Anyone use a CNC router for scales?

[REK Knives]

I'm considering getting the Shapeoko 4. The standard size looks good for my needs. I realize it doesn't have a tool changer so that would have to be done manually.

For those who have experience in this field, how would the work flow go? Fixture sheet, set up tool paths/CAM, then run all the paths one tool can do (for all the sets I can cram onto a sheet), manually switch tools and run all the paths that next tool can do, etc?

 

[HSC ///]

Yes, In general.
What you all mentioned is the “easy” part...
The tooling to hold all your parts/scales is the challenge.

how many parts will your tooling plate hold and how will you hold the scales down?

have you given any thought to this concern?

 

[REK Knives]

Yes, In general.
What you all mentioned is the “easy” part...
The tooling to hold all your parts/scales is the challenge.

how many parts will your tooling plate hold and how will you hold the scales down?

have you given any thought to this concern?

The Standard size has a 17.5" x 17.5" cutting area. So I'm thinking I would just fixture 1 sheet up at a time and see how many scales I can nest.

But you have good points - that's why I'm posting here. I have no experience with CNC at all, so there will be a learning curve. I have a manual mill, and can design anything I need in Fusion 360. But if I need an actual fixture made I will likely have to have a buddy who has a Tormach make it for me (which isn't a problem).

So is my thinking off in this thought process... 1 sheet of scrap g10 underneath actual sheet I'm cutting (so table doesn't get damaged by router bit/end mill). The Shapeoko 4 has T slots so I could clamp that down easily enough. As far as fixturing the actual sheet I'm cutting, I've seen it done with double sided tape, or else I could drill/tap holes easily enough (and even do a quick install of helicoil taps) or else just get some clamps that work with the T slots.

thoughts?

 

[HSC ///]

What kind of volume will you be doing?

I suggest you build once and cry once

I would suggest at least an aluminum base plate and you will need some locater pins

Double sided tape can work surprisingly well on a mill to fly cut something but I think you need more Precision in location and can’t afford any movement

you need a way to Square up the plate and find your 0,0

Although I’m a few years removed from cnc machining, the principles haven’t changed.... if you would like to reach out to me via my website or Instagram I can probably answer a lot more questions in a 10 minute phone call. Hsc3knives

 

[Drew Riley]

I built a 4x4 router and make scales and handles on it from time to time. I'm not yet doing any kind of real "production" per say, but it wouldn't be a huge leap if I needed to I suppose.

Do you currently have any experience with CAM or running a CNC machine? There's definitely a bit of a learning curve, but once you get the basics down, it starts to become pretty straight forward. You'll pretty quickly learn what you can and can't get a way with as far as speeds, feeds, and hold down methods.

Like HSC says, holding and accurately positioning parts is the biggest challenge. It get's even worse when you have to machine a double sided part.

Keeping your machine square is also pretty critical. Stepper motors will often lose steps and cause your gantry to go out of square. Spindles (or routers) can also get tweaked and need to be re-trammed. When making smaller parts, I feel like you get a little more wiggle room with tolerances, but you still need to be aware of how square your machine is.

Buy good collets (+/- .0002) and you get what you pay for with tool bits. Dust/chip control is pretty important also.

 

[TILLER]

There’s a lot of ways to do it. The way I’ve done it for scales is to do two setups. Cad/cam plan all done first.

The first to spot/drill/ream/countersink holes for the handle screws. You can set it up to do all the spots, then all the drilled holes, etc. this step involves several manual tool changes. You could try interpolating holes to save the tool changes. I’ve done this setup by holding material in a vise.

The second setup uses the holes for the handle screws to hold the scales down onto a fixture while profile and contour machining. For this I use a ball end mill. If you make your fixture to raise the scales up, or to give clearance to the ball below the scale bottom height, you can cut the profile with the sides of the ball mill and then go right into contouring without any more tool changes.
You can machine a boss or like a partial height pin with a threaded hole in the middle of it into the fixture to locate the handle material to the holes.

You might face tolerance issues with multiple holes lining up perfectly if you try to do this on a large sheet at one time. I tried it once with a 6”x10” sheet and used two bosses/locating pins for the whole sheet.

I’d also consider trying to do it without a fixture, using tabs, and simple clamps on the perimeter of the sheet.