Can I use Nomad to cut dowel holes in spoil board?

(Joshua Hume) #1

Using dowels set into the spoil board to line up the work piece for flipping. It came out pretty well! Had a hard time deciding if I should align against the spoil board or the metal transport thing beneath it. Eventually I decided to just use the line I had accidentally carved into the board when cutting out a rectangle, and that seems to have worked. See photo.

But for future holes, can you tell the Nomad to make some dowel holes? Safely, I mean? If so, how?

0 Likes

Workholding for 2-sided acrylic
(Jonathan K) #2

This is actually a bit more complicated than it seems at first—you could program some shallow pockets in and set your z-zero at the waste board surface, and only go say 3/4 of the way through the waste board so you can push your pins in.

But, then you’re putting the holes in relative to the program zero you set, so you’ll need to make sure you also have some way of capturing that program zero for future use. I would recommend doing this kind of thing relative to one of the “rapid” positions on the table (like the very center) and then you’re only adjusting the z-height to the top of your stock, and aligning the center of your fixturing (and your dowel pin-prepped stock) to a known value the machine already knows.

Does that make sense?

0 Likes

(Leith) #3

I’m thinking of doing something like this

that way the work can be positioned in a corner as a datum and locked down with a screw and clamp - piece of deralin with a hole for the screw in it.

1 Like

#4

@MrHume, not only can you drill the dowel holes with the Nomad, but if you ever want to do 2-sided machining with MeshCAM you must do so, to accurately re-register the stock when you flip it over.

This is an area where a little hand-written gcode comes in really handy.

I used 1/8" dowel pins becuse they are easily available, and it is convenient to put a 1/8" drill bit right in the collet. Put in the drill bit and move the axes around to where you want the X-Y zero point of your stock to be. Set the drill bit tip down on the spoilboard. Then zero all three axes.

This little program

G20 G90 (inch units, absolute coordinates)
M6 T1 (define the tool as tool 1)
G00 x0.0000 y0.0000 (rapid over to the origin)
G00 Z0.1000 (rapid down to the “safe level”)
F8 (set the feedrate)
M3 S4500 (turn on the spindle at 4500 rpm)
G00 X0.2500 Y-0.0625 (rapid over to the first hole location)
G00 z0.0200 (rapid down to just above the stock)
G01 Z-0.3000 (move down into the stock to drill)
G00 Z0.1000 (rapid up to the safe level)
G00 X-0.0625 Y0.2500 (more of the same as above)
G00 z0.0200
G01 Z-0.3000
G00 Z0.1000
G00 X-0.0625 Y3.2500
G00 z0.0200
G01 Z-0.3000
G00 Z1.0000 (rapid way up into the air just for the fun of it)
M5 (turn off the spindle)
M30 (end the program)

is what I used to drill the dowel pin holes for my Millennium Falcon attempt. The theory is to offset the holes by the radius of the dowel pin, so when you set the stock up against them, the lower left corner is at X0 Y0. The Z-0.3000 is the depth of the holes, which is not quite all the way through the spoilboard. I used 1/2" long dowel pins so just a little was sticking out. Chamfer the holes before you press in the pins (the MDF will spring back a little and grip the pins tightly) so that the pins don’t bulge up a collar where they enter the surface.

Here is a drawing of the three dowel pins from the sample gcode above, with a representative stock registered against them. This provides a virtual fence along the Y axis and and endstop on the X axis.

When you put the stock down, you just need to re-zero the Z axis using the cutting bit on top of the stock itself. The Nomad will keep track of the X and Y zeros between homings, and in my testing even between power downs, until you re-zero X and Y. The home switches are good to within .001" in my testing, which is well good enough for the belt-driven axes. (Editorial comment–I am very impressed at the level of thought, design, and fabrication that has gone into the Nomad. Every step in the chain is on the equivalent level to every other part, mechanically and electrically)

2 Likes

(Leith) #5

Okay, I will bow to that answer Randy. Very nice. Glad you like the machine.
Definitely agree dowel pins are the best way to go my solution is just a quick and dirty answer.

0 Likes

(David McMillan) #6

Randy… check me on this, because perhaps I’m missing something obvious. But it seems to me that this approach can only work if the dimensions of the stock are very well-known to start with, and the edges are very square all the way around. Without that, I can’t see how MeshCAM would know how the flip had moved the “top” cut relative to the dowel pins.

0 Likes

(Joshua Hume) #7

Thanks for all the help, guys, I really appreciate it!

One thing I’m not 100% clear on is why it’s necessary for the pins and program zero to be related to one another, at least in the case where you have defined the stock in MeshCAM and had it center the object you are cutting.

When I cut this sort of tilted oval shape, all I did was attach the Renshape to the board with double sided tape, and make sure that it was pressed tightly against all three pins. I set the zeros using the method described on this board, of touching the cutter to the edge of the piece and then manually moving it by 1/2 the diameter of the bit.

Once it finished the first side I flipped it (so that the Millennium Falcon did a loop-de-loop, thanks Randy! :wink: ), applied tape to the new side, and again pressed it tightly to all three pins as I put it down onto the spoil board. As you can see it got pretty good results. The only issue I had was a very slight bump in the corners of my oval, but I feel like that’s from the inherent limitations of a 3 axis machine… See photos below.

Did I just get lucky? Or would 1st_Kiwi_Nomad’s method also work, provided you were cutting in the center of stock?

Flipped and pressed against the dowels:

It came out like this:

The limitations of 3 axis milling?

0 Likes

(Joshua Hume) #8

Also, can you please tell me how you chamfer the holes? Is that in the code? Do you just use a tool for this and do it by hand?

0 Likes

#9

@1st_Kiwi_Nomad, your fixture is a very good idea, with the grid of clamp fixing holes and the built-in fences. It addresses something I kind of omitted–holding down the workpiece. As you can see in my Hello Galaxy thread, I drilled supplementary holes in the rawstock outside the machining area and screwed it down onto the spoilboard. When I flipped the rawstock I had to drill more pilot holes in the spoilboard because I just did the hold-down holes by hand. You could actually repeatably mount your jig to the spoilboard using the dowel pins and the fences would be automatically aligned to the machine each time. I will probably run with your idea. Thank you for designing it.

@SkyeFire, yes, this is true. To do 2-sided machining the stock must be as accurate as you say, and the actual measured stock size input into MeshCAM. The workpiece doesn’t need to be accurately centered in the stock though, because MeshCAM will take that into account. MC flips the stock, and the workpiece goes along with it. That is true whether you register the stock to pins, or in 1_K_N’s neat jig.

And of course my comments about the dowel pins above are in the context of machining 2-sided workpieces directly on the spoilboard. The guys at Carbide have developed the flip jig specifically to facilitate machining 2-sided workpieces as shown in the action figure video, without the extra preparatory steps.

0 Likes

#10

@MrHume, we were apparently typing at the same time. First the easy part–I just chamfered the holes by hand with a larger drill bit. The size or angle of the chamfer doesn’t matter, just that the surface immediately around the pins is recessed a little.

But you must have measured your stock and put its actual dimensions into MeshCAM before you generated the toolpaths. That’s the only way it works–both for X-Y alignment and for the thickness. Otherwise there will be an offset between the first side machining and the second side.

Also if the two pins along the Y axis are not accurately along the Y axis, there will be a little angular misalignment between the two sides machining.

I would say you maybe were a little lucky with your job, but as the old saying goes “luck is when preparation meets opportunity” and you created the luck yourself by thinking things through first. :slight_smile:

I find it useful to think through concepts like this, by exaggerating what could be wrong. Say the stock in MeshCAM was 4" deep (in Y) with the workpiece centered in it, and the actual stock was 5" deep. MeshCAM would machinine the workpiece centered 2" up from the near end, but when you flipped the stock the second side would be machined 2" up from what was the far end.

Same with angles. Suppose the two pins along Y were 10 degrees out from straight. The stock is tilted but the machining is straight. When you flip the stock, it is 10 degrees out from straight in the other direction but the machining is still straight. The two sides of machining are twisted relative to each other.

0 Likes

(Joshua Hume) #11

Oh, yes, I forgot to mention that, I always measure the stock with some calipers and input its dimensions down to at least the first decimal. I actually thought you had to do that.

As for the Y axis, I spent a long time trying to sort out how to align that exactly right, and eventually just decided that since the Nomad had cut that line in my spoilboard while cutting a rectangle, it was probably safe to assume that the machine thought that line was perfectly parallel to the Y axis - and luckily for me, it did!

Seems like a mixture of dumb luck and smart luck this time around, but I’ll take any kind of luck, I’m not picky. :grin:

Thanks again for all the help!

0 Likes

#12

You are exactly right. That is the foundation of the method. I measure and enter the stock to the nearest .001" (as close as I trust my dial calipers). And the ends of the stock must be accurately square to the side, at least out to the endstop.

0 Likes

(David McMillan) #13

One more n00b question, Randy, if I could impose – obviously, the axis you flip the workpiece around matters. But is that selectable, or does MeshCAM only flip on one default axis?

Actually, just one more thing, sir (/Columbo). What does the NC output look like? Is it a single NC file, that pauses and prompts you to flip the workpiece, like during a multi-tool cut? Or something more complex?

0 Likes

#14

@SkyeFire, the flip is always a loop-the-loop (somersault…) and not a barrel roll (rolling over in bed…) so the surface against the Y-axis reference (pins or fence or whatever) stays in contact with that reference and the “near” end becomes the “far” end.

On a 2-sided job, MeshCAM calculates all the toolapths at once. You then get an opportunity to view the top and bottom toolpath sets. When you go to save the toolpath, MeshCAM prompts you for a “top” toolapth filename and saves it, and then prompts you for a “bottom” toolpath filename and saves that. So you end up with two individual gcode files that you basically run independently.

And thanks for the Lt. Colombo reference. :slight_smile: I’m usually on the other end of that conversation…

0 Likes

(Joshua Hume) #15

Hey Randy,
I tried to use this code to achieve this task, but when I ran it, during the tool measuring phase it jammed the drill down hard onto the probe and failed. Do I need to modify the code somehow? I looked at the G-code for another toolpath and it seems like maybe I need to tell the Nomad that I’m using a drill bit? I monkeyed with your original code to account for my using a 1/4" bit and dowels. All I did was change .0625 to .125 in three places. Maybe I messed it up? I posted it below. Saved it as a text file, with a .txt extension, Carbide Motion opened it up no problem.

G20 G90 (inch units, absolute coordinates)
M6 T1 (define the tool as tool 1)
G00 x0.0000 y0.0000 (rapid over to the origin)
G00 Z0.1000 (rapid down to the “safe level”)
F8 (set the feedrate)
M3 S4500 (turn on the spindle at 4500 rpm)
G00 X0.2500 Y-0.125 (rapid over to the first hole location)
G00 z0.0200 (rapid down to just above the stock)
G01 Z-0.3000 (move down into the stock to drill)
G00 Z0.1000 (rapid up to the safe level)
G00 X-0.125 Y0.2500 (more of the same as above)
G00 z0.0200
G01 Z-0.3000
G00 Z0.1000
G00 X-0.125 Y3.2500
G00 z0.0200
G01 Z-0.3000
G00 Z1.0000 (rapid way up into the air just for the fun of it)
M5 (turn off the spindle)
M30 (end the program)

Any thoughts?

Thanks as always for your help!

0 Likes

#16

MrHume, I just reran the code (copied and pasted from your reply above just to be sure) and it ran fine. My own code didn’t have the comments (I added the comments as I posted) so I wanted to be sure Carbide Motion wouldn’t choke on them. But the () are the standard format for comments in MeshCAM so I was pretty sure they were OK.

For safety I zero the Z an inch or so up to test run a gcode, so that it will be “air cutting”. That is what I did to test the drilling program, so the spindle could be running and all.

The tool length sensing is an internal Carbide Motion routine called by M6. Carbide Motion doesn’t make any assumptions about the tool, and starts way up in the air to slowly move the tool down to the probe. Maybe a glitch in your probe?

You can test the probe by homing the machine, then when it goes to measure the tool in the spindle, press the probe down with your finger while the tool is still up in the air. CM should stop the spindle movement and retract back up. Of course, after you do that CM will think you have a really long tool installed so don’t try doing any machining after that before re-homing!

0 Likes

(Joshua Hume) #17

Thanks for this @Randy, I ended up just using the spoil board CAD model that @jdunne posted to OnShape, adding my dowel holes to it, setting the machine region to only do the holes, etc. It definitely took much longer than your method, but I was gunshy of the drill bit, I thought maybe it was just way too long, and didn’t want to chance destroying my probe.

I have not had any further problems with the tool probe - no idea what happened there. It’s strange… I don’t suppose feeding Carbide Motion a text file - with an actual “.txt” extension could have caused that problem?

0 Likes

#18

Ah, I forget how long regular “jobber” drill bits are. I have a set of “screw machine” length bits dating from my Sherline days, and the 1/8" bit is less than 2" long. I do have a set of jobber-length bits, but only use them in the hand drill or drill press.

0 Likes