ShopBot tips

These are tips for our 4x4' Shopbot:

Speeds and Feeds

Q: What is the conversion from the Shopbot speed to the feed rate in ft/min. For example, in the MS command if I set the x and y to 2.0 and the z to 1.5, what does that translate to in feed rate?

A: The MS command defaults to in/sec (it is possible to change the units but I’ve never seen any software that does that). So setting x and y to 2.0 translates to 10 fpm, and Z to 1.5 in/sec translates to 7.5 fpm

Q: What is the max feed rate of the ShopBot?

A: Depends on bit, pass depth and material. 1.5 IPS (90 IPM) is a good starting point for most use cases. If you are cutting very soft foam you could go much faster but anything over ~250 IPM would lose steps.

If your material is thinner than 0.25 inches you might consider using a spiral down bit.

Q: While moving one of the axis will struggle in spots and lose its position.

A: Our Shopbot cannot tolerate a jog speed of more than 4 inches per second. Reduce the jog speed and the problem should go away.

Q: The Shopbot "Feeds and Speeds" doc talks about "soft plywood" and "laminated plywood". But isn't all plywood laminated by definition?

A: They mean veneered ply, different feeds will leave cleaner cuts.

Q: The Feeds and Speed doc doesn't list any settings for '1/4” Downcut Carbide End Mill'

A: The doc is far from comprehensive. The ideal tool is a 3/8" compression for small projects but the 1/4” Downcut Carbide End Mill is 90% as good for less than half the cost.

Q: What is a reasonable chip load?

A: For a quarter inch bit I generally run a chip load around .010 inch per tooth.

Bits and Collets

Q: I have a 1/8 inch bit but the collet is larger than that.

A: Put the bit in and squeeze the collet in one hand. Try to lightly pull the bit out of the collet, if the bit is in snug, then you can use that collet. Many collets have a range of about 1mm, or 0.04“

Q: I'm looking to make some 6mm slots and was wondering whether to get a 1/4" or 3/16" shank bit. I figure the latter allows deeper contours.

A: 3/16" is getting into fragile territory. Control your feeds and make sure you're checking that the dust is clearing out of the slots. Pause the job periodically and break up any compacted dust with a thin rod; vacuuming it out is a plus. The danger here is not to the ShopBot but that you can easily snap your bit. An up-spiral bit would do better at clearing chips but will produce poorer cut quality.

Q: What are good sources of bits? What should I look for when buying them?

A: Top tier router bits: Whiteside, Amana, Festool. Very good: Freud, CMT, Lee Valley. Middle of the road: Bosch, Woodpeckers. Always buy carbide. 2 flute are better 1 flute because there is only half the wear on the cutting edge. For CNC cutting downcut is recommended.

For 1/8” bits and smaller buy a lot because they will break early and often.

We recommend going with a premium or solid brand for the most used bits and cheap off brand bits for ones you are going to use just one or 2 times.

Air Pass

Q: How do I run an air pass on the MN ShopBot?

A: If you use the special MakerNexus post processor it’s pretty hard to do an air pass. Two strategies come to mind, both requiring a second output of your shopbot code. First, lie to VCarve about the thickness of your material by an inch or two, (e.g. set it to be 2.25" thick when it is really .75" thick) and write a file using the zero-ing post processor. Second choice - create a separate output file (or files) and use the “no-zero” post processor, and manually set Z-zero to be somewhere above the actual surface of the material, run that file and when it is all good run the one with the z-zero code baked in. Anytime I post any tool paths out, I make a folder for auto zero and a folder for no zero. That way if I need to manually correct something on the fly or do an air pass, I just go to the no zero folder.

Toolpaths

Name your export Gcode with the tool name included. Examples: Pockets-inner 1-4 EM; Holes-feature 3-16 EM

Q: Can I output from Fusion 360 to the ShopBot?

A: Fusion has a driver called OpenSBP, which works fine. I used it this afternoon to do a cut, and if my measurements had been more accurate it would have been a Success. You have to do the manual Z-Zeroing for each tool, so having your Origin at the lower left will be Best Practice. Note our ShopBot doesn't have a software-controlled spindle speed or on/off. See this very helpful video: Create ShopBot Tool Paths in Fusion 360 for Plywood

Q: Can I use Fusion 360 to make the tool paths for the Shopbot?

A: Yes. But here's a tip - When importing a tool library, make sure no tool number exceeds 19. Otherwise, you’ll get weird x-offset behavior when you run a program using that tool on the ShopBot (specifically, your x-coordinates will all be increased by 6 inches).

If the ShopBot is the only CNC router you use, you might renumber imported tool libraries with an increment of zero. This will assign tool number 1 to every tool in the library. (If you use other CNC routers which have an automatic tool changer and/or multiple spindles, don’t do this. In that case, maybe import every tool library twice, renumber one of them, and then use the renumbered one on the ShopBot.)

The mechanism that causes this on the MakerNexus ShopBot is a bit involved, but the short version is that Fusion exports parts files that include the tool number (e.g., &Tool = 38) and a tool change command (macro C9) in the file header. The implementation of C9 on the MakerNexus ShopBot computer detects that there’s no ATC, and then it runs the code for the MTC (manual tool changer). The MTC code treats tools with numbers above 19 as belonging to an additional spindle that’s offset from the first. The exact interpretation of tool number is in a comment in MTC.sbp:

'Head 1 (Z) tools are #1...#19
'Head 2 (A) tools are #21...#29
'Drill 1 (Z) tools are #31...#39
'Drill 2 (Z) tools are #41...#49
'Drill 3 (A) tools are #51...#59
'Drill 4 (A) tools are #61...#69

For example, when using a tool numbered 38, the MTC code interpreted it as belonging to “Drill 1”. The MTC then reads the corresponding x,y offset defined in my_variables.sbc and applies the values as a temporary offset using the VO command. It looks like all the offsets are the same (x = 6 in., y = 0).

Unfortunately, the MTC code is the same code that displays the dialogs “Is tool number &tool in spindle?” and “Is Z axis zeroed?”, so it can’t just be disabled.

Troubleshooting

Q: A simple rectangular part I cut out measured about 0.85 mm longer and wider than expected. Meanwhile, the dado slots I cut into the face of said part measured about 0.4 mm narrower than expected.

A: There are three issues that cause dimensional inaccuracies, the most common is running the Shopbot too fast. It is an open-loop system so it has no feedback to say that it missed steps. The 2nd is errors in the translation from the drawing to the Shopbot part file; I would inspect the file and see if the dimensions seem correct. The 3rd is setting a bit diameter that does not match the physical bit; I would measure the bit to insure it really is 1/4”

How To Zero

Q: What is the Shopbot zeroing process for Fusion360 files?

A: Short version (easy way). Set your origin In Fusion to the bottom of your stock, at the lower left corner. Use C3 to zero the Shobot’s X and Y. Load your part, and the cutting tool. Move the spindle to X=-2, Y=11 and then use the C2 function to zero the tool TO THE SURFACE OF THE TABLE. run your file. clean up the mess. Watch video's numbered 4 and 7.

Tips

Goto: Avoid doing x/y and z gotos together. It's hard to visualize the path and your bit might crash into your work.

Break up your part files into one bit per file. This makes it easier to troubleshoot each one.

Best practice is to place your Z zero on top of your material. Also, if you can, place the Z-zero close to each cut so that you don't have to rely on the tram of the Shopbot to be perfect across a long distance - and it helps when your material is not perfectly flat.

Q: How can I do inlay with the Shopbot?

A: This is one of the great features of V-Carve software. Use a 90-degree V-bit to cut the positive image into the base, and use the same bit to cut the mirrored image protruding from the inlay wood. The depths of the two are set such that when the protruding part is set into the cavity, it forms an exact fit but with a ~.1” gap between the remaining flat sections of the pieces of wood. Glue is put in the recess and the parts are clamped together. After drying overnight, a bandsaw is used in the gap to separate the pieces, then the face is sanded. The result is a perfect inlay. There’s a good video showing the technique on YouTube