Questions on getting the best on this CNC cut baffle

[saabracer23]

I’m about to cut my first baffle on the CNC and thought I’d get some input for those who have been to this rodeo. I plan on using a standard 1/4” bit to cut all three driver cutouts and the tweeter recess. For the mid-woofer recess I was wanting to use a smaller bit to get the corners as sharp as possible. I have .125 and .063 available, but don’t think the .063 will be big enough to clean out the rest of that recess pocket. It would be nice to cut the perimeter of the recess with the small bit and clean the rest out with a bigger bit, but can’t figure that out. Does the .125” cut the corner sharp enough? I’m sure I’ll have a few practice baffles cut first. Thoughts?



Thank you
Dan

[philthien]

The smaller bit will work, it will just need to take more passes to clear the rest of the recess.

BUT, in a production (factory) environment, it is likely they'd make-do with a .25" bit.

[craigk]

I’m about to cut my first baffle on the CNC and thought I’d get some input for those who have been to this rodeo. I plan on using a standard 1/4” bit to cut all three driver cutouts and the tweeter recess. For the mid-woofer recess I was wanting to use a smaller bit to get the corners as sharp as possible. I have .125 and .063 available, but don’t think the .063 will be big enough to clean out the rest of that recess pocket. It would be nice to cut the perimeter of the recess with the small bit and clean the rest out with a bigger bit, but can’t figure that out. Does the .125” cut the corner sharp enough? I’m sure I’ll have a few practice baffles cut first. Thoughts?



Thank you
Dan

Dan, look up a Dogbone cut. Should find it on youtube. If not call me.

[saabracer23]

Dan, look up a Dogbone cut. Should find it on youtube. If not call me.

Thanks Craig, what on dog bone am I looking for specifically? I’ll give you a call tomorrow, Laina is going in for a small surgery and will be down for a bit so I’ll have some free time.

The 1/4” bit cut quickly, but when I changed to the 1/8” bit it cut much slower. I’m thinking I may have accidentally set it to cutting aluminum instead of mdf. It was taking very shallow passes. It took about 2-1//2 hours to cut each recess of the woofers.



The 1/8” bit cut the corners beautifully. I just need to see if I can adjust the feed rate. The program Carbide Motion has an odd tool change method. It pauses to let you change the tool, but one you do you can’t zero the z axis before you start again. So you need to make sure your new tool is sticking out the exact same amount. So it would be better to cut the entire thing with an 1/8” bit. Tomorrow I’ll do the entire thing with a 1/4” and see how that looks.

[saabracer23]

As you can see in the photo below the drivers don’t quite fit. I’ll need to make slight adjustments tomorrow. The tweeter magnet won’t even go through he cutout. I went by the measurements on the PE product page (Dayton RS28A).



Dan

[philthien]

First I'd measure my baffle and compare to the CAD, to make sure I'm getting what I'm drawing.

I'd think ideally you'd want holes/recesses in the baffle to be about .02" larger than the actual driver, to accommodate slight variances in the shape.

[Erich H]

If those are the same woofers used in the Jeff's Continuum speaker, then that would explain why they don't fit. Those woofer frames vary a bit from woofer to woofer and run to run. Not just that, the roundovers on each corner can be a little different.....meaning not symmetrical....on the same woofer frame. Sit two woofers up next to each other and you'll see the variance around the edges.

[ohaple]

I use the same shapeoko and carbide process you do. We never use anything besides .125" or .25" for milling out the material. We will use v-bits and ball-nose for carving 3d details though. We are novices when it comes to CNC, so we do not do the feeds and speeds as efficiently as possible. I think we usually use just under half the mill's diameter for the stepover and half the mill's diameter for depth. I think we use about 70ipm on the .25" bits and 50ipm on the .125" then use the carbide speed tool to speed up or slow down as needed. It looks like you did a nice job. We have not used the stop to change bits function, and instead treat them like two separate jobs so we can re-zero Z. I am sure there is an easier way, but it has worked well for us so far.

It sounds like Craig and Erich will be good resources, but I am also available to lend my limited knowledge, just @ me or PM me to make sure I see it. Using the CNC is addictive, and we now use it when it is completely unneeded, like cutting the rest of the box. We also use a laser cutter for some parts to make custom felt gaskets, overlays, etc. You can see our whole CNC-only build here: http://techtalk.parts-express.com/fo...theater-system

Here is a good chart that we found useful when trying to dial in our feeds and speeds, since we tended to run feeds too slow and speeds too fast when we started:



Dog-boning is usually done to allow a square part to fit into a slot cut by the CNC machine. Since the CNC cannot cut square corners, you either need to file or chisel out the corners, or use some sort of dog-boning to cut the slot larger than the square part, so it actually fits. This article explains it well, and also gives tips for minimizing the visual impact. I do not see why you would need to use dog-boning on this part though. http://fablab.ruc.dk/more-elegant-cnc-dogbones/

[saabracer23]

First I'd measure my baffle and compare to the CAD, to make sure I'm getting what I'm drawing.

I'd think ideally you'd want holes/recesses in the baffle to be about .02" larger than the actual driver, to accommodate slight variances in the shape.

Thanks for the tip, I measured and the machine seems to be dead on. I noticed some time back that the Aurum Cantus woofers aren’t made to exact specifications. I just made adjustments in Carbide Create and scaled them up by 1.01. They were extremely close to fitting so we’ll see how that goes.

Dan

[Mike220]

I have come across this when i first started using my machine. There can be a few factors.

1) the bit is not exactly 0.125 or 0.250 (i use 0.245-0.247 bit diameter) because the shank is 0.25 but after they mill the flutes in its slightly smaller.

2)driver variance

3) always add a few thousandths to the pocket cuts (0.005 to 0.018) seems like alot but even 0.018" is not much at all. (The cnc is cutting just on the inside of the line for a pocket so at best case you end up being the exact size of the object your trying to recess. Which is just enough for it not to fit. You can test this but by using the same shape and cutting 3 tasks an OD profile, an ID profile and a pocket then you can measure them all and see what the slightly/marginal difference is.

4) its possible the cnc is off a few thousandths (or maybe just one axis is off a few thousandths). I have a multi-edge finder (touchplate) for my machine which allows me to find a corner of a workpiece and also set the bit height and EASILY hit the same height with different bits. This means i can go back and recut a project when ever needed. Also, once your x and y zero are set never change it if the part hasnt moved and dont change it with a new bit just the z height
zero.

cncrouterparts version (which i am am pretty sure they stole the idea from bill griggs just added the spring feature. http://www.cncrouterparts.com/auto-z...ate-p-288.html

bill griggs triple edge finder http://www.themakersguide.com/home/p...-edge-finder-2

[Mike220]

Oh, i always load the outer diameter profiles i to a seperate file so if the driver doesnt fit i can just tweak it and load the updated file. Then i also make a OD profile file called an "onion skin". You can either cut 95% of tbe way though the material with a slight offset of a few thousandths then have this file make a full last pass at full depth but without the offset to save some sanding on the edges so you dont see the depth marks. Or i mainly use it incase i dont cut all the way though in a spot or two from the dust packing up in the groove so i load this file and it does a final pass.

[saabracer23]

Thanks Mike, I actually really need and want a touch plate. Is there any reason to buy the more expensive one over Bill’s? My issue was definitely with the drivers. Especially the Aurum Cantus woofers, all off them are slightly different. I finally got it though, I scaled up all of my openings by 1.003 and all of the drivers are a friction fit except for one that drops right in and out. I just wanted to make sure there wasn’t any gap which is what I got. I hate gaps lol. I first cut the entire baffle with a 1/8” bit and It took 6 hours!!!! I wanted the sharp corners though. I then cut the baffle again with a 1/4” bit and it took about 17 minutes. Just as sharp lol. Below are photos of the baffle cut with the 1/4” bit.





Dan

[saabracer23]

Thanks Mike, I actually really need and want a touch plate. Is there any reason to buy the more expensive one over Bill’s? My issue was definitely with the drivers. Especially the Aurum Cantus woofers, all off them are slightly different. I finally got it though, I scaled up all of my openings by 1.003 and all of the drivers are a friction fit except for one that drops right in and out. I just wanted to make sure there wasn’t any gap which is what I got. I hate gaps lol. I first cut the entire baffle with a 1/8” bit and It took 6 hours!!!! I wanted the sharp corners though. I then cut the baffle again with a 1/4” bit and it took about 17 minutes. Just as sharp lol. Below are photos of the baffle cut with the 1/4” bit.





Dan

[Mike220]

I think they both accomplish the same thing. I thought bill griggs does one or two things the cncrp unit doesnt. I bought mine from cncrp because i have their machine and electronics package so it was plug and play for me. I liked that if you drive a bit into it you have a second to stop the machine and the inner peace is spring loaded so you dont chip a bit immediately. Its not 100% necessary but atleast a z-axis touchplate is a must. It makes bit changed pretty effortless setting the same height.

[ohaple]

The baffle looks good. If the 1/8" bit took that long I would worry that you have your feeds and speeds off. I could have the math wrong, but double the diameter can cut 2x as deep, 2x more stepover, and faster IPM I think, resulting in maybe a 4x-8x difference on pocketing operations and maybe 3x-4x on profiling operations. Even with 3d contours, our 1/8" cut baffles end up all under an hour.

Regardless of how you got there, that is a very nice looking baffle. Very good tolerances all the way around.