User:Brianwcallaghan/CNCtutorial
Contents |
EnRoute/MultiCAM Tutorial[edit]
The purpose of this tutorial is to familiarize you with the EnRoute software and allow you to set up and cut parts on the MultiCAM CNC router. EnRoute is CAM software. Its purpose is to communicate the information of a drawing to a machine that will execute a cut. EnRoute works with most CNC routers, laser cutters, water cutters and the like. In order to cut your parts, you will need to import and export your files several times. In short, using EnRoute to set up a cut on theMultiCAM CNC router is a game of careful setup, and a journey through 4 different file formats.
Setting Up Your Drawing[edit]
Using EnRoute version 4, I found a few limitations on files that can be imported. No error message will appear if the file is incorrect. The result will instead be partial or non-existent. With this in mind it is best to set things up nicely ahead of time.
The parts for this project were drawn in AutoCAD 2012, but theoretically, you could import from any CAD software that can save in a compatible format. As I said, I used AutoCad. See the screenshot of my leg parts to the right.
The first constraint to consider is the size of the wood you are cutting. THe table on the particular router I am using on this project is 5 feet by 10 feet, but the wood I had was 4x8. So, my constraints were 4 feet by 8 feet. I had to split the drawing into 2 .DXF files to fit all the pieces in a 4'x8' rectangle.
While drawing in CAD, you will be creating a .DWG file. When you are finished with the work in CAD, you must save your file as a .DXF. EnRoute will not see the native AutoCAD .DWG format for import. Also, EnRoute version 4 seems to prefer a downsave to a .DXF 2007 format (rather than than 2010 format).
Lastly, I found (the hard way) that EnRoute will not import elements of your drawing that were placed in an array in AutoCAD. I ended up reducing the CAD drawing to 1 of each critical piece and multiplying them in EnRoute. So, I recommend, drawing only 1 of all your parts and importing just that, to later tweak in EnRoute.
Importing Your File to EnRoute[edit]
When you open EnRoute select "New". It will ask you for a template. I selected the 4'x9' template, because that is the size of the wood I am using. There are a few other size templates to choose from based on how your machine was set up upon install. From the "File" menu, select "Import." You will get a browser window where you can locate the .DXF file you saved in CAD. Click "OK" and it will begin importing your file. The file will now be saved as a .ROU file, which is the EnRoute proprietary file format.
You may, as I did, find that all or a portion of your drawing did not show up. This could be because you saved your .DXF file in the 2010 file format rather than down-saving to 2007 format. This could also be caused by an array command in your CAD file. If this is the case, you will need to go back to CAD, explode your arrays and re-save then re-import. I removed my arrays and reduced the number of parts to one of each type. After importing, I used the 'active nesting feature in EnRoute to duplicate and position the parts.
From the "File" menu, you select "Active Nesting." A window will appear at the bottom of the screen. It asks for an angle. Enter 360 degrees. This means that it will rotate the parts any way necessary to fit them on the template. It will also ask you how far apart, the pieces need to be placed. I entered ½inch. You then click on the first part to nest and enter the number of copies of that part needed and click "OK." Repeat with all parts and the software will fit them neatly into your template. See the photo to the right of the parts in EnRoute. The arrangement of parts was done by the nesting feature.
Setting the Toolpath and Setting Up the Cut[edit]
In order to toolpath your drawing the lines must be merged. This tells EnRoute that the line is a continuous cut. You can simply select every object on the screen, right click and select "Merge Selection." Now those four lines are a square. In other words, this makes the lines into geometry in the eyes of the software. Circles will be identified as separate objects. The software will think they are raised islands until you tell it otherwise.
Select everything again. Now click the "Toolpath" menu at the top of the screen. Select "Add Toolpath." The lines of your drawing will turn blue indicating a toolpath and a window will open showing the details of your path. Click where it says edit toolpath. You will now select the bit used for the cut. i selected a 3/8 inch compression spiral bit. Ii measured the thickness of my board with a digital caliper. It was 0.2 inch. I entered this into my toolpath as board thickness. Right click on any point of the toolpath and select edit toolpath. Select add bridges. It will ask you for the bridge quantity and size. I selected 3 per piece and .5 inch wide. Bridges are automatically added to the drawing. They will be cut on the second pass of the blade.
Now you select all of the points to be drilled (the little circles). Go to the toolpath menu and select "drill centers." This will drill the center point of any selected piece of geometry. This is where the software recognizes those circles as cuts rather than islands. I select a 1/8 inch up spiral bit for drill points and a drill depth of.21 inch.
Under the Machining menu at the top of the screen you will select "Setup." Under this menu set the RPM to 18000, set the feed speed to 400 and the plunge speed to 40. These settings will protect the wood and the bit. Set your surface depth to .2 inch (or whatever your board thickness is) and the surface at the bottom. This keeps the drill from going into the table.
Under edit toolpath, you will select order. Drag tool order to the top and drag your drill bit above your cutting bit. This will make a pass to drill holes first then return to the tool carousel to exchange bits and do the 2 passes of cutting 2nd. This is ideal. It helps keep everything in place to cut in this order.
Lastly, at the top right there is a button labeled "Output." Click this and select"To File." Name your file and tell it the destination folder where the CNC router is directed to retrieve. This will export the file to our last format. It will be a.CNC file that can be read by the router. Now you should be ready to make a cut.
Starting the Machine[edit]
Once the machine is powered on at the breaker, you will place your board on the table. The table is topped with a spoilboard. The spoilboard is a porous piece of cardboard that allows air to pass through it. There is avacuum under the spoilboard and this is what holds your wood in place. Line up the lower right corner with the lines on the spoilboard and turn on all 4 vacuum levers. Return to the breaker box and turn on the dust collection vacuum as well.
At the controller for the machine press the Home key and select home number 1. This will return the tool to the (0,0) point on the grid. Now press the Retrieve button and wait for the LCD display to show the list of files in the folder. Select your file and press "Go." The machine will begin cutting.
The machine will grab the drill bit and begin the drill pass. At the completion of all drilling, it will return to the tool carousel and exchange to the cutting bit. At this time, the machine will make the first pass cutting about .15 deep into the wood. Upon completion of the first pass the machine will begin a second pass to cut the remaining .05 inch of depth leaving bridges this time.
You have to stand at the machine and wait while it cuts with your finger poised at the pause button in case something goes wrong. You can pause the cut and look at it. The cut can be resumed if all is well and cancelled if there is a problem. There is a separate Emergency Stop button that kills all power to the machine and stops it immediately. This is more to avoid injury than to pause for small mishaps or errors.
When the machine stops and the cut is done, turn off the vacuum and remove your parts. Be sure to blow off the table and clear all moving parts of sawdust.
