This is a fairly in depth step by step tutorial on using Fusion 360 to design a Flat-Pack bookshelf for manufacturing on a CNC router such as a ShopBot.

It assumes a fairly basic knowledge of using Fusion 360.

Much thanks to Martin and the rest of the Pier 9 staff for all the help and advice getting this done.

You can view and copy the files here:

http://a360.co/1KQ01ik

Here is a link to a youtube video of the entire process as well:

Here are the two scripts that I use:

Nesting Script:
https://github.com/tapnair/NESTER

https://youtu.be/7SY367qt3YQ

Dog Bone Script:

https://github.com/caseycrogers/Dogbone

https://www.youtube.com/watch?v=EM13Dz4Mqnc

Step 1: Get Fusion 360

Download Fusion 360 here:

http://fusion360.autodesk.com/

After installation create an account to login. Fusion 360 is free for non-commercial use. It will start in a 30-day trial. At the end of the trial you can either purchase a license for $300/year for commercial use or select that you will be using it as a student, hobbyist or startup, which allows you to use it free.

When you launch Fusion you will be in a new design.

Learning the basics

It is recommended that you do some of the basic tutorials before attempting this one.

This tutorial is fairly simple, but assumes the user has a basic knowledge of working in Fusion 360.

Step 2: Create Parameters

We are going to create some parameters for this design. This will allow you to make modifications later in one place and then have those changes reflected everywhere.

Select: Modify/Change Parameters

In the User parameters section create all of the following parameters. It isn’t necessary to this for every value but it is really nice later. This way as we build the model all of these values will be used and easily edited in one place.

The most important parameter in here is ply. This is set to the thickness of the material. By using this technique you can easily adjust all of the pieces, fits, slots, etc. that depend on the material thickness. This is where using a 3D parametric modeler has huge advantages.

Measure the exact thickness of your stock and enter that value here. In the future you can just change the value here and in the CAM setup to rerun the job for the new material thickness.

Step 3: Create Sketch

Select: Sketch/Create Sketch

Select the Right plane.

Select Sketch/Rectangle/2 Point Rectangle

Type in Height for the height, press tab and Depth for the depth and press enter twice. Alternatively you can draw the rectangle and then place a dimension after the fact.

Draw more rectangles.

Use the dimension tool to match the following sketch. All of the dimensions shown reference a different parameter. All of the .725 for example are actually ply. If you see the fx designator next to the dimension you know it is actually an expression, in this case a reference to the parameter we defined previously.

Select: Stop Sketch

Step 4: Create Extrusions

In Fusion 360 you can extrude any profile in the sketch. In this case we have a lot of overlapping sections. When you are extruding the various pieces make sure you are selecting all of the regions in the sketch that correspond to the actual area you want to extrude.

Select: Create/Extrude

Select the top rectangle (you actually need to pick two profiles).

Type Width into the value for the extrude depth

Select “New Body”

Select: Create/Extrude

Select all the rest of the profiles (12 of you did the sketch the same)

Type Ply into the value for the extrude depth

Select “New Body”

(This is important because the default is to join this to the previous extrusion. In this case we want separate pieces for each component in the bookcase)

Step 5: Mirror Side Piece

Often times it is easier to simply mirror or copy components than to redraw them.

Select: Construct/Midplane

Select the two outer faces of the top shelf

This gives you a plane at the center of the model. This will be very handy for many things we will do later.

Select: Create/Mirror

Set the filter to “Bodies”

Select the sidepiece as the part to mirror

Select the newly created mid-plane to mirror about.

Step 6: Create Projected Sketch

Select: Sketch/Create Sketch

Pick the inside face of the bookshelf

Using the tree on the left select the light bulb next to sketch 1.

Select: Sketch/Project Include/Project

Select all the following lines from Sketch 1

This basically transfers the lines from the original sketch into this plane. We will then use this sketch to create the shelves. We don’t want the shelves to start at the outer edge; we want them on the inner edge. This technique is nice because it maintains the associativity.

Select: Stop Sketch

Step 7: Create Other Components

Select: Create/Extrude

Select the profiles for the back piece (5 in my case)

For distance select “To” and pick the inside face of the other side piece

Select “New Body” (Again this is a very important step)

Repeat this process to extrude the two shelves and the kick plate. Do each one as its own feature to make things easier to edit later.

When you are done you can rename the bodies in the tree at the left by slowly double clicking them. (Click, then click again). Change the names if you like to make navigation easier.

If you want to apply an appearance you can right click in space “Appearance”

Select a nice looking wood suck as Oak. Drag it onto the bodies.

Step 8: Create Tabs on Kick Plate

Now we need to create tabs on all of the parts for the joints. There are a couple ways to do this; we will look at different ways.

When dealing with many bodies in the same part there are some best practices to follow. For example if we are going to extrude some tabs on the kick plate it is often times a good idea to hide the other bodies. Using the tree at the left you can select the light bulb to toggle the display of the other parts. Alternatively you can select the part you want to display and right click / Isolate.

Select: Sketch / Create Sketch and select the front face of the kick plate.

Draw two rectangles approximately in this position (Sketch/Rectangle/2 point rectangle)

Draw a line at the center of each rectangle to define the mid point.

Select this line and right click / Toggle Construction.

Dimension the sketch as follows.

Notice some of the dimensions reference a parameter such as ply. Some of the dimensions can all create equations on the fly. For example here we use “Width / 3” for the position of the tab. This type of equation driven design makes it VERY easy to make modifications later.

Select: Stop Sketch

Select: Create / Extrude

Select Join

Select “To” for the depth and pick the back face of the Kick Plate

Step 9: Mirror the Tab

Select: Create / Mirror

Set the filter to faces

Select the side faces of the tabs. (6 in total)

Select the mid plane we defined previously as the plane

Step 10: Create Shelf Tabs

Hide the kick plate and show the bottom shelf.

Select: Sketch/Create Sketch

Select the top face of the bottom shelf

Select Sketch/Rectangle/2 Point Rectangle

Draw the three rectangles shown.

Draw lines at the mid points of each rectangle. Again make sure the line “snaps” to the midpoint. Select these lines and make them construction by right clicking “Normal/Construction”

Create the dimensions shown. Again they can be parameters or equations of parameters like: “Width/3.”

Select: Stop Sketch

Select: Create/Extrude

Pick the three profiles

Set the depth at “To” and pick the back face of the bottom shelf

Select “New Body” for Operation

Select OK

Step 11: Mirror Tabs

Select: Create/Mirror

Set the Pattern Type to bodies

Select the three new bodies

Select the mirror plane you previously created

Step 12: Mirror Tabs to Other Shelf

Rather than recreate the tabs on the other shelf we can simply mirror them up.

Show the Shelf

First create a new plane

Select: Construct/Mid-plane

Select the top of the bottom shelf and the bottom of the shelf

Select: Create/Mirror

Set the Pattern Type to be Bodies

Select the 6 tab bodies

Select the new plane as the mirror plane

Step 13: Combine Bodies

Select: Modify/Combine

In Target body select the Main Shelf Body

For Tools select the 6 tab bodies

Unselect keep tools

Operation: Join

This will combine all 7 of these bodies into a single part. This will be one part for our cutting operations latter.

Repeat the process for the Bottom Shelf.

Step 14: Create Back Tabs

This process is the same as creating the tabs previously for the shelf.

Hide the other bodies and Show the Back piece

Select: Create sketch on the front face

Draw three rectangles and create the centerlines

Dimension the rectangles as follows

Select: Create/Extrude and select the 3 tab profiles

Select New Body for operation

Set depth at “To” and pick the back face

Select: Create/Mirror select the 3 bodies

Pattern Type: Bodies

Plane: The original mirror plane you created

Select: Modify/Combine

In Target body select the Back Body

For Tools select the 6 tab bodies

Unselect keep tools

Operation: Join

Step 15: Create Side Tabs

This process is the same as creating the tabs previously for the back.

Hide the other bodies and Show the Left and Right pieces

Select: Create a sketch on the left side outer face

Draw two rectangles and create the centerlines

Dimension the rectangles as follows

Select: Create/Extrude and select the 2 tab profiles

Select New Body for operation

Set depth at “To” and pick the back face

Select: Create/Mirror select the 2 bodies

Pattern Type: Bodies

Plane: The original mirror plane you created

Select: Modify/Combine

In Target body select the Left Body

For Tools select the 2 tab bodies

Unselect keep tools

Operation: Join

Select: Modify/Combine

In Target body select the Right Body

For Tools select the 2 tab bodies

Unselect keep tools

Operation: Join

Step 16: Add a Lip

Show all the parts

Sometimes it easier to modify geometry later in the tree than going back and redoing the strategy you used to originally model with. If you notice there is a problem if you show all the parts now. The tabs extend right into the edge of the top piece as well as the back of the sidepieces. We could go back and really re think what planes everything was modeled from or we can simply make a slight modification to the existing faces with a move face command.

Select: Modify/Press Pull

Select the three back faces of the model

Offset Type: New Offset

Distance: .5” (Or what ever you like)

Note: now technically our depth is not exactly the value we set in the parameters the real depth of the whole bookcase is now .5” deeper. If you still wanted exactly the value specified then you could modify the parameter to be smaller by .5” and the same for the following operations.

Step 17: Repeat Lip

Now we will repeat the operation for the two other faces that need to be extended.

Select: Modify/Press Pull

Select the left face on the edge of the top piece

Offset Type: New Offset

Distance: .5” (Or what ever you like)

Select: Modify/Press Pull

Select the right face on the edge of the top piece

Offset Type: New Offset

Distance: .5” (Or what ever you like)

Note: again the model is now 1” wider than the specified original width parameter.

Step 18: Create Pockets

Now that we have created the tabs on all of the parts we can use them to automatically cut away the pockets, a nice feature.

Select: Modify/Combine

Target: Bottom Shelf

Tool: Kick Plate

Operation: Cut

Select “Keep Tools”

When you are doing a cut the Target is the body you want to remove material from and the tool is the body that will do the cutting. If you do not select the “Keep tools” option the software assumes the tool bodies are no longer needed. That is not the case here.

Step 19: Repeat Pockets

Select: Modify/Combine

Target: Back

Tool: Bottom Shelf, Shelf

Operation: Cut

Select “Keep Tools”

Select: Modify/Combine

Target: Left

Tool: Kick Plate, Bottom Shelf, Shelf, Back

Operation: Cut

Select “Keep Tools”

Select: Modify/Combine

Target: Right

Tool: Kick Plate, Bottom Shelf, Shelf, Back

Operation: Cut

Select “Keep Tools”

Select: Modify/Combine

Target: Top

Tool: Left, Right, Back

Operation: Cut

Select “Keep Tools”

At this point the model is done! The only thing missing is to apply dog-bone fillets to the inside corners. We will do this in a future step.

Step 20: Part 2: Fabrication Features

At this point you have created everything you need for the basic model of a bookcase. But now we want to setup the model to be manufactured. This will include creating stock for reference, laying the parts out flat, and creating dog bone fillets.

Step 21: Create a Reference for the Stock

This step is not necessary, but I think it is worthwhile. The next thing we are going to do is lay all of the parts flat. So that we have a good sense of how they will fit on a sheet I like to quickly model a sheet to represent the stock.

Select: Create/Box

Select the X/Y Plane

Draw a box 48” X 96” to represent your sheet of material

Select Stop Sketch

Set height to ply

Select ok

Step 22: Create Components

In Fusion 360 there is a distinction between components and bodies. I find it easier to model things as bodies and then when you are done turn them into components. This makes things like the combine operations we did earlier, simpler.

Use the tree at the left and select all of the bodies in the design

Right Click and select “create components from bodies”

You can now rename the new components if you like.

Step 23: Fix Stock

We don’t want the stock to move around.

Select the Stock component from the tree at the left.

Right Click, Ground (This will keep it from moving around)

Step 24: Create Joints

One major difference is that with components you can apply joints. Joints allow you to create relative movement between parts. I have found this very useful for laying things out in a sheet and then dragging them around.

Select: Assemble/Joint

Pick the bottom face of the Top (you may have to select twice to place the origin at the center)

Pick the top face of the stock

Select Planar in the “Type”

You may have to hit “Flip” to get the orientation correct. Here we want those blind pockets facing up.

Step 25: Repeat Joints

Use the same process to create a joint between each part and the top face of the stock. When you are done all the parts should be stacked up in the center.

You should have created 7 joints in total.

There is a script I made that can actually make this process easier.

See it in action here:

https://youtu.be/7SY367qt3YQ

Download the script here:
https://github.com/tapnair/NESTER

Step 26: Move Components

Now that you have made joints it is really easy to just drag components around to place them.

Just select them in the graphics area hold down the left mouse button and drag them around.

If you accidentally move the stock or don’t like something you’ve done you can always hit undo (ctrl+z, command+z)

For more precise movements or to rotate parts you can use the move command.

Select the component from the tree at the left so you are moving the component not its underlying geometry.

Select: Modify/Move

Now you use the drag handles to move or rotate the parts.

Step 27: Create a Snapshot

After you are satisfied with the position of the components,

Select: Position/Create Snapshot.

This will fix the position of all the components as you moved them around.

Step 28: Create Dog Bone Fillets

So we have all of these sharp corners that we need to lie

flush. For this we will use a dog bone fillet. Casey Rodgers has developed an Add-in to do just that. I have also modified it slightly to allow the selection of bodies as well as edges. In the case of selecting a body it will apply a dog bone fillet to any vertical edge that is on an inside corner. If you have some corner that you don’t want to apply a fillet to then simply select the edges you do want.

Download the Add-in here:

Casey’s Original: https://github.com/caseycrogers/Dogbone

Patrick’s Fork: https://github.com/tapnair/Dogbone

Once it is running you should see it in the Create menu

Hide the stock component

Select: Create/Dogbone

Select the 7 parts

Cutter Diameter: cutter

This way if you change the diameter of cutter you want to use then the features will update.

Note: this is a user-generated add-in and does not perform at the same level as a true feature. In this case there are roughly 150 corners that need fillets and it takes a few minutes to apply them all, be patient. Also if you do significant changes to your model you will have to re-apply the feature. Simply delete the feature from the timeline and re-apply it.

Here is a link to video that describes the use of the Add-in in more detail:

http://www.youtube.com/watch?v=EM13Dz4Mqnc

Step 29: Adjust Blind Pockets

One last modification for fabrication. The blind pockets are currently modeled exactly flush to the ends of the blind tabs. We should add some clearance.

Select: Modify/Press Pull

Select the bottom faces of the six pockets on the Top component and the two on the Bottom Shelf

Select “New Offset”

Value: -.04”

This will cut the faces back a bit and give us a little more clearance.

Note: The rest of the pockets are modeled exactly flush. I have found that with the accuracy of the ShopBot and with a good measurement of the stock this will give a very nice press fit.

Step 30: Part 3: CAM

Now that we have set the model up for manufacturing it is

time to create tool paths. In Fusion this is done right inside the design Software. The advantage here is that you can then make changes to the model and the tool paths are easily re-generated.

To switch to the CAM Environment, select the Drop down under Model and Select CAM

Step 31: Cam Setup

The first thing we do in CAM is to create a “Setup.” This is a collection of operations. When using a CNC router (with out tool changer) I like to make one setup for each tool I will be using. In this case that is just a single compression flat end mill.

Select: Setup/New Setup

Now we need to orient the stock.

Select the back half of the X Axis and then select a model edge in the desired X direction

Select the end of the X-Axis to flip its direction.

Now select the Stock Point input box. Select the lower left corner of the stock on the top of the material.

Select the Model Input Box. Now select all the parts of the bookcase.

Select the Stock Tab in the dialog

Set the size to be 48 X 96 X .725 (You should modify this value to your exact stock thickness)

Step 32: Create Pocket

First thing to do is to cut out the blind pockets.

Select: 2D/2D Pocket.

Select a tool (in this case I am just selecting a generic 2 flute, 3/8” cutter)

Set the feeds and Speeds as you would for your material. Here I am cutting a little slower because of the modified head we have on the machine.

Select the Geometry Tab

Select the 8 Pockets.

Make sure you have the pocket defined in the correct “direction” See the images. If the pocket is in the wrong direction the blue will be outside as will the arrow, to change the direction click on the red arrow.

Select the Passes Tab

Select Right (conventional milling) – Climb milling is better suited to very rigid CNC machines cutting metal at high tolerances.

Set the maximum step over to be half the cutter width if you like.

Select Multiple Depths

Set the maximum step down to be half the cutter diameter (.1875 here)

Also set the Finishing step down to be the same (If you don’t want a real finishing pass)

Uncheck Stock to leave (This is useful if you were going to be doing a finishing pass later)

Select the Linking Tab

I take mostly defaults here.

Change the ramp type to Plunge

Step 33: Create Internal Contours

Now we will cut out the through pockets. You could use a pocket here or a contour. I used a contour, but if you were using a smaller tool it might be nice to use a pocket, as it would clear out all the material and not leave a small piece in the middle

Select: 2D/2DContour

Select a tool (in this case I am just selecting a generic 2 flute, 3/8” cutter)

Set the feeds and Speeds as you would for your material. Here I am cutting a little slower because of the modified head we have on the machine.

Select the Geometry Tab

Select the 18 Pockets.

Make sure you have the pocket defined in the correct “direction” See the images in the previous step. If the pocket is in the wrong direction the blue will be outside as will the arrow, to change the direction click on the red arrow.

Select the Passes Tab

Select Right (conventional milling) – Climb milling is better suited to very rigid CNC machines cutting metal at high tolerances.

Set the maximum step over to be half the cutter width if you like.

Select Multiple Depths

Set the maximum step down to be half the cutter diameter (.1875 here)

Also set the Finishing step down to be the same (If you don’t want a real finishing pass)

Uncheck Stock to leave (This is useful if you were going to be doing a finishing pass later)

Select the Linking Tab

I take mostly defaults here.

Step 34: Create External Contours

Now we will cut out the actual pieces. Here we are going to apply some tabs to keep the parts attached to the stock.

Select: 2D/2DContour

Select a tool (in this case I am just selecting a generic 2 flute, 3/8” cutter)

Set the feeds and Speeds as you would for your material. Here I am cutting a little slower because of the modified head we have on the machine.

Select the Geometry Tab

Select the 7 parts external contours pick any edge at the bottom of the part.

Make sure you have the contour defined in the correct “direction” See the images in the previous step. If the pocket is in the wrong direction the blue will be outside as will the arrow, to change the direction click on the red arrow.

Check the Tabs option on the geometry tab.

Select Triangular

Select “at points” for Tab Position

Pick points on your model to apply the tabs. I put 4 tabs per part

I used a tab .75” wide by .185” tall (On recommendation from Pier 9 staff)

Select the Passes Tab

Select Right (conventional milling) – Climb milling is better suited to very rigid CNC machines cutting metal at high tolerances.

Set the maximum step over to be half the cutter width if you like.

Select Multiple Depths

Set the maximum step down to be half the cutter diameter (.1875 here)

Also set the Finishing step down to be the same (If you don’t want a real finishing pass)

Uncheck Stock to leave (This is useful if you were going to be doing a finishing pass later)

Select the Linking Tab

I take mostly defaults here.

Step 35: Simulate

Simulation of your tool paths is a really nice feature. I have found many mistakes in my setups by looking at the result after doing a simulation. I highly recommend doing this every time before posting out your g code.

Select the Setup folder

Select: Actions/Simulate (or you can right click the setup folder)

Turn on Stock display by checking the box.

You can press play to watch it simulate. You can drag the slider to speed things up.

Also you can skip to the end to see the result.

Step 36: Post Process

Once you are satisfied that everything is setup its time to create g code for the machine.

Check that the value of ply is the same as the actual thickness of your material. Also check that this same value is set as the stock thickness in the CAM setup operation. Accurately measuring this will ensure a nice press fit of your parts.

Select the Setup Folder

Select: Actions/Post Process

Select the “shopbot iso.cps” post to create generic g code or the “shopbot.cps” to generate open SBP code.

Select ok and save this file to disk.