3D Carving Pinewood Derby with Fusion 360

Patrick Rainsberry

Project by

Patrick Rainsberry
Alta Loma, USA

General Information

Here is a project showing how to use Fusion 360 to model a pine derby car, set up the 3D CAM and then cut it on an X-Carve.

http://youtu.be/agLS_PRQJLQ

Like this project
File Description Unit Price
File-type-blank

Pine Wood Derby.f3d

Here is the finished car with the CAM Setup

$0

File-type-blank

pinewood_car.stl

STL Model of Car by request

$0

Download Zip

$0
from Inventables

1

Get Fusion 360

Download Fusion 360 here:
http://autode.sk/Fusion360Download
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.

2

Sculpt - Intro

Fusion 360 is capable of all kinds of different solid modeling and design. For this particular project we will be using the sculpt environment. This is a very easy way to develop complex shapes quickly.

Select the sculpt command to start a new shape.
Create a new Box with the following dimensions 1.5 X 7 X 1.25
Select the crease command and crease all of the bottom edges
Select the symmetry command to apply symmetry to the model.

(You’ll notice in the video I modeled the car a little wider. I will then scale it down later)

3

Sculpt – Insert Edges:

Insert Edge will allow you to create more definition in the model.
Double click to get an entire loop
Insert an edge on “both sides”
As you continue to refine the shape you can continue to insert edges to achieve the desired result

4

Sculpt - Modify

Begin dragging edges with the modify command.
Start with a basic shape and refine it as you go.
You can drag Edges, Faces, or Vertices
Don’t worry too much about the options in the dialog at this point
Just select an entity in the window and use the manipulator to drag it around

5

Sculpt – Subdivide Faces

Select subdivide face command
Select faces onto which you want to create more definition
More faces gives you more control over the shape in that area

6

Sculpt – Finish

Continue to refine the geometry until you are happy with the shape.
Finish the sculpt command

7

Scale (Optional)

Possibly add a scale feature to your model.
In the video I modeled it originally to the wrong specs. It is sometimes very convenient to take an existing model and scale it to fit a particular piece of stock material. Also if you have a model you really like but realize your stock is just a little too small this is a really easy way to make some small adjustments to get it in there.

8

CAM Setup

I have found the easiest way to manage tool paths in Fusion 360 for the X-Carve is to create a unique “setup” for each tool (and possibly part orientation). Each setup in the CAM tool will be easily processed as a single G-Code file. This is what you will use to actually communicate with the machine later.

Switch to the CAM mode in Fusion 360
Create a new setup
Select your model
Enter in specific sizes for Stock
Select the origin point for the stock. By using the bottom left corner of the model we can setup a zero that will easily facilitate changing tools.
Set the model to be at the bottom of the stock
(You can rename the setup or tool paths by slowly clicking the name twice)

9

CAM – Roughing Tool Path

We are going to cut this part in two phases: roughing and finishing. For the roughing pass we will use a flat end mill.
Create a new 3D Pocket tool path
Select a tool from the library (1/8” flat end mill)
Set the feeds and speeds. I used these based on some info I read in the forums.
Select the “Passes” tab
Set the Maximum Roughing step down to be .05”
Set the stock to leave to be .04”

10

CAM – Finishing Setup

Create a new setup
Use all of the same settings from previous setup
(Alternatively you can copy/paste the existing one and delete the roughing operation from the new setup)
**Important: Make sure you position the origin point in the same place in both setups

11

CAM – Finishing Contour

Create a 3D Contour tool path
Select a tool from the library (1/8” ball end mill)
Set the feeds and speeds.

12

CAM – Finishing Parallel

Create a 3D Parallel tool path
This is maybe a little over kill but thought I’d show two types of finishing
Set the set over to be nice and small like .04 (This isn’t high run production so lets not worry about time)

13

CAM –Simulate

You can simulate the tool path to make sure everything looks good
Select a single operation, a setup or the entire Operations folder
Turn on Stock to see what is cut away
Turn off tool paths to see the stock better

14

CAM – Post Process

Select the first setup (with the 3D Pocket operation)
Select Post process
Save it out with a name so you’ll remember: Pinewood_Flat_1_8
Select the second setup (with the finishing operations)
Select Post process
Save it out with a name so you’ll remember: Pinewood_Ball_1_8

15

Edit G-Code *IMPORTANT*

Important: Have you set a G28 position? No?

If you don’t know what this is or haven’t set it you must open the g-code files and REMOVE the lines that start with G28.

I will add a tutorial at some point on this but for now if you don’t remove these lines you will probably crash your machine.

After exporting the G-Code Fusion will launch an editor where you can view the code. Use search to find G28 and delete those lines. (cmd+f. ctrl+f)

Typically there would be three lines one at the beginning and 2 at the end.

This is actually nice if you have set it as it will send your machine to a nice “home” position when it is done and before it starts.

16

Part Setup

I first did this with only tape and it knocked free after a while so I had to restart. I think it might have just been too hot in the garage usually this heavy-duty double sided paper tape is enough. Anyway I decided to fixture it much heavier.

I just put a couple screws in the bottom through a piece of scrap wood and then taped and screwed the waste board down.

Probably total overkill but after losing one part way in I didn’t want to waste any more.

Also I like to make sure to square the material nicely against the side of the X-Carve

17

Measure Z (Optional)

If you want to really dial it in at this point you can measure the actual Z height off the work surface. Here you can see it is slightly off of the supposed height of 1.25”

After you take the measurement you would go back into Fusion 360.
Change the Z height in the Setup for the two tools to match this value.
Click “regenerate” on the operations.
Post the g-code again
Delete G28 commands if you aren’t using them!!!

18

Set Work Zero

Open up Universal G-Code Sender (UGS).
Use the jog functions to move the tool (flat end mill) to the lower left corner of the wood.
Click Reset X and Reset Y in UGS.

Now jog the tool a little away from your work piece and bring it down to the work surface. A nice trick is to use a piece of paper under the tool. As you lower Z (use small increments) keep moving the paper until it won’t move anymore, then you are just touching.

Now click Reset Z in UGS.

19

Run the job

Load the first file
If you are unsure you may want to set Z a couple inches up in the air and do a test run.
If the tool starts to take off in an unexpected direction you probably didn’t remove the G28 lines.

Run the G Code

When it is done cutting jog the tool to a safe place.

20

Switching tools

After the first code is done all of your zeros are still good for the part.
You may want to jog the machine to an easy location to change the bit.
Make sure not to ever forcibly move any of the axis or it will mess up your X/Y.
Change the bit to a Ball end mill
Now jog the Z Axis down so it is just touching the bed.
Zero JUST the Z-Axis (Your X and Y are still good)
Load the second file (Ball end mill)
Run the code

21

Done!!

Well done congratulations.

Post some pics if you do this project and let me know what you think!!!

Paul Munger
Need Help!!! Cant get ur project to open. Nor can I get 360 to generate tool paths!! Every time I try it says Invalid paths cant be regenerated????? uber confused.
Paul Munger
Paul Munger
Very knowledgeable with Illustrator from cs2-cs6. New to 360 though. Tutorials not working?? wonder if its my system??? win 10 4 g 64 bit
Paul Munger
Patrick Rainsberry
Hello Paul, What exactly are you having difficulty opening? If you are generating tool paths is it on a different model? I'll tell you there will be a bit of learning curve as you move from Illustrator to 3D CAD, but you will be surprised how easy it does come.
Patrick Rainsberry
Patrick Rainsberry
If you are having problems getting Fusion to load, then the best place to go is here: http://forums.autodesk.com/t5/fusion-360/ct-p/1234 the team is extremely responsive to requests for help in the Fusion forum.
Patrick Rainsberry
Patrick Rainsberry
Also if you click the help icon in the upper right corner of the screen you will see Step-By-Step tutorials option. If you just want something quick to get familiar with different aspects of using Fusion 360 this is another good way to go.
Patrick Rainsberry
Paul Munger
So when I am in the cam mode the default xyz axis are not on the same planes as yours and I dont know how to switch this??
Paul Munger
Paul Munger
It seems y and z are backwards? x seems fine also I notice when u open your new project the numbers and planes are the oposite direction of when I open mine up???
Paul Munger
Paul Munger
Im actually just trying to make a simple acoustic guitar bridge!! Lol and having a hell of a time! lol
Paul Munger
Patrick Rainsberry
This discussion is probably better had in the forums, so we can post longer than 300 words but I will try.
Patrick Rainsberry
Patrick Rainsberry
You create the work piece coordinate system when you create a new setup for the part. In the setup dialog box you can define the XYZ orientation. By default under Work Coordinate System you see model orientation. Here you can change from Model orientation to selecting the direction for Z and X
Patrick Rainsberry
Patrick Rainsberry
For the default orientation in preferences one important thing you may want to set is "Z up." If you click on your name->preferences, you'll see an option for default model orientation, select Z up.
Patrick Rainsberry
Patrick Rainsberry
This will only apply to new parts, but I think it makes things much simpler if you will be machining them.
Patrick Rainsberry
Paul Munger
Sweet. Ill give this a whirl. just gettin up and around:-) I wish I had someone like u here for one hour!! Lmao. Id learn more watching u! tutorials it seems i have to watch hours just to get to a part of the tutorial that i can use ! Lol. ok forums. ill check it out. Thamks patrick!!
Paul Munger
Patrick Rainsberry
Where are you located?
Patrick Rainsberry
Paul Munger
Im in Ithaca Ny
Paul Munger
Paul Munger
I switched to z up but It did not change???
Paul Munger
Patrick Rainsberry
Like i said it is a global setting for "New Designs." If you create a new design you should now see that Z is up.
Patrick Rainsberry
Paul Munger
yup It switched after I closed and reopened. So What is The g28? And do I disable it? as well do I delete just g28 or the whole line?
Paul Munger
Paul Munger
Theres One up top and two at the bottom right?
Paul Munger
Paul Munger
And Thank you Patrick for your help! Im two inches away from getting a carving now!!
Paul Munger
Paul Munger
And its universal g code sender ur using right???
Paul Munger
Patrick Rainsberry
NP, Here is a good discussion on G28: https://discuss.inventables.com/t/learning-about-g28/12205 Yes one at the top and two at the bottom Also you can disable it in the post options. You can see that in the video.
Patrick Rainsberry
Patrick Rainsberry
Yes correct, I am using Universal G-Code sender in this tutorial.
Patrick Rainsberry
James Moore
Here's a video I made on how to adjust the axes using the little indicator thing: https://screencast.autodesk.com/main/details/87a6567a-3f75-4e0b-ae0b-db39a2899561
James Moore
Paul Munger
I watched the post but am still a little confused. do i disable it AND delete the whole G28 line AND write the G28.1 then G28?? One of these all of these in a specific order???
Paul Munger
Patrick Rainsberry
If you uncheck "Write G28" in the post processor options then there won't be G28 lines in your g-code at all. Your decision to use it or not. If you are having trouble best to not use it at first.
Patrick Rainsberry
Paul Munger
so my comp updated and now 360 wont even open at al??
Paul Munger
Paul Munger
brand new . a month old
Paul Munger
Patrick Rainsberry
Hey Paul, I really want to help you but the comments section of this tutorial is definitely not the best place. I recommend you post your install problem here: http://forums.autodesk.com/t5/fusion-360/ct-p/1234 Somebody will get back to you very shortly.
Patrick Rainsberry
Paul Munger
ok. I will . Ive been Wicked busy and at that not only fusion 360 but the last 5 carves on easel all screwed up on me. the hdpe knuckles!! Cut one fine then destroyed multiple stocks. im on the verge of either returning this thing or driving to chicago at this point. im pretty pissed
Paul Munger
Patrick Rainsberry
Have you posted the issue in the Inventables forum? They are usually really good about helping people. They wouldn't be monitoring these comments though i don't think. Forum is really best place for help. Not here.
Patrick Rainsberry
Rick Troiani
Love the work you've done. I have a friend who has to make a derby car for his kid and I have a Shpeoko 3. I don't have fusion, but have Meshcam. Any chance you would post a .STL of your car so I can make him one?
Rick Troiani
Patrick Rainsberry
Just posted. If you want Fusion 360 is free for personal use and that file already has the tool paths in it as well. Good luck!
Patrick Rainsberry
Rick Troiani
U Rock! I didn't see where F 360 was free for personal use, but am definitely going to check again. It blows away Meshcam! Thanks again!
Rick Troiani
Patrick Rainsberry
Awesome. Yah just download it and after you start the trial there is an option to say personal/hobby use. Then you are good to go.
Patrick Rainsberry