Fast Fusion 360 - 3D Print Hinges from a Single Sketch (and Snap Fit Lids!)

[Music] all right let's jump right into hinges a hinge consists of three parts the pin the wing anchors for the pin and the knuckle that revolves around the pin these three parts can be created from one sketch by selecting different offsets and objects to start the extrude from to create our hinge first let's make a box go to create box choose the x y plane and enter a dimension of 50 millimeters for each side next go to create create sketch and select the side face of the box go to create select line and then in the sketch palette choose the construction line type the starting point for our box will be the midpoint of the box draw out the construction line several millimeters away from the box we're going to use this construction line to draw three concentric circles that will make up our pin and our knuckle go to create center dimension circle and then draw three concentric circles on the construction line the size of the circles doesn't matter at this point we will use the dimension tool to size them go to create dimension choose the circumference of the inner circle this will be our pin size it at three millimeters for the gap between the pin and the knuckle select the circumference of the inner circle and the middle circle and enter dimension of 0.2 millimeters finally for the knuckle choose the middle circle and the outside circle and enter a dimension of 3 millimeters select the edge of the box and then click on the middle of the circle and enter a dimension of five millimeters we will need to draw a line between the edge of the box and the outside circumference of the knuckle in order to close the sketch go to create line and draw a small line between the midpoint of the box and the outside of the knuckle sketch a line about 45 degrees from the edge of the box to the tangent point on the knuckle your mouse will also snap to indicate the point of tangency go to create dimension and then select the line drawn for the wing and then select the vertical edge of the box enter 45 degrees go to create line and draw a line from an angle off of the top half of the box to a point of tangency on the outside of the knuckle go to create dimension select the angle line select the vertical line and give it a dimension of 45 degrees next we're going to create a mid plane so that we can split our box into a top half and bottom half go to construct mid plane choose the top of the box rotate your view cube choose the bottom of the box and then hit ok to split our box into two halves choose modify split body select the box and then in the dialog choose select for the splitting tools and then select the mid plane go ahead and open up your browser tree so that you can expose the bodies and the sketches i'm renaming the bodies top and bottom okay now we can start extruding from our sketch to create the pin the wings and the knuckle go to create extrude and then choose the four sketch features the bottom wing the knuckle the pin and the space between the knuckle enter negative 9.5 millimeters make sure the operation is set to join here i'm turning off the top body for visibility click ok if the sketch disappears after the first extrude command go to the browser tree go to sketches and click on the visibility icon to show the sketch again now we're going to create the wing anchor on the other side of the box go to create extrude select the same four profiles the wing the knuckle the pin and the space between them in the extrude dialog go to start click on the drop down and choose object for the object select the opposite face of the cube enter a dimension of negative 9.5 millimeters next for our pin press the keyboard letter e to open the extrude dialog choose the center circle in the sketch for the pin in the extrude dialog menu go to extent type and in the dialog choose to object for the object select the opposite face of the cube the default operation is to cut so it is colored red change the operation in the dialog from cut to join now we're going to create the knuckle for the top half of the box turn off visibility for the bottom and turn on visibility for the top press the keyboard letter e to open the extrude dialog and select the wing and the outside circle when we drag the arrow for the extrude it starts from the profile plane instead in the extrude dialog we're going to go to start offset and we're going to enter an offset of negative 10 millimeters for our distance we'll enter negative 30 millimeters let's turn off our sketch turn on the bottom and now our box with the hinge is complete to inspect our hinge go to inspect section analysis select the side face of the box and drag back and forth to check your pin and knuckle for another perspective add another section analysis for the face adjacent to the knuckle so you may have noticed that our box is not hollow so let's fix that with the shell command in the bottom left of the window is the timeline grab the vertical handle and drag it between the box command and the sketch command go to modify shell and select all six faces of the box enter an inside thickness of three millimeters and hit ok back in the timeline drag the handle back to the end of the timeline turn on section analysis and verify your box is hollow as a bonus let's add some snap fit parts to the box adjust your section analysis as shown and then turn off the top body go to create create sketch and then choose the inside face of the bottom body go to create two point rectangle start your two point rectangle from the top of the body and enter dimensions of two millimeters by six millimeters next we'll use the midpoint constraint to center the sketch on the body choose the top edge of the sketch and then the top edge of the body we will cut from the bottom body and then add a catch to the top body so that they will snap together press the keyboard letter e to open the extrude dialog choose the two point rectangle sketch drag into the body two millimeters and enter a taper angle of negative forty five go to modify and chamfer choose the top edge and enter 0.5 millimeters now we can work on the top part turn on visibility for the top and turn off the bottom in the browser tree also turn on the sketch for the two point rectangle we will use this sketch to create our top part press the keyboard letter e select the two point rectangle extrude out two millimeters verify the operation is set to new body and click ok to create an attachment point we're going to use the draft command go to modify draft for the pull direction select the face towards the center of the box for the faces select the top of our new body grab the rotation handle and drag to 60 degrees now we need to combine these two bodies the top of the box and the snap fit part go to modify combine for the target body choose the top of the box for the tool bodies choose the snap fit part verify the operation is set to join click ok in our browser tree the new body has now been combined with the top body we still need to create the catch point on the top of our box rotate the view cube to get a good view of the snap fit part press the keyboard letter e choose our two point rectangle again enter a distance of 0.2 millimeters verify the operation is set to cut verify the object to cut is the top body and then click ok let's do another extrude press the keyboard letter e select the two point rectangle in the extrude dialog for the start drop down choose object choose the front face of the snap fit part drag it out two millimeters and enter a taper angle of negative forty five let's add a fillet to our catch point to ensure a smooth operation press the keyboard letter f to open the fillet dialog for affiliate enter 0.3 millimeters that's it you're all done use the section analysis tool to verify your parts the 0.2 millimeter cut into the top of our snap fit part will ensure a good fit we can also animate the rotation of the lid go to assemble new component in the new component dialog choose the from bodies check box select the top and bottom bodies in your browser tree two new components are added one for top and one for bottom next go to assemble and joint turn off the bottom body and then carefully select the center of the knuckle turn on the bottom body and then carefully select the center of the pin you may notice the knuckle shift over by 0.5 millimeters which is the gap that we left between the anchor and the knuckle use the arrow handle to drag it back out 0.5 millimeters to restore that gap you can grab the rotation handle to rotate the top lid of the box to print your box go to tools 3d print i'm saving my print to file select the top level component and click ok in cura verify your settings for your printer most of my settings are default for an ender 3 pro i've changed my printing temperature to 212 degrees for the material and 60 degrees for the bed and that works well for my printer i'll save this now to my sd card and start the print do do and there you have it a hinged box thanks for watching have a beautiful day you

Channel: 3D Hobbee

Views: 10,939

Keywords: 3D, 3D Printing, 3D Print, Fusion 360, Fusion360, 3D Model, 3D image, Fusion, CAD, Creality Ender 3, Ender 3, Ender3, Hinge, Hinges, 3D Hinges, Print Hinges, Print Hinge, Printable Hingle, Printing Hinge, Hinge Fusion 360, Snap lid, Snap, Snap fit, Snap fit joints, Snap fit parts, Snap closure, Fusion Assembly, Fusion 360 Assembly, Assembly

Id: KL1aj16ynf4

Length: 14min 19sec (859 seconds)

Published: Sat Apr 03 2021