Cutting Parameters for Small Slotdrill

I'm in the process of re-designing the regulator mechanism for my traction engines, I need to reproduce a cover with a 0.4mm deep recess that contains raised lettering; the original would have been cast. It's simple to draw and in theory to use the CNC mill to create the recess and lettering.

However, the small scale of the lettering means I need to use a 0.5mm slotdrill. I've used 1mm endmills and slotdrills before for engraving and gear manufacture, but not as small as 0.5mm, nor in steel.

I'll be running the cutter at 24000rpm, but the question is what chipload would be advisable and what depth of cut and stepover should be used. I've got some values for the parameters in mind, but what does the panel think?

Andrew

I'm not wishing to belittle your question, but the answer is surely that it all depends...

How stable is the set-up, particularly as far as high-frequency, small amplitude vibration goes? What material is the cutter? What does the manufacturer's data sheet suggest (then reduce it)? Does it matter how long the job takes? Does tool life matter - from a wear, rather than breakage point of view? Can you ensure there's no significant chip re-cutting? I guess the real-life answer, for a one-off job as opposed to production, is to be pragmatic and to suck it and see. Probably best to buy a spare cutter. Or two...

Does the maker not give any indication ?

Looking at the couple of catalogues I have here they only give data on the 2-flute cutters for slotting eg full width cuts which may not suit if you are rest machining and using the sides. But if any use for a 0.5mm 2-flute speed is 36K, feed 105mm/min, chip load 0.001mm and DOC 0.15D. That's for a YG-! 4Gmill in non alloyed steel.

One other thought, could it be milled into say 1mm easier to cut brass sheet and then soldered into a recess in your steel cover plate?

Edited By JasonB on 15/03/2020 10:04:30

How about using a tapered engraving cutter, on the lines of Taylor Hobson engraving cutters, I have used them for similar jobs with good results, for your cutter I would step over 35%, depth of cut about point one mm and 65 to 70 mm min feed.

Andrew, if you go along with Baz's suggestion, I think I have some Gravograph 1/8" in my workshop, please PM me if you are interested. I have used successfully for doing brass relief lettering.

Can't check at the moment as I had an eye stroke 2 weeks ago and are struggling with severe double vision, and the workshop is out of bounds at the moment!

If there is raised lettering, as already said, a tapered cutter will give a more true to cast appearance.

Will you use air blast to send the chips away?

I wonder if a ball end mill would help in this situation.

APT seem to have a good price at the moment for cutters of this size.

Jason asks: Does the maker not give any indication ?

Jason, you clearly have never bought anything from e-bay.

My comment about the raised lettering is that it may be that the easiest way to get a plausible scale result is to use etching. With a laser printer to produce letters at the required size, but mirror-image, these can be ironed onto the clean flat metal. Then you add a surround created using varnish, or shellac in alcohol, etc, and an acid suitable for the metal in use. Some people prefer electrolytic methods, using a salt instead of acid and relying on elctricity to do the work. I'm sure a back issue covers this, but when ... ?

Regards, Tim

I doubt very much if Andrew is buying from an unknown e-bay source but it can vary from maker to maker so just wondered what Andrews brand suggested.

Andrew you might try contacting Edward to see what was used to do those nice 6" scale nameplates he had, though material was different the guy that did it may be able to give some ideas of what was used in the router. TT post

Edited By JasonB on 15/03/2020 20:00:54

In my working life as a toolmaker in the mould making industry I have done a lot of engraving. This included 3D type of work in the days before CNC on an Alexander GK21 Deckle clone machine. Does anyone remember the original Cadbury "Old Jamaica" chocolate bar ? I did the mould for that. Cutter was hand made 30 degrees a side D bit with a slight flat on the cutting edge. Speed unknown just as fast as the machine would go and a 3 thou step over because it was the minimum the machine would do with it's ratchet type feed engaged. For the final finishing I did check the size of flat on the cutter tip on a shadowgraph. Depth of cut around 2 to 3 thou.

Edited By Chris Evans 6 on 15/03/2020 21:18:48

That sort of response always dampens the spirits, as it usually means the speaker is probably going to do exactly what they claim not to be doing.

I have no idea about high frequency vibration, but the high speed spindle has made a good job of machining so far with small cutters without breaking any. While I have some high end professional accelerometers I'm dis-inclined to muck about making a charge amp. Been there, done that and it's non-trivial for large signal bandwidth,

I have a golden rule for buying cutters. If I buy two I don't break the first one. If I only buy one I break one, usually on a Friday evening.

Andrew

Thanks for the replies, plenty to think about. To avoid confusion this is the current CAD model of the part:

For scale the width of the part is 3/8" and the lettering is 0.08" high. Material is low carbon steel.

The supplier I was looking at was Drill Service, about the same price as APT and a quarter the price of the YG cutters from Cutwel! Sadly Drill Service don't provide any detailed cutting parameters. I found something from Harvey Tool where, for a 0.015" cutter, they recommend a chip load of 0.00009" with a depth of cut of 1D and radial cut of 0.13D for finishing in steel. They seem quite agressive depths of cut. Out of interest I looked back at my CAM files for the governor bevel gears (1mm ballnose in bronze) and the smokebox nameplate (1mm endmill in engraving brass) and I ran both cutters at 24000rpm and 350mm/min.

I'd thought about engraving cutters, but assumed they wouldn't be good for raised lettering; is that a misconception? Special thanks to Adam for his generous offer, which I'll keep in mind as I decide which way to go. I have some engraving cutters from Arc but they have a sharp point unlike the Taylor Hobson ones.

I had rather assumed that I'd need to pocket out most of the metal with a larger cutter and use the small one to re-machine just the detail. But oddly the CAM system doesn't think it'll take long to do the whole thing with the small cutter. Likewise using a tapered cutter and V-carve was suprisingly quick.

As an aside I use a program called NCPlot to sanity check my G-code. Run times are normally quite close to the CAM program estimate, and a bit more accurate. Today I've been CNC milling and drilling the valve chest covers. The CAM program thought each one would take 40 minutes, which I finally got down to 30 minutes by tweaking parameters. NCPlot thought it'd take 14 minutes, which it did. Not sure why there's such a big difference, although I don't normally do a lot of CNC hole drilling. So may be the CAM has it's knickers in a twist over drilling?

I run flood coolant on the CNC mill so getting rid of the chips shouldn't be an issue.

In the picture I have of the regulator on a full size engine the definition of the lettering is fairly poor, so may be I shouldn't try too hard!

Andrew

Andrew. Oh dear, I really didn't mean to dampen anyone's spirit. I understand your reaction, however: it's probably a bit like mine, when faced with anyone starting with "With all due respect", only I'm angry.

I was worried that my comments could be interpreted negatively, so included the opening words to try to prevent that. This forum is read by people with a wide range of skills, knowledge and, it seems, willingness to think. From your extensive previous posts, it's clear that you are highly experienced, knowledgeable and a thinker. However, others aren't. Mainly for them, I thought it was perhaps useful to suggest that apparently simple questions may not be so simple, when their ramifications are considered, and that following someone else's recipe may not be the best course. Clearly I failed. Sorry. And if I've stuck my foot in it again, I apologise again.

Edited By Kiwi Bloke on 16/03/2020 05:32:07

Edited By Kiwi Bloke on 16/03/2020 05:36:57

Taylor Hobson did their taper-shank cutters in a range of widths, but I cannot currently find the vintage chart that I have put ‘somewhere’

‘Pantograph Services’ lists an even wider range, including plain shanks, on several PDFs **LINK**

http://www.pantograph.co.uk/engraving-cutters-diamonds.htm

It’s worth browsing those pages, and perhaps contacting them for advice.

MichaelG.

Idle pondering here:

Andrew is planning to use CNC and 24,000 rpm ... but traditional Pantograph engraving machines used much lower speeds.

Does the ‘micro-manipulator’ characteristic of the pantograph provide a delicacy of touch which is lacking in powered feeds and which allows the operator to intuitively balance speeds & feeds ?

... or did they just do a great job with the available tools ?

MichaelG.

If you use the pantograph to engrave at a significant reduction, you are tracing the copy with a large mechanical advantage, so it's less sensitive than 1:1. Also, the proportion of a single-lip cutter which is shank is much more than a slot drill, so much stiffer for the same diameter. The proposed 0.5mm dia. slot drill will be about as stiff as an excited gnat's whotsit. I thought the spindles gould go at impressively high rpm...

.

Mmmm : That’s an interesting different perspective ... and I’m sure the truth must lie somewhere between our interpretations.

Micro-manipulation isn’t really about mechanical sensitivity, because [unless it’s artificially contrived haptic feedback] there is none discernible ... it’s more about the operator’s ability to produce tiny movements of the tool with ‘human scale’ [i.e. relatively gross] muscular inputs.

MichaelG.

.

http://microscope.database.free.fr/520_files/520-8c%20leitz%20micromanipulator.pdf

Edited By Michael Gilligan on 16/03/2020 08:53:35

I do. I'm glad to see that you didn't "knock it all back at once"

(sorry Andrew),

Rod

.

They could ... but 18,000 rpm was about the maximum, and I’ve seen much lower speeds used for profiling work.

Hopefully Chris can enlighten us.

MichaelG.

I have been engraving on and off for around 50 years. Started with a Gravograph IM3, and within a year purchased a larger model which had ratio's from 1 to 1 up to 1 to 8, and purchased a computer model when they became available. My sons run the business now, we still have a IM3 a 10 year old computer Gravograph machine which get some use but most of our work is done on a Trotec laser machine these days. We also have a Gerber Dimension CNC router we have had for 25 years!

In my workshop I have my own Gravograph IT4 cup engraver, an ongoing project, which now looks like being abandoned due to my eyesight problem. Anyway to get to the point, it has a 3500rpm motor on it, but it a slightly smaller pulley on the head, so the cutter will be going a little faster. It appears to be the same motor as fitted to the manual machines.

Andrew, yes I have got some 1/8" cutters, and also some 11/64" which fitted one of our original machines, if you decide to go along that route. They are from Pantograph Services who we have used for years.

I can confirm Max spindle speed on a Taylor Hobson Model K engraving machine is 18,000 rpm, used one for many years but now sold on.

Emgee