CNC workflow


1. open File in Partworks
2. I think it's an easy practice to put all inside profiles or pockets on a seperate layer than the outside profiles.
2.1 I think this makes it easier to select what you need and to avoid selecting what you don't need in order to generate the toolpaths.
3. Set Material Thickness
4. Uncheck "use origin Offset
5. Check "center data in Job"
6. Go to the drawing toolbar and select all the geometry in the file.
6.1 Click on the join tool and joint all geometry.
7 Under the "edit objects" area on the drawing toolbar you can find the "create fillets" tool.
7.1 This clears out inside corners and avoids the time sink that is drilling for all the inside corners.
7.2 If you have a lot of geometry, it takes a while to complete this step.
7.3 Choose dogbone or t-bone depending on your hiding preferences/techniques.
8 Select the geometry that you want to generate the toopaths for.
8.1 Go to the toolpaths toolbar and select the type of toolpath you are looking for.
8.2 For profiling, be concious of outside versus inside of the line cutting.
8.3 If you are cutting something out of your piece then cut on the inside of your line, but if you are cutting a piece out, cut on the outside of the line.
8.4 Select your start depth 0" and your ending depth (a little more than the thickness of your material).
8.5 Select your tool by clicking on the select button under the tool section of the toolpaths toolbar.
8.7 You can set the pass depth to be equal to the diameter of the tool.
8.8 If you are using a stepover, it should be no more than 50% of the tool diameter. Set the feed speed but be consious of your units (120 inches / min).
8.9 Also set the spindle speed to 18000 rpm.
8.10 And the plunge speed to 30.
8.11 Be concous of these numbers. You can determin your feed speed with the formula RPM * # of flutes * chip load. Wood has a chip load of .02 to .04. Which means you could cut at a feed speed of 140 inches/min.
8.12 You can reference THIS WEBSITE for some handy numbers for specific materials. keep in mind that the chip load is derived from the material you are cutting as well as the diameter of the bit you are using.
9. Be consious of your tool type.
9.1 Are you using a flat endmill (good for pocketing and profiling) or a ball nose endmill (good for 3d surfaces).
10. Click calculate and give the toolpath a name.
10.1 Be counsious that if you need to change tools in the middle of a job, you should save the toolpaths to different files.
10.2 If you are using the same tool throughout, then you can use a naming convention to order the toopath files top to bottom.
10.3 You can also order them maually from top to bottom before you save the toolpaths.
10.4 Cut inside profiles out BEFORE the outside profiles. You can toggle the "output all visible toolpaths" option to determine if you will output all the toolpaths into one file or to pick out only certain ones to isolate tool types for those toolpaths (check the boxes - pretty straight forward).
11 If you have nested many parts close together be advised large portions of the material may become unsupported as the job progresses.
11.1 Because of this it might be useful to run a drill pass.
11.2 You can add circles that are the exact diameter of the drill bit you are using and then us the drilling toolpaths tool to generate a drilling pass toolpath.
11.3 It is not necessary to drill all the way through the material for these only to mark where you can safely drill a srew into the material to anchor it down.
11.4 At least two screws per piece that is to be cut out is a good rule of thumb to keep them from popping up and/or rotating.
11.5 You can also use common sense to determine which areas of the left over stock should also be anchored down.
12 You can follow the shopbot along and drill screws into the table. Do this before it begins it's final profiling toolpaths.
12.1 You may have to pause the machine to complete this in time / safely.

Partworks 3D

1. Open file (.stl), Confirm model size, Confirm units -inches, Sides to machine - select which side if facing up.


1. Put the stock on the bed. Try to make it straight and anchor it at least at the corners and midway of the long sides.
2. Change the tool.
3. Turn on the Shopbot.
4. Open Shopbot Software.
5. Hit the blue reset button.
6. Type "k" to open the keypad. 7. Locate the x,y origin. Do this by traversing the tool into place so that it will avoid hitting any of the edge screws but so that your parts will fit on your stock. Use the "zero(s)" pull down menu and choose the zero x and y option with z and a safe height.
8. Place zero plate under the tool (make sure it is flat on the stock) and place the alligator clip on the bit. Zero the z now by going to the "Cut(s)" pull down menu and choosing "zero z axis with z plate.
9. After returning z plate and alligator clip to their home, make sure key is in and turned to the right one click.
10. Load the part file.
11. Turn on Vacuum. 12. Hit the small greet start button on the screen.
13. Hit the large menacing physical green button (not as menacing as the large red button though).
14. Hit OK.
15. You can pause the machine at any time by hitting the spacebar or clicking the blinking STOP on the screen. Hitting resume from there will take you back through hitting the physical green button and having the machine pick up where it left off.

back to main page