'll click OK to confirm the results unfortunately fusion 360 won't always let us offset multiple projections at once so I'm going to right click to do the repeat offset command and I'll repeat these steps to do the same offset for the other three circles you now that I'm done with the offsets I'll hit the extrude icon in the toolbar I'll select all four circles then I'll extrude these up a distance of five millimeters and I'll click the ok' button now that we have the pins in place we'll take a look at making the cutouts for all of the power connectors hdmi and other slots on the Raspberry Pi but first if you're enjoying this tutorial so far then go ahead and click that like button and be honest if you're not enjoying it then click that dislike button if you want to see more 3d printing related tutorials then comment the word print in all caps down below we could create a sketch on the right side of the model however I'm going to create an offset plane so it's a new sketch that's not directly tied to this face of the model in case I changed the overall shape later down the road I'll simply select the offset plane in the toolbar and then I'll select the right face after the value is set to zero millimeters I'll click OK we can now toggle open the construction folder in the browser which will let us right click and select create sketch to create the cutout for the Ethernet port in these USB ports will want to project some reference geometry which will help us ensure our cutout is large enough to help us better project the reference geometry we can turn on our width section analysis you'll see that after I click the light bulb that it cuts it in half as we initially set it up to the Y Z plane to make this more useful I'll right-click on it in the browser and I'll select edit I'm simply going to drag the blue single directional arrow towards the right side until I can see the three connectors being sliced in half or about 32 millimeters then I'll click okay I'll now hit the keyboard shortcut letter P as in Papa to activate the project command I'm also going to make sure to look at the model from an angle so I can see what I'm selecting watch as I select the first connector you'll notice it projects a square to the active sketch plane I'll go ahead and click on the next two before clicking the ok' button in the project dialog box now that we have the shape of the connectors we'll need to offset the geometry to factor in some room for a small tolerance I'll hit the keyboard shortcut letter o as an Oscar and I'll offset the first square a distance of one millimeter to the outside before clicking the OK button then I'll have to right click to select repeat offset and I'll repeat the last two steps for these remaining two squares making sure that they're both offset one millimeter away from the projected geometry we can now hit the extrude feature in the toolbar then we'll need to select all of the profiles to extrude so we can cut them away from the outer case after the profiles are selected I'm going to switch to the top section analysis then I'll rotate the model around so I can click on the inner wall but first I'll make sure the operation is set to cut I'll also make sure the extent type is set to to object and I'll select the interface of the plastic case lastly we'll want to make sure to toggle open the objects to cut option you'll notice that because our raspberry pi is contained within its own component or sub assembly we don't have to worry about accidentally cutting into it throughout your time modeling this case you may find it helpful to activate the top level component to take a look at the model without the Raspberry Pi component being ghosted just remember to reactivate the case component before continuing to work on it to create the slot on the other side for the USBC and micro hdmi ports we could follow the same process by projecting their geometry an alternative would be to create one slot that covers all four ports on the side I'll quickly walk you through this process so you're aware of a different approach I'm going to select the sketch drop down list and I'll find the slot flyout folder the slot commands let us quickly create rounded rectangles or slot cutouts I'm going to select the overall slot then we'll need to click on the front face of the case component the overall slot command requires us to define the start and end point of the slot and then we can define the overall width I'll click around the midpoint of the audio jack making sure to click on the right side of it then for the second point I'll click just past the USBC port as I now drag my mouse cursor out you'll see that we can define the width by typing out a value I'll type out six and a half millimeters and then I'll click to place the slot once again we'll extrude cut this by selecting the extrude command I'll select the slot profile and then I'll turn the top section analysis on again this will let me set the extent type as to object then if I click the inside wall you'll see that fusion is smart enough to switch this to a cut operation we can then click the ok button to confirm the results as you'll see this option is not quite as clean looking as cutting out a hole for each individual component however this method is a lot simpler and requires less work lastly we'll need to cut out a slot for the micro SD card that is on the bottom of the board if I look at the left side of the model you'll see the card slot is at the bottom Center to cut out this hole I'm simply going to cut out a rectangle that runs up to the bottom edge of the case I'll select the center rectangle from the sketch drop-down list then I'm going to click on the left face of the case I'll select the center origin point and I'll drag out with my mouse I'll make this rectangle 12 millimeters in height and 16 millimeters in width I'll activate the extrude command and then I'll select the rectangle profile you because your fingers will run along this lip while you insert the microSD card you'll want to round over these edges I'll activate the model Philip command and then I'll add a Filat of two millimeters to the surrounding edges now that we have all the cutouts complete I'm going to turn on the full opacity and turn off all the section analysis options at this point we can finish off the case by slicing it into two parts and then we'll create some snap fit joints to split the case in half we'll use the split body command first we'll need to create a construction plane that we can reference as the splitting tool to set up the construction plane will use the midplane option which will ensure that our plane always stays in the middle of the case after selecting the mid plane option from the construct drop-down list will be prompted to select the planes I'll select the top face and the bottom face which places the midplane directly in the middle then I'll click the ok button we can now activate the split body tool in the modified drop-down list we'll need to select the case body as the body to split then we'll need to select the splitting tool selector and select the construction plane as the splitting tool you'll also want to make sure the extend splitting tools option is selected as that will make sure that the case is completely split even if we update its size after clicking ok you'll see that we have two new bodies I'll go ahead and rename these top and bottom in the browser so I'm aware of what bodies I'm working with later on we can also click the light bulb for the midplane construction plane to hide it now that we're done using it if I hide the top body you'll see that we now have successfully split our case into two parts so one can 3d print each part with the flat side on the build plate let's go ahead and finish off this model by adding the snaps the first thing we want to consider while adding snaps is where the snaps will go looking at the model you'll see we'll need to be aware of the internal components of the Raspberry Pi when possible I always like to make the snaps directly across from one another as that typically provides for a better experience getting them to snap together given those requirements it looks like we can squeeze the snap into the area between these connectors and then we can put one on the opposite side there are many types of snap fit joints but for this particular tutorial I'm going to show you how to create a cantilever style joint in general snap fits will encounter the most amount of stress during the attachment to reduce the amount of stress we want to design this so the joint returns to its neutral position once the joining process is completed then once the parts are together in undercut we'll hold them together let's start by cutting out an undercut on the sidewall of the case I'm going to activate the mind tool and I'll click on the front face to create a new sketch then I'm going to turn on the construction option and I'll create a construction line running four millimeters down from the top I'm also going to use the dimension tool to add a dimension from the endpoint of the line to the edge of the inner component making sure our whole on the opposite side doesn't conflict with that then I'll be sure to turn off the construction option next I'll activate the center rectangle command and I'll start the rectangle at the endpoint of the construction line I'm going to make this rectangle six millimeters wide by three millimeters tall then we'll extrude cut this rectangle out of the box once again making sure that it's extent type is set to the inside wall of this case we're going to Mir this to the other side once we get the cantilever portion completed I'll now turn the top body back on by selecting it in the browser then I'm going to turn the with section analysis back on I'm going to right-click to edit the section analysis and I'll drag it over until it's lined up with our cutout so we can see what we're doing I'll now create an offset construction plane of this inside wall of the cutout to make this zero point five millimeters factoring in a small tolerance well then need a right-click on the construction plane in the browser to select create sketch I'm also going to hide the Raspberry Pi component so it's out of the way then I'll hit the keyboard shortcut letter P as in Papa to activate the project command I'm going to select the top bottom and cross lines so we can reference these projected lines which will let us snap to it with the other sketch geometry I'll now be able to activate the line command in the toolbar and because of these projected edge lines we can easily start the sketch off the corner I'm going to make a line going up with a distance of 8 millimeters then I'll go to the right two millimeters next I'll go down ten millimeters I'll go to the left six millimeters I'll go back up two millimeters where it snaps in with the line and then I'll connect this line over to the original starting point well now want to extrude this profile and then we'll finalize it by adding some fill 'its and chamfers I'll hit the extrude button in the toolbar and then I'll select the profiles that make up the shape and I'll type out five millimeters for the thickness I'm also going to make sure the operation is set to join and I'll hide the bottom body so it only joins to the top body then I'll click okay at this point we'll want to add some champers to the snap I'll start by selecting the chamfer tool from the modify drop-down list then I'll select the bottom front edge I'm going to make this chamfer two millimeters and I'll click OK then I'll right-click and select repeat chamfer this time I'll add a chamfer of one millimeter to the top front edge and then I'll click OK finally I'll add a third chamfer to the inner side where the stem is attached the top case body this will allow the top portion of the case to 3d print better with an angle instead of an undercut I'll make this one two millimeters or the thickness of this stem and then I'll click OK lastly I want to add a fill it to the inner edge of this snap this will strengthen it a bit more and make sure it slides along the undercut I'll activate the Philip command from the modify drop-down list and then I'll make this a Filat of 0.5 millimeters we can now turn the bottom body back on so we can add the same fill it radius to the inner edge of the cutout I'll reactivate the Filip command and I'll select the inner edge to create a fill it radius of 0.5 millimeters looking at this snap-on screen it appears that this snap cantilever is pretty large however if I inspect it you'll see that it appears to be much larger on screen as its true size is only about two and a half to three millimeters I've also found that nylon 3d printer filament works best when creating objects with snapple parts I've put a link to my favorite nylon filament on the resource page for this tutorial I should also note that this particular snap design is intended to hold two parts together for a long period of time and it's not the best snap fit if you're looking for something to take apart daily let's now go ahead and mirror these features to the other side so we can have a snap on each side of the box I'll activate the MIR command from the create drop-down list then I'll set the pattern type to the features option this will let us first mirror the extrude cut out that we created earlier I'm going to separate this mirror from the rest of the features as it's likely that fusion 360 would have trouble computing all of them at once I'll select the XZ plane as the mirror plane and then I'll click OK after the cutout is mirrored we'll need a mere the rest of the features I'm going to hold down the command key on my keyboard use the ctrl key if you're on Windows and then I'll select the last extrude the three chamfer icons and then the first phillyd icon to be used as the mir results we then have to select our mir plane once again I'll select the XZ origin plane and then I'll click OK instead of mirroring the Filat of the inner wall we can just edit the last Filat feature and select the other edge first we'll need to drag the fill it to the last spot in the timeline so it appears after the mere results then we'll need a double click to edit the fill it I'll select the plus symbol and then I'll add a fill it of 0.5 millimeters to this other edge we can now switch our section analysis to the top view I'll also turn the PI component back on and you'll see that we now have these nice snap fit features in addition to all of our cutouts the last tip that I want to share with you in this tutorial is how to create a nice edge that will help you align the top and bottom pieces as you're trying to snap them together I'll turn off the section analysis and then I'll hide the top body and the PI component I'm going to then hit the keyboard shortcut letter o as an Oscar to activate the offset command I'll then select the top face I'll select the outer edge and I'll type out negative 1.25 we're going to extrude this profile up just two millimeters so we can create a ridge that will cut away from the other body I'm also going to add a fill it radius of 0.5 millimeters to both edges which gives it a nice round over at this point we'll need to subtract this new addition from the top body I'm going to turn the top body back on then I'll select the combined body tool from the modified drop-down list I'll select the top body as the target body and I'll select the bottom body as the splitting tool I'll set the operation to cut and then the most important part here is to make sure that you check the keep tools option as we want to keep this bottom body after it's used to cut the cavity out of the top let's click OK to see what happens if we hide the bottom body and look at the top one you'll see that we have now cut out the negative part of the groove ultimately this subtle feature we just added will make a huge difference in helping each half of the case line up when we're trying to snap them together to summarize in about a half hour or so we were able to create this fairly complex Raspberry Pi or Arduino case that snaps together you may also want to consider customizing the case by adding your name logo or project name to the top of the lid you can also further develop the design by adding more snaps for durability vent holes ribs or other features to enhance the plastic casing if you made it to the end of this video then let me and the community know by commenting below if you have ever used an Arduino or Raspberry Pi for a project as always I truly appreciate you taking the time to watch this tutorial click that thumbs up icon if you want more free content and click on that playlist in the lower right hand corner to watch more 3d printing in fusion 360 tutorials to be part of the product design online community be sure to subscribe and check us out on patreon by clicking that patreon logo right now

Channel: Product Design Online

Views: 292,125

Keywords: fusion 360, autodesk fusion 360, snap fit joints fusion 360, snap fit joints 3d printing, adafruit snap fit joints fusion 360, fusion 360 snap fit, fusion 360 snap fit case, fusion 360 snap together parts, fusion 360 raspberry pi case, fusion 360 raspberry pi, fusion 360 raspberry pi 4, fusion 360 raspberry pi case tutorial, fusion 360 raspberry pi model, 3d printing, 3d print, product design online, 3d printing nerd, 3d printing for beginners, makers muse

Id: E0NVC8xhf3I

Length: 35min 15sec (2115 seconds)

Published: Fri Aug 16 2019