[jalessi]

JBR,

That is a really nice mount you made.

How much time is the Colt saving you?

Semper Fi,

Jeff...

[John Bear Ross]

Jeff,

Thanks, and Semper Fi to you, too. The adaptor plate was just a piece of scrap 6061 I had laying around. It works.

We'll see how much time it saves me when I get back from ComicCon, and fire it up.

Minibeast,
The bracket should serve nicely. Delrin dust and wax chips will probably settle in the pockets, but they're harmless, for the most part. As to the bracket, it's not my design, but it's a solid piece of kit. K2CNC makes a nice product.

Best,
JBR

[jemmyell]

I know that the donut guys comments were more to troll a fight than actually discuss anything rational, but I thought I'd put another point into the mix;

I do high speed machining of camera parts, often on steel, and with small enough bits (under 1/16") to require speeds that high. On paper it looks like it would work. It doesn't work in real life however.

You can't go over 5% of a bits diameter in runout without trashing it. Even that is pushing it. Runout of .001 won't bother a larger bit, but with small enough bits to require these high speeds it simply destroys the bits.
For bits small enough to require 20k+ RPM, the runout has to be in the tenths. Just not router territory.

Even if a routers runout was only .001 (and it usually isn't) it still won't work for high speed machining of steel as it can't handle tools small enough.

Cameraguy, Precisebits makes some of the finest tools in the industry. Growth into certain markets was being limited by the quality of the spindles. They did some tests and discovere that MANY routers (Porter Cable first) had essentially ZERO runout. It was badly made factory collets causing all the problems. Please look here:

http://www.precisebits.com/products/...h_Colt_Collets

either .0006 or .0004 runout specs are available. Really great for mother of pearl and recon stone (Porter Cable - my applications).

-James

[TDA]

Mr. John Torrez,

I sent a memo via the website, asking for a 3/16th collet to be made in the future for my new Colt rig, so I can use my tooling with that shank diameter. Any chances of that happening?

Best,
JBR

Currently demand for 3/16" isn't enough for a production run. I'm not sure why but we have only had 3 people even ask for them .

You can't go over 5% of a bits diameter in runout without trashing it. Even that is pushing it. Runout of .001 won't bother a larger bit, but with small enough bits to require these high speeds it simply destroys the bits.
For bits small enough to require 20k+ RPM, the runout has to be in the tenths. Just not router territory.

I don't know in steel but we have had multiple customers using a .0156" cutter with at least .001" runout in ebony. As I said I don't know about steel but I would have bet a lot that that would have broken in ebony.

Even if a routers runout was only .001 (and it usually isn't) it still won't work for high speed machining of steel as it can't handle tools small enough.

Goto http://www.precisebits.com/gateways/ColletsNutsHome.htm and click on "Video" under Porter-Cable. Total runout in the router, collet, and tool was .0005"




John Bear Ross:

Let us know how it cuts and what the runout is. I'm quite interested in seeing how the colt does in this setup.

I'm also interested in what you think of the K2 mount. Any thoughts?

Sorry about the 3/16" until we see enough demand for them we can't justify making hundreds of collets.

[John Bear Ross]

Currently demand for 3/16" isn't enough for a production run. I'm not sure why but we have only had 3 people even ask for them .

Let us know how it cuts and what the runout is. I'm quite interested in seeing how the colt does in this setup.

I'm also interested in what you think of the K2 mount. Any thoughts?

Sorry about the 3/16" until we see enough demand for them we can't justify making hundreds of collets.

Not to worry about the 3/16th. It would be nice, but I understand the economics.

I only recently discovered your presence after extensive searching on this forum, though, so it might be a matter of lack of exposure.

The lockup of the bracket to the router body is quite solid. Metal to metal engagement, and with a pocket milled out so the spindle lock button can be pressed while changing bits.

I chucked up a ground .250 dowel pin in my new collet, and set up my old Starrett 196 plunge-back. It didn't waiver, nor did the naked spindle (though there was a thousandths dancing back and forth because of the threads). I'll start making cuts, and will report back.

Best,
JBR

[fretsman]

Thanks for the info JBR. I found some interesting info that all of you will get a kick out of.

James (Leonard), I did indeed check the spindle taper itself when it was new and pretty much dismissed the idea of using it as spindle so it has been getting used as a hand tool for chamfering/ rounding over edges etc. Out of curiousity I went ahead and checked it today and low and behold, it's only out by .0015" and yet still no play in the spindle. None. So now I do not know what happened as the only thing I can come up with is I measured it wrong and I wanted all of you to know.

Looks like I may be doing this mod after all as it might come in handy. Again, thank you JBR for getting me to revisit this

Dave

[TDA]

JBR, any update?

[John Bear Ross]

JBR, any update?

I just did my first test cuts in machinist wax. Here are some notes...

>Cutter used: .125 dia, .750 flute length Atrax 4-flute TiN coated carbide end mill, centercutting (they're on sale right now... http://www.use-enco.com/CGI/INSRIT?PMAKA=ST326-0142 )
>Feed: 15 ipm
>Step-Over: d/7 (.0178)
>Run Time: 25 minutes
>Part size: 1.8 inches wide by 3 inches long by .250 deep
>Stock size: 2 inch wax rod


This cut was for a tank-hull bottom that I do most of my test cuts on. Overall, I've happy, and will move on to delrin next, as well as experiment with smaller bits at higher speeds.

Obviously, my stock isn't as large as my part, but I just wanted to see how it would cut. I initially set the Colt router spindle at 4 for the first half of the cut, and bumped it up to 5 for the second half, just to see a side-by-side comparison in surface finish. Surprisingly, the finish was much smoother at 4 than the higher 5. From the manual...

SETTING RPM
1 16000
2 18000
3 20000
4 22500
5 26500
6 35000

4 is 22.5K rpm, while 5 is 26.5K rpm. Something about that extra 4000 revolutions made the wax heat up and streak, causing a nastier finish compared to the lower setting. The segment of the part done on "4" was very smooth, comparable to a hand-sculpted piece, and I was able to leave fingerprints on it. Not so on the "5" side, which showed tooling marks and a spottier finish.

The pluses of the new arrangement are that the downdraft from the spindle blows off most of the wax chips before they have a chance to re-fuse to the work, which has been a problem before with my wax builds. Also, the Colt performed like a champ. The K2CNC bracket heated up, but that is to be expected on a 25 minute run. The true torture test will be on some of my finish passes that last most of the day. We'll see...

I saw no visible run-out or end-shake by eye, even with the extended length . The precisebits collet and nut held up well for its initial test, even with .250 plunge cuts into wax at high rpm. I'm liking what I'm seeing so far.

Best,
JBR

[TDA]

4 is 22.5K rpm, while 5 is 26.5K rpm. Something about that extra 4000 revolutions made the wax heat up and streak, causing a nastier finish compared to the lower setting. The segment of the part done on "4" was very smooth, comparable to a hand-sculpted piece, and I was able to leave fingerprints on it. Not so on the "5" side, which showed tooling marks and a spottier finish.

Used for aggressive machining of stainless steels, high alloy carbon steels, nickel-based high-temp alloys and titanium alloys.

The tool you listed is a metal cutter which means it's going to have a cutting angle that is less than ideal for wax or plastics. They are more likely to cause melting and have a poor surface finish in plastics or other soft media.

You should be able to run faster with a better finish if you switched to a 2 flute tool designed for soft media. As an example here are some test cuts in HDPE I did recently. The "sweet spot" in these test is where I had a very good surface finish no melting and good extraction of the material.

HDPE

Tool: .1250" x .50" 2 flute upcut
RPM: 20500
IPM range run: 40-180 IPM
Sweet Spot: 165-180+ IPM

Tool: .0625" x .31" 2 flute upcut
RPM 20500
IPM range run 40-180 IPM
Sweet Spot: 145-165 IPM

Tool: .0313" x .13" 2 flute upcut
RPM 20500
IPM range run 40-180 IPM
Sweet Spot: 135-140 IPM

That would cut down your machining time by quite a bit. The only thing that would concern me is that Jeff said he didn't think the Taig could be pushed that fast. I don't have any experience with those machines myself so I don't know if that is an issue. I would still consider it though. Especially since you have the RPM for it now .

[John Bear Ross]

Delrin results are in!

I roughed with a .125 diameter 4-flute end mill at d/5 step/tool paths, 15 ipm, and results came out nice. I did the same with a .250 4-flute end mill, and it hogged out nicely as well, for roughing. Both were at speed setting 1, around 16K rpm.

I then did a finish pass with a .031 diameter ball mill, at speed setting 5 (around 26.5K rpm). Things were moving at 15 ipm. Step/tool paths were at d/9, or .003 inches. Finish and detail are beautiful. Length of cut is only .300 inches on the cutter, though, so I'm limited to that depth for now (per toolpath layer).

Overall, I'm very happy with the results of the spindle swap-out. I'm going to be switching back and forth for stock prep and such, but for fine detail, I like the Bosch.

Best,
JBR

[TDA]

How fast can your machine feed reliably?

[John Bear Ross]

How fast can your machine feed reliably?

I'm doing 15 ipm right now. I can try 20, but past experience says I'll start getting binding and missed steps. I have nothing but time, though, and the work I'm doing isn't production.

I'll try, and report. I suppose I should take a picture or two, while I'm at it.

Best,
JBR

[Jeff-Birt]

TDA - properly configured a Taig can do 100 IPM reliably. There are a few Drive systems for Taigs out there that will barely manage 20 IPM due to a poor selection/matching of components. Take a look at post 14 in this thread: http://cnczone.com/forums/showthread.php?t=84700&page=2, I have my Taig doing 250 IPM, but it was NOT reliable at that speed. Doing 100 IPM was fine, but with a 10K spindle there is not much point.

[John Bear Ross]

TDA - properly configured a Taig can do 100 IPM reliably. There are a few Drive systems for Taigs out there that will barely manage 20 IPM due to a poor selection/matching of components. Take a look at post 14 in this thread: http://cnczone.com/forums/showthread.php?t=84700&page=2, I have my Taig doing 250 IPM, but it was NOT reliable at that speed. Doing 100 IPM was fine, but with a 10K spindle there is not much point.

Jeff,

I assume this is with Gecko 540s, right? What about my aging Xylotex? I'm hesitant to cause a situation that releases the magic smoke from my box or steppers.

Best,
JBR

[Jeff-Birt]

The Xylotex is limited by is basic design (low voltage, type of driver chip). They are great for what they are but they just can't perform as well as the G540. I would suspect that you should be able to reach 15 to 20 IPM though.

[thumper650]

Hello JBR,
How is the spindle going? Was wondering have you cut any aluminum with it yet? And how has it held?

[Fixittt]

John,
Do you have any type of dampening on the steppers? harmonic dampeners? If not then I suspect that your motors are growling something fierce when you are at speed.

Do a search on the zone for harmonic dampeners if you are not using them already. They make a world of difference with your setup.

[John Bear Ross]

No aluminum, yet. Just Delrin and Wax. The Bosch spindle is great on those materials.

And thanks for the tip on harmonic dampeners. I'll have to look at that.

Best,
JBR