High-speed spindle experience for engraving?

[ucdwino]

Hey All,

I just bought a used series 1 1100 for my company. We will be primarily using it for making steel dies for forming caps as well as for making brass embossing dies to form winery logos into the top of a wax disc that sits on top of the cap.

There is an illustration here that might help show what we are doing.

I just bought a used air turbine spindle to do the detail work for the milling of the molds for the top. That part is 3/4" in diameter and I want to be able to give as detailed a decoration as is possible (many wineries have elaborate logos)

We are going to be engraving those logos into a 6x6" brass plate in a 4x4 matrix so that we can press 16 at a time (this is still a prototyping phase for us - so yes it is going to be slow)

I have a few questions about using this spindle in this application.

1) cutting tools: is there any advantage to getting cutting tools with a thicker shank? I have noticed that from the online shops, you can get an engraving tool with the same size end, but with shanks from .125" to .25". I am imagining that if I'm running the thing at 40k RPM, heavier tools might not be better for accuracy, (especially with a single tooth cutter that I figure is not balanced) but I'm also concerned about snapping them...

2) is 40k RPM overkill given the speed limitations of the tormach? 40k is at the slow end of the range for spindles like this, but I have also noticed that the Tormach speeder only really gets you into the neighborhood of 15k rpm. I'm wondering if I'm making a newbie mistake thinking that 40k will help me.

I have based my assumptions that 40k is right based on the online videos of Datron machines which and run in that range. - their feeds are probably faster, but I dont think by much. I want to use as narrow as a 0.010" tip with a 30 degree included angle and get a good finish, so I'm assuming that 40k isn't overkill... am I wrong there?

3) DOC. Can anyone recommend a good starting depth of cut for brass when running these tools at those speeds? Some of the videos that I have seen show a pretty aggressive cut. - basically one pass. I have broken my fair share of endmills in learning this stuff on my sherline at 10k rpm, so I'm wary. I also do not have much of a sense of scale for what is happening in those videos. I cant tell if they are cutting down to .02 inches, or .002 inches..

4) The spindle I am getting has a .75" shank. I do not think I am going to use a variety of bits in it, so I'd like the ease of TTS tool-table setup so that I can swap the tool in after I finish roughing the mold with larger tools.

At .75" I can use a R8 holder that I already have, but I think this tool is also a candidate for conversion to a TTS tool using their conversion kit.

Is there any advantage to using the R8 over TTS for this application? Has anyone done that conversion and are there any drawbacks to it in this kind of application?

Any guidance would be appreciated!

Thanks, and cheers!

Tim Keller

Similar Threads:

• High Speed engraving attachment??
• High Speed Spindle - Engraving
• Oddity with high speed engraving
• LOOKING FOR HIGH SPEED ENGRAVING MOTOR
• Engraving with High Speed Spindle

[zephyr9900]

Tim, I can't answer all your questions but can give one datapoint.

I have the Proxxon auxiliary spindle that Tormach sells. I did replace the nose bearing with a hybrid ceramic bearing from a shop in Australia.

The attached photo is of some small model railroad wheels I machined last year. The pockets between the spokes, I machined with a .009" 2-flute carbide endmill. On the four large pockets, I did rough with a .020" endmill, but the six small pockets were entirely the work of the .009". The wheels are nickel silver (a little tougher than typical brass) and I ran the .009" endmill at 20,000 rpm, 1.3 ipm feed and .002" depth per pass. The depth of that operation was .040" (i.e. 20 passes). I did use flood coolant.

The endmill survived machining two wheels, then I snapped it off attempting to re-measure the length with my dial height gauge...

According to Machinist Mate software, the .009" 2-flute should be turning 170,000 rpm in brass with a feed of 10.9 ipm. I just ratioed the feed down to suit my 20,000rpm spindle speed. With 40krpm you'd be able to double the feed.

There's some more description of the machining in this thread here on the Zone.

Randy

[ucdwino]

Thanks for that info randy, I am really relieved to see that kind of resolution coming from the tormach.

I have already broken a number of engraving bits MUCH larger than .0009 while learning on my sherline. But I think that is because of Z-axis slop on that machine. .002 too far down with a .001 diameter point is a big deal.

I am assuming that the tormach is more repeatable in Z than that.

I got this particular spindle so that I could use the TTS system and set the tool height offline. I just don't trust myself to touch-off a small cutter without snapping it. I also like that it is concentric with the main spindle.

Any reason to believe that TTS height repeatability isn't fine enough for this application? (assuming my spindle nose is clean )

I have seen people talking about how DOC should never be more than 50% of the tool diameter, but it looks like you kept it below 25%. (which makes sense for delicate tools) would you think that is a good rule of thumb? Also, what % stepover would you reccomend? Given that we are making molds, I am guessing that I want to be below 50%...

Again, thanks for your help!

[BlueFin]

The attached photo is of some small model railroad wheels I machined last year.

Randy

Jeeez Randy where have you been? If I ever get around to it I have a 2.5" diameter train wheel to machine for my son. I'll post some pics when it's done.

Tim, I have found there to be .001" to .0015" of backlash in the Z axis, but it should be tight, I think the book said that of you took the Z axis ball screw out of the machine it should require 80 Lbs of weight on top of the head to overcome stiction and begin to move down. Just always machine from the same direction.

[ucdwino]

Think that it is worth turning on mach 3's backlash comp for that amount of backlash? My hunch is no, but I'd be interested to hear if anyone does.

[BlueFin]

Think that it is worth turning on mach 3's backlash comp for that amount of backlash? My hunch is no, but I'd be interested to hear if anyone does.

You have to sign a waiver at Tormach before you can use Backlash Comp, they don't want to assume your liability for using the software compensation. If you are milling 3D surfaces then there will be a height error in your finished part due to this mechanical error. If you can live with that then it's no worry....

[zephyr9900]

Tim, the little pockets on my wheel were full-width cuts for the start of each pass, but yeah, I'd keep it to less than 50% stepover if I had a choice. You only get to snap each bit once... In my testing the Tormach is depth-repeatable to better than .001" and I personally wouldn't try messing with backlash compensation in Mach. I came from a Sherline background too and bought the Tormach when I got tired of tweaking the Sherline more than I was actually making parts with it...

It's not quite your application, but one of the first things I ever machined on the Tormach was engraving a wine stopper, done on Christmas Eve for a stocking stuffer for my wife. I did it with .031" ballmill in the main spindle in stainless steel. 4500rpm, .005" DOC for 3 passes to .015" total depth.

Bluefin, my own Tormach is sitting on a pallet in the new garage after we relocated from California to Texas. It will be a while before I can get the house's electrical service upgraded (I need a new breaker box--the current one is a 125-amp and every single slot not already dedicated 220V for stove etc. is already populated with tandem breakers)

Randy