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This lesson will demonstrate a step-by-step method of designing a flat-pack / friction-fit table for CNC fabrication.

You may want to skip this lesson...

If you're just interested in CAM setup and don't want to learn about flat-pack design, you can skip ahead to the **next lesson. The full table model will be provided.

But if you stay with us, you'll learn a lot...

I've been doing flat-pack / friction fit projects for more than 10 years. I've learned a lot of tricks that I'm about to pass on to you, and if you stick with me I think you'll learn some really useful concepts and techniques that will serve you will with any kind of fabrication, especially CNC.

FLAT PACK / FRICTION FIT

You're going to design a table that's flat-packed and friction-fit. Flat-pack refers to its being made of interlocking flat parts, and friction-fit means it can be assembled so that the friction between the pieces will hold it together without any fasteners.

The example in the lesson has 7 parts in total. Two legs, four stiffeners, and one table top. The stiffeners provide lateral stability to keep the table from twisting or wobbling.


Sketch the Table Top Profile

Most things in Fusion are best made by creating 2D sketches, then turning those sketches into 3D objects. For a round tabletop, that means drawing a 2D circle, then extruding it to give it thickness.

Create Component

A component is an encapsulated part that can have one or more 3D bodies or 2D sketches in it. You want each of the table parts to be its own component because it will allow you to manipulate and manage the whole model more easily.

Go to CREATE > New Component, and give the component a name like "tabletop". Keep the default settings there (Empty Component) and click OK, and you'll see that your new component has shown up in the Browser and that it's activated. While it's activated, anything you make will be within this component.

Create a Sketch

Go to SKETCH > Create Sketch, and click on the bottom plane of the model space. This will bring you into the Sketch environment. The view will change to the Top view.

For this sketch, all you'll need is a circle. Go to SKETCH > Circle > Center Diameter Circle and click on the model origin as your start point.

Type in 42 for the diameter and you'll have a 42" (1066mm) Ø table top. Click the Stop Sketch button on the upper right to leave the sketch environment.


Create 3D Part / Use Parameters

MEASURE YOUR PLYWOOD

Before you design anything, you need to know exactly what the thickness of your plywood is. 3/4" (19mm) plywood is a nominal dimension, meaning the actual thickness will vary a bit. This can be an infuriating problem if you're not prepared! Never make assumptions, always measure twice and cut once.

You should always have a set of digital calipers on hand to measure the wood. Close the jaws on the sheet as shown to get an exact measurement.

CREATE A THICKNESS PARAMETER

Any time you're making flat pack furniture, you almost certainly should use a parametric thickness. In 3D modeling, parametric means that a variable has been established that can be changed later, automatically changing any part of the model that used the parameter.

Plywood thickness changes from batch to batch, even from the same supplier, so if you use parameters, you can just change the parameter to adjust all of the parts instead of doing it manually- this will save you hours of work!

To set a parameter, go to MODIFY > Change Parameters, click the green plus-sign next to User Parameters to create your thickness parameter.

  1. Name: The name you'll use to enter the parameter in any number field. This should be as short as possible because you'll be using it a lot, so pick "t" for thickness.
  2. Unit: Defaults to the units your file is working in, but you can use any unit you want and it will automatically convert.
  3. Expression: This is the value in selected units of the thickness of your plywood. This will be different for practically every batch of plywood, so use digital calipers to measure your plywood to get an exact measurement. Mine is .76.
  4. Comment: This is optional, but if you've got a really complicated model it's a good idea to make a note about what the parameter is for here.

EXTRUDE SKETCH

Now that you've got your parameter set, you can extrude the tabletop profile sketch you made previously. Go to CREATE > Extrude, select the circle sketch profile, then type "t" in the Distance field in the EXTRUDE dialog that comes up. Operation should be set to New Component. Click OK and you'll have a tabletop component.

You can go back to MODIFY > Change Parameters and change the parameter value to see the thickness of the table change.


Move Table Top Component

The tabletop was made on the floor of the model, so we'll need to move it to the proper height. Click on the tabletop, then right-click and select Move from the popup dialog.

You'll get a manipulator that will let you move and rotate the part. Drag the Up arrow to move the table up, then enter 28" (710mm)- that's the standard underside height for a dining table.


Sketch Leg Profile

CREATE A SKETCH

With your tabletop in place, it's time to draw the first pair of table legs. To do this, like pretty much everything else, start with SKETCH > Create Sketch. Pick either the Front or Side plane to sketch in. You'll get a warning about parts having been moved. Be sure to click Capture Position. If you click "Continue", the tabletop will move back to the bottom plane.

PROJECT TABLE PROFILE

Remember that when you're in the Sketch environment, you're only creating lines. Parts of the 3D objects and other sketches that might be visible can sometimes be snapped to, but they don't represent lines in the sketch you're working in.

You're going to need the line representing the underside of the tabletop to make the profile of the legs. To get this, go to SKETCH > Project / Include > Project. As with any tool, hit ESCAPE to get out of it.

Click on the underside edge of the tabletop, and you'll get a pink line with points at each end. Click OK to exit the Project tool.

CREATE LEG PROFILE BOUNDARY

With the projected line, you can now make a rectangle to create a boundary for the profile of the legs. You could always just draw the legs however you like, but I like to start with boundaries that relate to other objects as a way to control the geometry. To make a boundary, just go to SKETCH > Line and complete the rectangle with the projected table line as the top. You could also use the Rectangle tool in the SKETCH menu.

Table legs should always touch the floor so that there's a significant gap between the foot and the edge of the table as seen from above. Did you ever notice how your kitchen cabinets have a kick underneath them? This recess lets you belly-up to the countertop without stubbing your toes.

The idea is the same for tables. Work backwards from the rectangle you just made to create this recess. Go to SKETCH > Offset, unchenck Chain Selection, and select one of the vertical lines. This will offset the line parallel to the original by a distance you specify. A 4" (100mm) offset will give you enough room to avoid stubbing your toes without sacrificing too much stability. Notice by pulling the arrow that you will probably need to enter a negative value since you're offsetting to the inside of the rectangle.

Think of this line as the outermost possible distance the leg can go from the center of the table.

DRAW LEG PROFILE

Now that you have your boundary complete on the left side, you can start drawing your table leg profile. To make them slanted, draw a Line from the bottom point of the line you just offset and move the other point so that it makes an angle. An 85º angle (meaning 5º off of the vertical line) works well for style and stability. You can make this angle any arbitrary angle that's close to 5º, but if you want to be precise, hit the Tab key and enter the degree in the degree box, then hit Tab again to lock it. You'll see that you can now drag the mouse to make the line longer or move it around the origin, but the angle will be locked. Click the other end of the line when you're satisfied.

This line will be the outermost edge of the table leg on the left-hand side. To give the leg thickness, go to SKETCH > Offset and offset the line you just drew. 3" (76mm) is about the minimum that will be stable with off-the-shelf soft plywood in my experience. When you've dragged the arrow in the correct direction, give it a value of 3" (76mm) and click OK.

The pair of table legs is going to be a single, connected part, so it's going to need depth to give it stability. To do this, just go to SKETCH > Offset and offset the line you projected from the underside of the table. This should also be at least 3" (76mm), but don't go too much deeper or you'll hit your knees on it!

At this point, the leg profile is finished aside from all the crossing lines. Remember, a 3D object comes from an extruded sketch (just like you did with the tabletop), so you'll need a closed profile for the table legs. You can clean up the crossing lines by going to SKETCH > Trim and clicking on the line segments that you don't need. As with any tool, hit ESCAPE to get out of it.

With your leg profile finished on one side, you can avoid drawing it again on the other side by mirroring it. To mirror, you'll need a centerline. Go to SKETCH > Line and draw a line down the center of the leg profile. You'll see a triangle symbol when you're snapping to the center of the top line. It's important that this line is vertical and centered on the drawing.

To mirror the leg profile to the other side, go to SKETCH > Mirror, then select the lines that make up the leg profile on the left side. Click on Mirror Line, then select the centerline you made in the last step. You should see a preview that gives you a symmetrical pair of legs. Click OK, and you should have all the lines you need to make your 3D part.

If you use the Trim tool again to clean up the profile, you should see a closed profile like the one shown below. This is what you'll use to create the 3D leg part. Click Stop Sketch to get back to the modeling environment.


Create First Leg

With your leg profile complete, you can now make a 3D part. You can go to CREATE > Create Component to create an Empty component to work in. This will save you having to deal with the other parts of the model- you'll be in the activated component you just made, which will gray-out the other parts as shown below.

Go to SKETCH > Extrude and click on both of the profiles separated by the mirror line. If you pull on the arrow, you'll see that the 3D part will be extruded in one direction only. You want the table leg part to be aligned with the center of the table, so you'll need to do an extrusion that does in both directions and still has the t thickness parameter.

To do this, set Direction to Symmetric, and Distance to t/2. This will extrude the part in both directions by a value of 1/2 t, which totals t.

You should end up with a new 3D part with a thickness of your t parameter that's aligned to the center of the tabletop.


Create Tab Feature

This is a flat-pack / friction-fit design, so we're going to need some interlocking features- tabs and slots. The top of the table leg part will slot into the underside of the table with a tab.

CREATE SKETCH

To create a tab, go to SKETCH > Create and select the front face of the table leg as your starting plane.

The tab should be centered on the top part and have gaps on the sides- if it's too wide it'll be too difficult to build. Go to SKETCH > Line and draw this gap at about 6" (150mm) along the top edge.

Draw another 6" line on the other side, then draw a tab that looks about half way through the depth of the table top. Make sure all the angles are 90º! The cursor should snap to 90º automatically.

USE PARAMETER FOR TAB HEIGHT

Remember, all your parts are parametric, meaning you need to make sure they'll update properly when you change a material thickness. The tab needs to be exactly half as deep as the thickness of the material. To make this work in a sketch, go to SKETCH > Dimension, and click on the top line of the leg part and the top line of the tab part. A real dimension will show up, but you'll need to change it to t/2. This will give you a tab that's 1/2 the thickness of your material and will update when you change the parameter. If the parameter was entered properly into the dimension, you should see "fx: " then a number value. In my case, it's 0.38" because that's 1/2 of .76".

Click Stop Sketch to get back to the modeling environment.

EXTRUDE TAB

Go to CREATE > Extrude and extrude the body back to meet the back face of the leg part. You should enter t for the Distance here as well to make sure the parameters are being used everywhere. Operation should be set to Join by default.


Use Leg Tabs to Create Pocket

Now that your leg is done, click the circle next to the Top-Level Component in the Browser. This will be the first item in the list. At this point you should have two components under the top level- the leg and the tabletop.

COPY BODY TO NEW COMPONENT

Next, you'll need to make a copy of the table leg for the second leg component. If you copy the component in the browser, you'll have two copies that are connected, meaning if you change one the other will change to match. If you copy the body within that component, you'll get a new, independent copy of the leg in that state.

Click the arrow next to the leg component in the browser, then click the arrow next to Bodies in that component. Right-Click on the body, then Copy+Paste it. You'll now have a new body in the Bodies folder under the Top-Level Component in the Browser.

Right-click on the body you just made, then select Create Components from Bodies. You'll get a new component that you should name something like "leg 2".

ROTATE LEG

Right-click on the new component, then select Move. Move the Rotation Arc on the Manipulator to rotate the leg by 90º. You'll now have two legs at a right-angle to each other.

CREATE POCKET IN TABLETOP

Now that the leg components are in place, you can make the pocket in the tabletop. Go to CREATE > Combine, and select the tabletop as the Target Body. For Tool Bodies, select both of the table legs, and be sure that Keep Tools is checked- if it's unchecked, both of your legs will disappear.

If you turn off the leg components in the Browser (click the lightbulb next to them) You should now see that your table has a pocket on its underside.


Create Interlocking Features

The next step will be to create an interlocking feature between the legs. The trick here is to make a tab on each leg that's half-way through the depth of the top part. This will keep the legs in place but won't sacrifice too much in the way of stability.

CREATE SKETCH FOR SLOT

Start by creating a Sketch on the face of one of the table legs.

Go to SKETCH > Project / Include > Project and select Bodies in the Selection Filter. Click on the leg part that's crossing the sketch you're drawing in, and you'll get two lines that match the thickness of the leg.

To draw the cutout, draw a Rectangle from a top point to the intersection between the lines on the opposite side of the bottom.

With that in place, bisect the rectangle with a Line from midpoint to midpoint (the triangle icon means you're snapping to a midpoint). Click Stop Sketch to get back to the modeling environment.

EXTRUDE TAB CUTOUT

Turn off the crossing table leg component in the Browser, then go to CREATE > Extrude and select the top part of the tab sketch. Pull the arrow into the component so that it cuts through, and you'll see that this will be a negative value. Enter t for the Distance, and leave Operation on Cut.

SUBTRACT TAB CUTOUT FROM OTHER LEG

There's no need to repeat all these steps for the other leg. Go to MODIFY > Combine, select the leg without the cut as the Target Body, then select the leg with the cutout as the Tool Body. Be sure to have Keep Tools checked.

You should now have one leg with a cut at the top and one leg with a cut at the bottom.


Draw Stiffener Profile

This table would stand at it is, but it would wobble like crazy. There's nothing to keep the legs from bending against the short dimension so you would basically get a twisting motion if you were to push on the tabletop. To prevent this, we'll need some stiffeners.

Go to CREATE > New Component to make an empty component to work in. Next, create a Sketch on one of the leg faces. You'll need a centerline for this part, so just draw a Line roughly down the center of the leg.

In the Sketch Pallette on the right side of the canvas (it might be nested, if so just click on the double arrow), click on Parallel under Constraint. Click one of the table leg lines first, then click the centerline you drew before. This will allow the centerline to move but will keep it parallel to the leg line. You should see a couple of double line graphics showing you they're constrained.

To make sure the line is centered, go to SKETCH > Dimension, and click the leg line and centerline. Enter a value that's 1/2 of the width of the leg, which is 1.5" (38mm) if the leg width is 3" (76mm) as shown.

This line represents the center of the stiffener from the side. To give it thickness, go to SKETCH > Offset and offset it by a factor of t/2 in both directions.

Draw a Line from the intersection at the top of the outer line so that it meets the inner line at a 90º angle. This will be the top of the stiffener.

Next, Offset the top line by 14" (355mm) to make the bottom edge of the stiffener. It needs to be at least this deep to keep the table from wobbling.

You should now have a closed rectangular profile, select it to be sure there aren't any gaps in the lines.


Create Stiffener Component

CREATE A 3D BODY

Use the side profile you just made to Extrude the part. Be sure to use the t parameter and extrude it in the correct direction. The Operation should be New Body.

When that's done, Extrude both faces of the new body by a Distance of 3" (76mm).

CREATE CUTOUT SKETCH

Like the table legs, this stiffener part will need a slot to interlock it with the legs. To do this, create a Sketch on the face of the table leg, then use the Project tool. Make sure Bodies is selected in the Selection Filter, then project the side face of the stiffener to create a rectangle that's constrained to the shape.

Draw a Line connecting the midpoints of both of the long lines that make up the rectangle. This will give you a profile you can use to create a cut in the stiffener that's half way down its length.

EXTRUDE CUTOUT

Use the CREATE > Extrude tool to select the cutout profile. If the stiffener is turned on in the browser, you probably won't be able to select the profile you want. Hit the down arrow to cycle through the possible selections with the cursor hovering over the profile until the profile is highlighted, then click on it.

Extrude this profile into the stiffener using your t parameter. This should give you a cutout that's centered on the piece.

CREATE TAPERED PROFILE

The stiffener needs to be tapered at the end to keep knees from knocking into it, it should also be narrower at the top. To make this profile, create a Sketch on the face of the stiffener.

Draw a Line from the midpoint of the bottom line to give yourself a top point to aim for.

Offset the line on the side of the cutout by a distance of -t. Be sure Chain Selection is off.

Draw a diagonal Line connecting the two points to create a tapered profile.

Draw a vertical Line at the midpoint of the cutout to give yourself a mirror reference.

Go to SKETCH > Mirror, select the diagonal line under Objects and the vertical line for the Mirror Line. This should give you a symmetrical tapered profile.

With your profiles finished, go to CREATE > Extrude and select the profiles you want to cut out of the stiffener. Use the t parameter for the thickness here as well.


Multiply Stiffeners and Create Interlocks

MULTIPLY STIFFENERS

Now that you've got a usable stiffener, it's time to copy it in place at each of the four legs. To do this, go to

CREATE > Pattern > Circular Pattern.

Set Pattern Type to Component Bodies, select the stiffener under Objects, select the model up axis under Axis, and set the Quantity to 4. This should give you four stiffeners in the correct place at each leg.

CREATE INTERLOCKING CUTS

Now it's time to cut the profiles of the stiffeners out of the legs so they interlock. To do this, go to MODIFY > Combine, select one of the table legs as Target Body, then select the two corresponding stiffeners as Tool Bodies. Be sure to have Keep Tools checked or your stiffeners will disappear. Repeat this step with the other leg component.

This will leave behind a small wedge at the top of the cutout, so just select those faces and extrude them so that they cut all the way through the top of the leg.

When you're done, the legs and stiffeners should look like the picture below.


Fillet Sharp Corners

Sharp corners tend to split and chip easily, they're sharp to the touch, and, in my opinion, they don't look as nice as rounded corners. To round off the corners, go to MODIFY > Fillet, and select the edges of the legs and stiffeners to fillet them. You can do multiple parts at once, but in the video, you'll see that I did a few different fillet radii for different parts. The tapered points of the stiffeners should be about a .25" (3mm) radius to keep them from being shortened too much. You'll see that when you fillet the edges on one of the stiffeners, all the other ones will change automatically, since they're all copeis of each other.


Recap

We covered quite a lot in this lesson. Give yourself a hand if you stuck with it and modeled something!

Your finished table should look something like this:

Did you design a table or something similar?

CLASS PROJECT

Share a photo of your finished project with the class!

Nice work! You've completed the class project