tool diameter minimum recommendation

I am currently testing out tool compensation on the various machines in our shop. All 3 axis routers cutting hdpe plastic. (Shop Sabres, Onsruds, Multicams).
Our context doesn't require us to hold tight tolerances (compared to metal fabrication), but I would like to extend the usage life of our cutting tools after resharpening. Historically, our shop has used our .5 diameter cutting tools until they are resharpened below .480. Then we dispose of them. But if it makes sense practically to use tool compensation in order to use these tools longer, I'd like to.
My question is about the tooling: How thin of a diameter can I use a .5 tool (carbide 3-flute rougher, carbide 2 flute upcut spiral finisher) before it is too thin? Theoretically, it seems I can go a lot thinner than .480, but will the tool be compromised at some point?
Any thoughts?

Your limiting factors will be the flexural strength of the cutter vs cutting forces, and the size of the gullet for holding chips (which will shrink when the cutter is sharpened.) If the cutter loads up and starts melting the material, or breaks, then you've gone too far. This can be compensated for by cutting slower, but that costs money.

You should also be aware that the smaller diameter effects your SFM/RPM calculation; ideally you'd spin the .480" cutter faster than the .500" one.

As small as they make cutters..3/8 and 1/4" common with the speeds and feeds right for the size.

Yes, flute depth. losing flute rake angle needs to be considered.

Having a dozen, all the same, might be a good practice if running a long run part.

Hi sf74cam:
You also need to consider whether your comp value is going to get bigger than the lead-in and lead-out you've programmed.
If so you may need to re-program it,or the control may alarm.
Of course this depends on how you program the comp...if you're centerline programming and comping the full tool radius you'll be OK...a resharp is always smaller than nominal.
But if you're wear comping you might get into trouble.

I just gotta ask; you say you're cutting HDPE with these 1/2" cutters.
Are they some kind of special or something?

Bog standard 1/2" Garr carbide cutters are just barely worth sharpening if you're really really cheap and find a good local sharpening service that's super inexpensive but still does a good job..
For most machine shops, they're throwaways.
Also in HDPE I'd expect them to last half of forever.

So what is it about THESE cutters that makes it worthwhile for you to regrind them and jigger with the programming and keep track of the sizes etc etc?
Just the logistics would piss me off...obviously the calculus is different for you.

Inquiring minds want to know.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

High volume production situation... a program, once set, gets run over and over and over. The cutting tools, being used on 3 shifts especially, do wear down in hdpe effecting finish. We do have a trusty re-sharpening service. I'm evaluating if it would be worth it to sharpen further. I believe it could be worth the effort over time, as once the programming is set, all that would need to be done is entering tool diameter in machine control at a tool change...my concern with the original question is more along the lines of what a tool can handle as it gets thinner.

Hi again sf74cam:
OK it souds like you are centerline programming and inputting whatever radius the cutter has as your offset.
If that is so, my point about alarming out the control doesn't apply and you can ignore it.

So the issues that remain are as others have pointed out...there comes a time when you've ground away so much of the flutes that there's no gullet left to accommodate the chips.
Only you can determine when that is, and the only way to do that is to keep regrinding a sample cutter until it starts to chip pack and smear the part surfaces.
There are a gazillion factors that will influence this; everything from feedrate to chip evacuation, to chipload to gullet form to gullet smoothness to helix angle to flute count...you get the point.

If you truly want to find out where the limit is, take a dozen cutters that have already been reground the the limit of 0.480" (and are scrap anyway) and have them ground smaller: one of each in 0.010" decreasing increments .
Run them and see whether any or all are still OK.

If you can run them all, you know you were much too conservative.
If you can run none of them without issues, you know your first guess was just about right.
IMO that's the only way forward; all else is bullshit speculation.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

In my experience it costs more to deal with a regrind than a new cutter. Track the time and money spent to pack and ship the dull cutters, file the paperwork, store them separate from the new ones, account for smaller diameter and different cutting behavior, and I think that'll very quickly eat up the few dollars you seem to save over buying new. Also, if your .480" regrind does the job just fine with the same cutting parameters, that means you aren't pushing the .500" cutter hard enough and you're leaving money on the table.

Back in the 1980's I was told not to regrind more than 10% off an end mill. 1/2" mill could then go -.05 to .450 although grinding etc has changed a fair dinkum since some guy in his garage pulling endmills on a TC grinder.

michiganbuck said:

..... losing flute rake angle needs to be considered.
.

Click to expand...

This is so often a missed point.
But at .010 off each side depends on flute shape and that seems rather light.
A handful of degrees here can be make and break.
Also the helix angle changes with each regrind but not real fast. (more of a problem in helix step drill designs)
Re-cutting the flute to fix this is very rarely done in regrinds due to cost but a standard OD regrind does change chip formation and flow so one runs into "packing" even if the flute large enough.
Hence the 10 percent rule but have violated that in the past in high production use.
100 percent agree that testing it is the proof in the pudding.
Helical flute anythings can be complicated animals. Add to that what the regrind source may change things.
Bob

For some kinds of work the ends take the most punishment. A look at the wear land with a loop might confirm this.

With finding this is the case one might cut the number of cycles (parts cut) a little, and then send tools out for end sharpening only so retaining the OD size and cutting tool geometry.

Another good policy is to send out cutters in groups and request that the group to be made the same size so a program or tool length does not have to be changed. *If it doesn't matter then don't ask for this.

Yet another way of sharpening is to face grind a tool such as a straight flute router bit. With having a .005 or .010 wear land on the major length and a .030- .050 wear land on the portion near the end face grinding might be the better choice.

For some router jobs the length and OD are not even important, just being sharp is important, like hand plunging through plastic and by hand or plung and rake across by machine, raking across a jig or free standing to rout out screw clearance holes and screw clearance slots. I once had a job like that (Onsruds 2flt Str HSS) for cutting HDPE plastic and just hand sharpened them with pushing (grinding) the face back .020 or so, and then a tickle grind the ends. Not uncommon to get a thousand at a time.

The more fancy you make your sharpening requests the more the job costs.

Often a sharpening will cost half the new price and give the same performance as new.

End mills are straight-sided, not taper length like a reamer, some shops have end mills cut off and end sharpened only. Some have selected ones cut off, even to their own mark, most just let the sharpener do what they choose. One die shop I worked at never had a dull or resharpened end mill. I think they just sold or scrapped dulls and replaces them with new ones.

Any thoughts?
Consider your annual sharpening costs,
Try straight flute HSS and straight carbide.
If straight flutes work then consider in-house sharpening.
likely you will only save half the sharpening costs so your cost has to be high to consider this.
if you can't save $40k don't bother,
If you have toolmakers with nothing to do then consider it.
Straight flutes because they are easy

Many shops try in-house sharpening and fail or find in-house cost more than a sharpening shop because of so much competition in sharpening they bid low.