Editing CNC Router (section)

==Aspire==

#Open up Aspire 8. [[File:Aspire Icon.png|thumb|The Aspire 8 Icon]]
#Start a new project (you can not directly “open” a vector file, you can only open Aspire project files so you must start a new project).
#Specify material size. Measure your material in multiple places and go with the thickest value.
#Import your file. File > Import > Import Vectors.
#Scale your project appropriately. If after importing your design looks either too small or too large for your selected material size. You can scale it by selecting all vectors and selecting the scaling icon (show image). However it is worth mentioning that even though vectors are scalable, you can specify a size for the overall vector image in most vector design programs. Start off working in inches and design to the scale you want to cut at and you should be able to avoid any scaling issues after import.
#Delete any reference vectors or lines that you do not intend for cutting. For instance if you had a dimensional marker left over from a CAD program that you don't want to cut, delete it and get it out of the way.
#Make sure your vectors are contiguous. If they are not, you can join them by first selecting the vectors to join then Edit > Join Vectors. A pane will appear telling you how many vectors are open and which tolerance you should have on joining the vectors.
#Click on tool paths on the right pane. You may need to click out of a pop-up pane.
#For general cutting along a vector, select 2D Profile Tool path. Click on “Show advanced tool path options”.
#You can set your start depth. 0 is the top of the work piece. Set your cut depth to be just slightly over the thickness of your piece, an extra .1” is a good max.
#Next, select your end mill. Clicking Select will allow you to choose different styles of end mills and bits. Click on Edit to edit the tool options.
#Enter your tool diameter. Don’t worry about pass depth, that will be set another way.
#Enter your Spindle Speed, Feed Rate, and Plunge Rate. To determine these, see the section on Chip Load.
#Click on Edit Passes to specify the number of passes and pass depths. When selecting the number of passes, you need to consider the end mill. Given a chip load of .01 inches per tooth, the pass depth should never exceed the radius of the end mill. The chip load equation is designed with a step down of the radius of the end mill so you should stick to pass depths of the radius or less. For a ½” sheet of plywood, I’ve selected 5 passes at a depth of 0.12 inches. The pass depth is calculated off of your cutting depth value and not your material thickness value.
#Next select the direction and orientation of the cut. You can cut inside your lines, outside of your lines or on the line. Stick with a conventional cut as opposed to a climb cut because it reduces the forces on the wood and reduces the risk of sending a piece flying.
#Next, add tabs. Tabs are critical to safe CNC routing. Tabs are pieces of material skipped over by the router to hold your pieces together. For instance, if you are cutting a circle, when you are done the piece will be loose on the table top. Tabs ensure that the pieces stay put and resist the forces of the end mill that want to send the piece flying.<br>

 <nowiki>!!!SAFETY NOTE!!!
   Tabs are important to make sure you do not turn your project into a dangerous projectile</nowiki>

#<li value="16">Choose your tab dimensions. These should be substantial sized tabs to hold the piece. As mentioned above the forces at the end mill are very strong and without substantial support on your piece it will go flying. A good rule of thumb is they should be no thinner than 25% of thickness of your work piece and no shorter than .5” wide.
#After selecting tab dimensions, click on Edit Tabs. You can auto place them or manually place them but either way you should re-arrange them to make sure there are enough of them for the piece being cut out. A good rule of thumb is 4 tabs minimum per piece but it doesn’t hurt to err on the side of caution and add more.
#To interactively place them, select your vector, then hover over where you want the tab and left click.
#After making your tabs, select Project tool path onto 3D model. Choose a name for your profile and click calculate. If you set it up right, you will get a warning that the tool will cut through the material. This is ok as you want the tool to cut all the way through.
#Next preview your tool path by clicking play. You will probably need to slow down the speed all the way. You can change the orientation by left clicking and dragging, and you can move the piece by clicking and dragging the scroll wheel. Clicking and rolling the scroll wheel will zoom in and out. Take some time to review your preview. Make sure you are conscious of where your screws are holding down your pieces and where the end mill will go.
#Close out of the Preview pane. Select the toolpaths you want to export click on save toolpath. Export the file to ShopBot (inch)(*.sbp).