Making your own panels with a desktop CNC

From circuitbending to homebrew stompboxes & synths, keep the DIY spirit alive!

Moderators: Kent, Joe., luketeaford, lisa

Post Reply
nateflanigan
Common Wiggler
Posts: 169
Joined: Fri Jun 19, 2015 4:31 pm
Location: Philadelphia

Making your own panels with a desktop CNC

Post by nateflanigan » Sun Aug 09, 2020 5:41 pm

Hellos,
A month ago when I started researching this I found tons of information and lots of videos on hobby cnc machines but very little that seemed to directly address milling panels for modules, rack gear or pedals with a desktop cnc. This thread is to document my learning process, share what I find successful and what I screw up, and hopefully get some advice on how to better run my machine.

The backstory to this is something surely many of us have thought, since I've got little else to do, I figured I'd finally wrap up some long suffering DIY projects. After designing my panels and getting a quote from FPE I realize "heck I could just buy a CNC for that much money" and so the rabbit hole opens before me.

After a lot of research, asking dumb questions on CNC reddits and forums, the usual hemming and hawing and all that I decided on a Next Wave SD100, 2w diode laser, touch plate and a 0.005" carving bit.

https://www.nextwaveautomation.com/shop ... p198998896
https://www.nextwaveautomation.com/shop ... p114869874
https://www.nextwaveautomation.com/shop ... p121064790
https://www.amanatool.com/45771-k-solid ... 1&fp=12841

The number one reason I went with this package is that I was eligible for employee pricing from one of the distributors which was a pretty great discount. None the less it still totaled up to quite a bit more than the FPE quote, but anyone reading this is SURELY familiar with a simple idea ballooning into a whole room full of synths.
The other reasons I went with this over some potentially cheaper options,
  • the SD100 comes assembled, I just didn't feel like putting the machine together, I didn't want to screw something up, or have it work but have shitty alignment.
  • The Next Wave products come with the Vectric Vcarve software, after messing with Fusion 360 and some open source software I really wanted a complete software/hardware package. Even being pretty good with vector graphics software I feel theres a pretty steep learning curve to most CAD software.
  • Also, I don't have a lot of space so size definitely matters, the sd100s cutting area is plenty large enough for modular panels and pedals, and I think I should be able to do 19" rack panels by doing half then flipping it around and doing the other half.
About the laser, I really wanted to try one, and as best I could tell a 2w laser should capable of etching anodized aluminum, which is all I want it to do. This is the blog post that made me think it was worth trying.
https://jtechphotonics.com/?p=2687
I was also looking at k40 machines too but the ones that are about $300 aren't large enough to do a rack panel and the next size up is a lot more money and a very large tool.

About the touch plate, I consider this essential for setting the z axis. I watched some videos showing how to home the z axis manually which I'm sure works fine if you're carving an 1/8" deep into 3/4" wood since if you're a fraction of a mm off it doesn't really matter. However, being that the goal here is to engrave pretty fine text and line work into aluminum, like 0.05 mm deep, being off by a fraction of a mm is a lot.

About the bit, it's the pointiest bit I could find. There's cheap ones on ebay which I'll try soon but I wanted to start with something good, one less thing to worry about.
Last edited by nateflanigan on Sun Aug 09, 2020 5:52 pm, edited 1 time in total.

nateflanigan
Common Wiggler
Posts: 169
Joined: Fri Jun 19, 2015 4:31 pm
Location: Philadelphia

Re: Making your own panels with a desktop CNC

Post by nateflanigan » Sun Aug 09, 2020 5:51 pm

My goals with this are to engrave or etch text, simple graphics, and pilot divots for drilling. For now I'd be happy to buy blanks, do the engraving then finish the holes on my drill press. It seems that milling aluminum is totally possible on these machines I just don't feel like messing with it yet. I'm mostly interested in 4 and 5u systems, rack gear and maybe some pedals.

So far I've been doing tests on anodized aluminum business cards, I'll post pics shortly.

nateflanigan
Common Wiggler
Posts: 169
Joined: Fri Jun 19, 2015 4:31 pm
Location: Philadelphia

Re: Making your own panels with a desktop CNC

Post by nateflanigan » Sun Aug 09, 2020 6:56 pm

First test, in Vcarve (and other CAD software I've tried) you have to specify the size of text in mm or inches. This text is 4.2mm high which should be about 12pt. The fonts are single line fonts, if you don't know what that means a quick google will explain it better than I can. Suffice to say CAD/CAM handles vectors a little differently than something like screen printing.

Feed rate was 40 ipm, depth of cut 0.1mm. The only tool path I can get to work for single line fonts is called profile cut, Fusion 360 calls the same function the same thing so maybe it's a standard term. Basically the bit just follows the line, you can set the depth but the profile of the bit determines the width of the engraving. Since I was using a V bit the deeper the cut the wider the line.

After making the cuts I lightly sanded off the burrs and used a laquer stik to infill the engraving.

Image

Same thing but with 3.5mm text, I think I reduced the depth to 0.05mm
Image

And 2.7mm text, definitely 0.05mm depth on this one. This one got a little shakey, I have some ideas about why, but need to experiment more.

Image

KSS
Super Deluxe Wiggler
Posts: 3731
Joined: Mon Jan 25, 2016 7:28 am

Re: Making your own panels with a desktop CNC

Post by KSS » Sun Aug 09, 2020 6:58 pm

You've begun a journey filled with -pretty much every emotion you've ever felt. Enjoy the process!

Commercial engravers use nosecones with floating heads for good reason. You can get close with the choices you've made. Still suggest you look at nosecones and floating head mounting. Takes the z-axis 'perfection' requirement out of the picture to a large degree. The nosecone also supports local chip removal. Whether nosecone or not, be sure to address this super important aspect when mechanically engraving. Your MDF is not going to be anywhere near flat enough to get good fine engraving on aluminum. it'll do great Vcarving wood and some plastics.

When you do oversize rack panels, don't flip them around. Slide them along a fence to the new position. If you use X for your gantry movement you'll find the whole thing works better. When you flip you change relationship of the leadscrew threads to your part. In addition to any mistakes making the move. By keeping the leadscrew threads in the same relationship to your part, their errors play out the same on both ends of your panel. Flip the part and their errors are doubled. Use the machine to get the fence in the right place, and also to 'calibrate' the slide along it to the next set of cuts.

J? Macready of Animodule has made some good videos of his panel making process with a machine similar to yours. Check them out. I see them on Matrixsynth, but it's been awhile since he posted a new one. He has a subforum here down below.

Handle the chips -efficient and effective removal!- and pay strong attention to your feeds/speeds. You don't want to cut things twice and its almost worse to be cutting air. Because then the cutter rubs instead of cutting, heat goes up and your lool life is shot. You're better off going a little too fast than a little too slow. Do the math and get it right for chip size.

I suspect before long you'll want an aluminum plate for your table and be cutting holes rather than drilling them. The biggest benefit besides a better working plane -that stays flat- is the ability to use coolants and lubricants.

VCarve's a nice program but Vectric's other less expensive software Cut2D is better for the typical 2-1/2D type work you do for electronics panels and packaging.

Much of what I've said is ahead of where you are now, but it will be good to have it in yor thoughts sooner than later.

Good luck! Have Fun!
Treat utility modules as stars instead of backup singers.
Treat power supplies like Rockstars instead of roadies!
Chase magic sound, not magic parts.

nateflanigan
Common Wiggler
Posts: 169
Joined: Fri Jun 19, 2015 4:31 pm
Location: Philadelphia

Re: Making your own panels with a desktop CNC

Post by nateflanigan » Sun Aug 09, 2020 7:15 pm

Laser testing. The first test I did with the laser was all screwed up, the tool path didn't generate right and the etch came out really light. Once I sort of figured out the deal with the tool path I really overcompensated and made the laser go really slow. There's two tool paths on this one, the top line of text is a single line font using the profile tool path. I wanted to see what happened if I did the same operation as the above engraving but with a laser. The normal tool path function for laser etching is called quick engrave, it basically wants to see vectors that are a closed object, ie a rectangle instead of a line, and it "colors them in" so to speak. The bottom line of text is true type Arial 2.7mm high. What I'm confused about here is if you were doing a larger engraving with a say 1/8" end mill, you can picture that plowing out a big shape, you specify the step over to be some % of the width of the bit, meaning it cuts a 1/8" wide line then moves over 1/16" and cuts another line. This is an important parameter but I don't know what the diameter of the beam of my laser is. I just messed around putting in different numbers until it generated a tool path that looked like maybe it would work. I think I have the step over set to something minuscule like 0.001 mm. I also reduced the feed rate to 20 ipm. I think this looks good but It took about 4 minutes to do this. Also, it's not quite as high contrast in person as it looks in the photo.

Image

nateflanigan
Common Wiggler
Posts: 169
Joined: Fri Jun 19, 2015 4:31 pm
Location: Philadelphia

Re: Making your own panels with a desktop CNC

Post by nateflanigan » Sun Aug 09, 2020 7:28 pm

You've begun a journey filled with -pretty much every emotion you've ever felt. Enjoy the process!
Thanks, I have a two year old daughter so I am familiar with simultaneously feeling of all emotions at once.

That's GREAT advice about sliding as opposed to flipping a larger panel, I sort of had the sense that sliding would be better but that really explains why.

nateflanigan
Common Wiggler
Posts: 169
Joined: Fri Jun 19, 2015 4:31 pm
Location: Philadelphia

Re: Making your own panels with a desktop CNC

Post by nateflanigan » Sun Aug 09, 2020 7:46 pm

On to some graphics.
I generated this dial scale in front design, which makes a single line graphic. The dial on the left is just that SVG file imported into Vcarve then cut with a profile tool path, 20 ipm and 0.05 mm deep. The scratches are because I screwed up a setting, or rather forgot to change it back from the laser settings. Basically I didn't tell the machine to pull up high enough when moving from one cut to the next. None the less, I think it came out very nicely, I'm not sure if it was the slower feed rate or not picking up so high between cuts (obviously it needs to come up a bit higher) but this was definitely a smoother cut than the 8pt text test. I also added a pilot divot to the center, I'd probably go a bit deeper on this next time but it wouldl be very easy to align a drill bit to this.
The dial on the right is laser etched, for this I imported the SVG to affinity designer (my vector graphics program of choice) and added a 1.2 pt stroke to the lines then used the expand stroke (which is I think convert to paths in illustrator). It imported way big in Vcarve, I eyeballed resizing it and made a quick engrave tool path. This took 1/2 hour to etch. I think it'd have looked better with a 1 pt stroke, and I need to figure out if I really need to be etching so slowly, but otherwise it looks really nice.

Image

Image

KSS
Super Deluxe Wiggler
Posts: 3731
Joined: Mon Jan 25, 2016 7:28 am

Re: Making your own panels with a desktop CNC

Post by KSS » Sun Aug 09, 2020 7:48 pm

Measure the width of your NORM line and you'll have the laser spot size at this distance.

Does it raster cut the ARIAL 8PT line or is it doing a mechanical cut style toolpath?

Guessing the latter from your description

What do 6 and 5 pt look like?
Treat utility modules as stars instead of backup singers.
Treat power supplies like Rockstars instead of roadies!
Chase magic sound, not magic parts.

KSS
Super Deluxe Wiggler
Posts: 3731
Joined: Mon Jan 25, 2016 7:28 am

Re: Making your own panels with a desktop CNC

Post by KSS » Sun Aug 09, 2020 7:54 pm

CSx4 over D is your friend. If you have only the one cutter, figure this out sooner than later.
Treat utility modules as stars instead of backup singers.
Treat power supplies like Rockstars instead of roadies!
Chase magic sound, not magic parts.

KSS
Super Deluxe Wiggler
Posts: 3731
Joined: Mon Jan 25, 2016 7:28 am

Re: Making your own panels with a desktop CNC

Post by KSS » Sun Aug 09, 2020 8:06 pm

Don't go deeper with the center divot! Your cutter isn't designed for that. It is NOT an end cutting type design.

You'll be FAR better off using a smaller, less deep divot to locate a center punch. Use the center punch to do what it's designed to do.

Your engraving cutter is tracing little .005 circles and its ability to 'pierce' is limited to the angle of the short 005 slanted segment across its bottom.


Go beyond that slant depth and you're dulling your cutter.

If you're noticing a difference when going negative Z, it's a clue that what I've written above is in effect. The longer the Z travels the more time it has to ramp up speed. Again, an engraving cutter is a single point tool which is NOT designed for straight Z end plunging cuts. It will do fine for the depth of the slant across its bottom. After that it NEEDS to go sideways at least .0035 before going any deeper. 0.005 or really, .008 is better.

This sideways movement clears the middle and THEN you can again go another slant depth deeper.

The reason an .008 move is better than an .005 -which would seem to be enough to clear the middle- is that your cutter is not a right cylinder. It's a taper. As it goes deeper, it gets wider.

I still suggest an .010 divot, which clears the center to the slant depth, and is enough to locate the punch tip. But the best toolpath for your divot if you want it deeper would be to slope sideways into a circle of the *largest* diameter and trace concentric circles -or spiral if your software has that available- to the middle. Then go sidesways one slant bottom depth and circle or spiral back out not quite to the first diameter. Repeat this process to make a deeper than slope-bottom-depth dimpled hole.
Treat utility modules as stars instead of backup singers.
Treat power supplies like Rockstars instead of roadies!
Chase magic sound, not magic parts.

nateflanigan
Common Wiggler
Posts: 169
Joined: Fri Jun 19, 2015 4:31 pm
Location: Philadelphia

Re: Making your own panels with a desktop CNC

Post by nateflanigan » Sun Aug 09, 2020 9:03 pm

CSx4 over D is your friend. If you have only the one cutter, figure this out sooner than later.
That's gonna take me a minute to unpack. This is all excellent information though, thank you.
Does it raster cut the ARIAL 8PT line or is it doing a mechanical cut style toolpath?
Mechanical style, it's treating the laser point as a micro end mill. I don't know what raster cuts are, seems more googl'n is in order.

nateflanigan
Common Wiggler
Posts: 169
Joined: Fri Jun 19, 2015 4:31 pm
Location: Philadelphia

Re: Making your own panels with a desktop CNC

Post by nateflanigan » Sun Aug 09, 2020 9:53 pm

CSx4 over D
Ok, so this equation solves for RPM, and when we talk about RPM we mean how fast the router is spinning right?

KSS
Super Deluxe Wiggler
Posts: 3731
Joined: Mon Jan 25, 2016 7:28 am

Re: Making your own panels with a desktop CNC

Post by KSS » Mon Aug 10, 2020 2:35 am

Yes. Spindle RPM is a first step.

It's a feedrate calculation. First you need the RPM then you need to decide how big a chip each cut takes. That gives you your feedrate. The problem is that often hobbyist level machines do not have enough RPM or IPM to meet the best CS for the materials being cut. CS for most any material you can think of to use is available online at any good supplier selling cutters.

Your engraving cutter has a single cutting edge, so it will have a different result than the same size .005 end mill with teo or more cutting flutes. "End" in endmill is a clue. Many -but not all- end mills will plunge cut in ways your engraving bit can't. Fortunately you're starting with engraving, and there is a LOT of information on cutting rates for typical materials. Your machine looks capable of decent work so these will be guides until you learn for yourself and your setup.

The important parts to understand are the relationships between CS, RPM and Feedrate. So that you know what effect your choices are likely to have on the finished article. Like so many things, you'll be seeking the best compromise for your own systems' limitations. Usually that means you're trying to keep from overcutting -because RPM is more easily had in a hobby level machine than IPM. And since the choice there is to reduce RPM to match available FR, you then fall away from the CS ideal for your material. Overcutting means the machine is making fits and starts as it encounters material then air. Because it hasn't moved far enough since the last cut was taken. So it rubs instead of cuts with the problems I described earlier. Rigidity of everything involved adds more to the mix. Like with making music, sometimes things don't sit well in the mix!

A flexible machine, which yours is, adds the flex into these factors. Flex from the standpoint of the cutter means variable chip size. Said flex may come from the cutter itself, or the spindle runout, linear guides or table flex, or general structure flex. And it actually comes from all of them to varying degrees for all systems. Even the massive Excellon drills used for PCBs in the factories with their 6 or 8 inch thick granite bases.

If you know all this you can make informed decisions about which compromise makes the most sense. It won't be the same for all materials. You can also better understand and evaluate your results for troubleshooting.

Now is the golden time to experiment with these three. Except if the one cutter is all you have, best to use the engraving website info of machines closest in RPM and FR to yours. Until you have more tooling on hand to handle the inevitable mistakes you'll make. Everyone does.

That's why I was frantically typing earlier. I didn't want you to mess up your one cutter because it seemed some of this was still mystery.
As I hinted before, it's a journey filled with all kinds of things. I was afraid you -or your cutter- would be 'lost in the weeds' without knowing how or why that happened. I see so many people just winging it and they don't even realize where the problems they're having are coming from.
Treat utility modules as stars instead of backup singers.
Treat power supplies like Rockstars instead of roadies!
Chase magic sound, not magic parts.

KSS
Super Deluxe Wiggler
Posts: 3731
Joined: Mon Jan 25, 2016 7:28 am

Re: Making your own panels with a desktop CNC

Post by KSS » Mon Aug 10, 2020 2:51 am

Sorry, missed the raster reference. Raster is like back and forth mowing a lawn, or the way a CRT TV scans the screen line by line. Or your computer's printer. Lasers can do this faster than they could cut using vector moves, so it's preferable when you're trying for best throughput. It can also give more consistent results.

Those laser cut personalized wood, glass and plastic doodads you find at tourist spots are cut on a machine that works like a GIANT old school record player. The laser is the needle and a whole large 'donut' shaped tray of parts spins rapidly beneath it as it moves straight line from outer to inner or the other way round. Hundreds of items are all lasered at once. The laser turning off, on, and adjusting power as needed for each bit of each item passing under its path.

As with the lawnmowing or computer image rendering style raster, it's much faster to run in circles without ever stopping or massivly changing direction. Raster at your machine level still has to stop and reverse for each new line. But even that's better -from a production standpoint- than navigating the winding, curves and straightaways of vector cutting. It's F1 vs Indy or NAScar. Go fast, turn left.
Treat utility modules as stars instead of backup singers.
Treat power supplies like Rockstars instead of roadies!
Chase magic sound, not magic parts.

Lemmy
Common Wiggler
Posts: 186
Joined: Mon Oct 24, 2016 1:06 pm

Re: Making your own panels with a desktop CNC

Post by Lemmy » Mon Aug 10, 2020 3:39 am

Thanks for sharing this info and your tests @nateflanigan, this is really useful stuff.

Lemmy
Common Wiggler
Posts: 186
Joined: Mon Oct 24, 2016 1:06 pm

Re: Making your own panels with a desktop CNC

Post by Lemmy » Mon Aug 10, 2020 6:11 am

BTW, have you considered using it for making PCBs?

nateflanigan
Common Wiggler
Posts: 169
Joined: Fri Jun 19, 2015 4:31 pm
Location: Philadelphia

Re: Making your own panels with a desktop CNC

Post by nateflanigan » Mon Aug 10, 2020 7:26 am

Thanks for sharing this info and your tests @nateflanigan, this is really useful stuff.
You're very welcome.
BTW, have you considered using it for making PCBs?
Certainly. It's so easy and cheap to get boards fabbed though that I'm not sure if there's much of a point. Maybe in instances like the yusynth stuff where some one shares a pdf of the traces. I can imagine that if I had my process dialed in it might be as simple as printing a page of paper, which is of course an attractive idea. Also, the dust from fr4 is pretty gnarly so I don't know if I'd want to do that in my basement, I'm sure I'll try it at some point though.

nateflanigan
Common Wiggler
Posts: 169
Joined: Fri Jun 19, 2015 4:31 pm
Location: Philadelphia

Re: Making your own panels with a desktop CNC

Post by nateflanigan » Mon Aug 10, 2020 7:58 am

Yes. Spindle RPM is a first step.
@KSS, OK time for some hand holding, I think I'm misunderstanding some of this data as I'm getting really weird numbers.

Using this calculator and chart...
https://www.daycounter.com/Calculators/ ... ator.phtml

I'm going with an SFM of 280 for 6061 aluminum, cutter diameter 0.005, I get 213,920 RPM. Now my router can't go nearly that fast and looking at the data sheet for the tool all the recommended parameters are based around 18,000 RPM.
https://www.amanatool.com/pub/media/pro ... art-v3.pdf

Suffice to say, I'm totally not understanding how to plug in these numbers.

KSS
Super Deluxe Wiggler
Posts: 3731
Joined: Mon Jan 25, 2016 7:28 am

Re: Making your own panels with a desktop CNC

Post by KSS » Mon Aug 10, 2020 11:29 am

KSS wrote:Like so many things, you'll be seeking the best compromise for your own systems' limitations. Usually that means you're trying to keep from overcutting -because RPM is more easily had in a hobby level machine than IPM.
The numbers are right. That calculator just does the actual exact math instead of the good enough rounding of CSx4. Do that and you get 224K RPM.

I told you your machine wasn't fast enough! ;)

But it's a really good time for you to find all this out. Early. Since you don't have 213 or 224K RPM, the compromises begin.

If the tool company is saying something else, then they're giving you the benefit of them having already made the best compromise for their tools based on their expected customer's typical machine limitations. It's why I made the suggestion to look to them for the best advice. But notice this disclaimer. They understand -and are covering themselves against liability. :
Amana Tool wrote:
Disclaimer: It is important to understand that these values are only recommendations
So what you've learned from this situation is that a tiny bit and typical spindle can't cut aluminum anywhere near its ideal CS. And you can't do much about that without extensive and expensive changes to your setup. Your initial results also tell you that this is not a game ender, as good enough can be good enough.

But it does also mean you need to pay special attention to things you CAN do something about. Like making sure the chips are getting out of the way so they don't make an already less than ideal situation even worse. Hence my focus on chip removal. And maybe using a lubricant -a spray drylube suggested for this case- to ease the EFFECT of the unavoidable rubbing and air cutting. Once you have something besides MDF for a table your options there get wider.

Yes some industrial machines made for this kind of work DO have 240K RPM spindles. 120K RPM is more common. Even they make compromises!

213K /18k= 11.83. We'll call it 12. If you can increase your FR 12X, you can help the situation. ;) But then all the other factors already mentioned come into play. Flex, primarily. And power if your machine uses steppers instead of servos. Because they lose significant 'strength' as they speed up for higher FR's.

So you go back to working from chip load and do the best you can. And there's one more factor you still can control which hasn't been mentioned yet. Cut direction. Climb cutting vs conventional. You'll find that those in the know tend to c'limb cut' aluminum. For the very reasons in this thread. But when climb cutting, you're starting with the thickest part of the chip, and moving towards it becoming thinner through the cut. So you need a stiff machine and adequate power to fully embrace its benefit. Here -finally!- you gain advantage from the small diameter and small cut depth capability of your cutter.
It's likely your machine is strong and stiff enough to climb cut with it!

Conventional cutting starts with the thinnest part of the chip and increases its thickness trhough the cut. Do you see how this can be a problem if you already aren't going fast enough in RPM and FR? The cutter rubs as pressure builds up until theres enough force to begin the cut. Compare it to when you're trying to cut a tomato with a less than sharp knife. Which brings us to the last important thing you CAN control. Cutter edge sharpness.

Because you have all these things working against you, the cutter needs to be scary sharp. And kept that way. That's why I was frantically typing when you were attempting things that were working against a result where the cutter has the best chance of staying sharp.

In the old days, every engraver had the skills and tools to sharpen their own bits. You can still do that inexpensively. But since many in our throwaway and "git 'er done" world now don't, the tool industry has gone the direction of addressing it with special coatings. This increases lubricity during the expected rubbing, and may promote cooling during air cutting. But it also means you lose its benefit when you sharpen a cutter, since the sharpening will have to go through at least one 'corner' of the coating. They're by design intended to be used and thrown away or sent out for sharpening and re-coating.

D-tools like your cutter are fortunately -and also by design!- easy to self-sharpen. That's another compromise decision you have to make. Do yo buy expensive coated tools for their 'better' initial performance? <--Scare quote and underline revealing my bias OR do you buy uncoated cutters and learn to keep them sharp?

As I said from the beginning, it's a complicated Journey.

But one well worth taking.





'
Treat utility modules as stars instead of backup singers.
Treat power supplies like Rockstars instead of roadies!
Chase magic sound, not magic parts.

nateflanigan
Common Wiggler
Posts: 169
Joined: Fri Jun 19, 2015 4:31 pm
Location: Philadelphia

Re: Making your own panels with a desktop CNC

Post by nateflanigan » Mon Aug 10, 2020 3:53 pm

Woo! Thank you KSS for personally writing a textbook for me. This advice is so valuable, I'm sure I'll be rereading these posts for years to come. I have some questions about climb cutting but I want to study up a bit so I can ask as articulately as possible.

Let's side bar for a minute. I'm already looking at upgrades, one that seems very easy is a higher precision collet. Do you think there is any advantage to this? Meaning given the reality of a small desktop machine is the collet really the weakest link?

Also, for chip clearance I've been poofing the bit with air from a compressor while engraving.
Last edited by nateflanigan on Mon Aug 10, 2020 3:58 pm, edited 2 times in total.

nateflanigan
Common Wiggler
Posts: 169
Joined: Fri Jun 19, 2015 4:31 pm
Location: Philadelphia

Re: Making your own panels with a desktop CNC

Post by nateflanigan » Mon Aug 10, 2020 3:54 pm

Since bouncing back and forth between engraving and laser etching lead to some mistakes I'm going to stick to one process for a minute. I spoke to Next Wave tech support this morning, the focal point of my laser is 0.003 inches. Depending on FR and material it can have an "over spray" up to 0.008 inches. Tonight I plan on doing some more simple text tests with larger stepover figures and a some different speeds. While the results I got for the dial look good, it would take several hours to do a panel.

I'll post pictures later tonight.

KSS
Super Deluxe Wiggler
Posts: 3731
Joined: Mon Jan 25, 2016 7:28 am

Re: Making your own panels with a desktop CNC

Post by KSS » Mon Aug 10, 2020 6:50 pm

side bar:
Think about what a higher -or lower- precision collet does for you with your current cutter. It will be different for other cutters. Also depends on spindle -for those other cutters. I don't know what your machine has presently.

Pretend it's a REALLY crappy collet. What is the effect on your single point cutter path through the material? Compare that with a theoretical perfect collet's path, and you have your answer. Hint: I'm not saying perfection is the answer here. Consider what differences exist between the crappy and perfect collet for a single point engraver style D tool. At the point of the cut, what is the difference?

Compressed air is good for clearing chips. Often it and vacuum together are even better because sometimes the swarf from your cut is nasty to just 'poof' into your -and your daughter's- breathing space.

poofing implies sporadic. The cutter is *not* cutting sporadically. Well, it is, but timewise in comparison to poof, poof, it's constant.
Treat utility modules as stars instead of backup singers.
Treat power supplies like Rockstars instead of roadies!
Chase magic sound, not magic parts.

User avatar
Flounderguts
Ultra Wiggler
Posts: 818
Joined: Thu Dec 07, 2017 5:56 pm
Location: SLC
Contact:

Re: Making your own panels with a desktop CNC

Post by Flounderguts » Mon Aug 10, 2020 7:20 pm

KSS wrote:
Mon Aug 10, 2020 6:50 pm

poofing implies sporadic. The cutter is *not* cutting sporadically. Well, it is, but timewise in comparison to poof, poof, it's constant.
This is a good point.

Clearing swarf from an engraving tip needs very little in the way of pressure. I have seen a few desktop setups that use a bit of tubing from a computer fan, or even from the motor fan (a la scroll saw) to clear the chips. Another great way to do this at the desktop scale is using an aquarium air pump, which even comes with tubing.

One of the issues that I have seen with desktop engraving spindles is that as the machine approaches maximum speed (which it seems to always want when you calculate your chiploads and rpms) the spindles tend to vibrate a LOT more. Sometimes (counterintuitively) slowing the machine down just 100-200 rpm can reduce overall vibration, and improve the crispness of the contrast line.
----------------------

Flounderguts

nateflanigan
Common Wiggler
Posts: 169
Joined: Fri Jun 19, 2015 4:31 pm
Location: Philadelphia

Re: Making your own panels with a desktop CNC

Post by nateflanigan » Mon Aug 10, 2020 9:14 pm

Seems like some more info is in order. My spindle (which is a palm router) is the ubiquitous DeWalt 611. Its speed settings range from 16,000-27,000.
Clearing swarf from an engraving tip needs very little in the way of pressure.
Oh, good to know, I assumed a hearty POOOOOOOOF was necessary.

jimfowler
Veteran Wiggler
Posts: 659
Joined: Mon Feb 22, 2016 1:13 pm
Location: New York
Contact:

Re: Making your own panels with a desktop CNC

Post by jimfowler » Mon Aug 10, 2020 9:48 pm

The first "upgrade" I made to my machine was ditching the mdf spoilboard and getting a few sheets of HDPE and cutting them to fit. This allowed me to drill through the panel and run coolant/lube mist that also evacuates chips. Any wet lube is going to ruin your mdf spoilboard in surprisingly short order.

The second "upgrade" was abiding by the tool manufacturer's speeds/feeds and recognizing that I can't do their SFM because my spindle doesn't do mach 9. Adjust your chip load and run those little bits at high rpm. I've found that 20k works well with a 0.125" 30 degree engraver cutting 0.20mm depth.

If you're doing bare aluminum you can use the panel as your touch plate. See attached pic.

To your point re: "performance collets" the total runout isn't that much better relative to decent standard collets (e.g. not ebay junk). I think Harvey Tool advertises 0.003" for their standard ER collets and 0.002" for their performance counterpart. Odds are (and I'm just guessing since I've no experience with your setup) is that there are lots of other places to increase accuracy/rigidity before spending 75 bucks on fancy tool holding.
You do not have the required permissions to view the files attached to this post.

Post Reply

Return to “Music Tech DIY”