What's new
What's new

is a tool like this possible to make?

empower

Diamond
Joined
Sep 8, 2018
Location
Novi, MI
in reference to an earlier thread i made about having to make a back counterbore feature, wanted to see if there are any tool grinding experts on here that could tell me if this is doable or not. and would anyone be interested in making something like this?

1710449127329.png

basically the red part's only function is to act as a stop to bottom out the counterbore. blue part is the cutting flutes that need to make the counterbore at .5" +.0007 -0.

green part needs to be precision ground to .382" +- .00025. grey part would just be 3/8" shank. overall length 6"
 
So if you're going that route, are you wanting to do this with a cordless drill or something?

If you could control depth another way, such as with a bridgeport quill, I'd use one of these (i saw mentioned in the other thread): https://www.mscdirect.com/product/details/09937269

Edit before i posted: the radius is 1/32", there are solid carbide ones with 1/64" but they are pricey!


Look on the next catalog page in the book for a shank.

You could make a bush that fits the shank to hold in your .382 hole. You may also be able to rig up a stop on the rod or tool itself but I'm not sure.


I would really really really suggest shrinking in a tube or convincing someone that a 1pc bushing is better. But I gather that you already weighed that option and you can't. bummer.

Since it's a hinge and you can't get to the other side, I assume there's actually 2 hinges in line with each other. Kinda seems like "line boring" type thing, but I don't see anyone doing that with a 3/8" nominal diameter tool?
 
either cordless drill, or i could set it up in my bridgeport.

i asked about pressing in a 1 pc bushing, was told no.
yes, 2 hinges in line with each other.
 
Hi Empower:
I just gotta ask:
If you intend to put the grey part into a collet. how will you get the tool into the bore?
Are you planning to thread the tool through first and then put it in the collet?

Also, you realize that if you want to back bore with this tool, you really should put a left hand spiral onto the tool so the cutting edges have positive rake instead of negative rake.
You could also put the cutting edges on the other side and run the tool in reverse of course, but you want positive rake to help you get a clean cut and with the tight tolerance for that counterbore you have an impossibly challenging problem here...one picked up chip and you're fucked.

This is one of those high risk features that can trash the whole job in a heartbeat, and there is no way to sneak up on your size with a counterbore...you have to hold your breath, grab your cojones and go for it, and then find out whether it's fucked up or not when you pull the tool and inspect the bore.
I personally HATE shit like that, so I feel for you.

I'm with the guys who advocated burning these with a sinker if there's any way to farm these out.
Burning it makes the job predictable and easy to control.
You can whisker out the diameter in tenths if you want and it's just a matter of editing the trode orbit...one or two lines of code, that's all.
You don't have to care how big the trode turns out...just make it whatever is convenient and then write the orbit to accomodate what you made.
It'd also cost less than making and qualifying a tool like this...you can just lay the 48" long part down sideways and orbit a 3/8" trode in Y and Z from the back side... easy peasy.
You do need a substantial sinker to get the whole part in the tank though, or else leave the tank door open and defeat the interlock and dam your cutting zone...lots of stupid shit to do no matter how you tackle it.

On a last note, whoever designed this thing and dropped it in your lap needs a dope slap.
It's a ridiculously difficult design.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Last edited:
I have made a surprising number of back spotfacing and counterboring tools like that over the years. All bigger than yours, which makes it a lot easier, but the idea is sound.

Off the shelf versions exist, eg. Granlund, but you'll never hit that tolerance with one of those.

I expect you'll struggle with that tolerance no matter what.

Re. sinker, I assume there is also a concentricity / coaxility tolerance with the other end, how difficult would it be to get them properly aligned on a sinker?
 
Hi gregormarwick:
You asked:
"how difficult would it be to get them properly aligned on a sinker?"

Easy, I can control it within microns and my sinker is a cheapass one from 1996.
You make your trode smaller than the 0.382" bore and just stuff it in and then pick up.

Sinkers use a touch to pick up almost like a touch probe...they're exquisitely sensitive.
A circuit senses when the trode touches the workpiece and establishes electrical continuity between trode and workpiece.
The smallest movement increment on mine is a tenth and it'l reliably discriminate that tenth, so if you touch the trode and then back off a tenth you'll lose contact and the control can tell.
Modern ones are much better than mine is.

On a high quality modern sinker this job would truly be a doddle...you wouldn't even break a sweat.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
If a pull cutter for a steel or aluminum part you definitely need positive helix flutes to the direction of rotation of axial feed, perhaps 10 -12 * end clearance, and not bump the following tooth axial cutting edge, need Od clearance to the circle grind margin., and perhaps .0002 per inch OD back taper. to be much like a flat bottom reamer.

Might wish to add centers so to grind between centers, may need to use a steady to keep a 3/8" x 6" part straight.
I dont want the job, you might call Special Drill and Reamer on Troy Michigan.
Tell them what you want to do and the material. They may come up with a better method/Tool.
A one up will cost pretty big bucks.
Tell them Buck recommend…See if anyone remembers Buck.
.
 
Hi nihilistic:
Here's the original thread.

This part is awful to try to make...truly awful as soon as you check out the details.
Whoever designed this thing hates machinists and wants to make them hurt! :willy_nilly:

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Hi Empower:
I just gotta ask:
If you intend to put the grey part into a collet. how will you get the tool into the bore?
Are you planning to thread the tool through first and then put it in the collet? essentially, yes

Also, you realize that if you want to back bore with this tool, you really should put a left hand spiral onto the tool so the cutting edges have positive rake instead of negative rake. just modeled for illustration, not to represent accurate flutes
You could also put the cutting edges on the other side and run the tool in reverse of course, but you want positive rake to help you get a clean cut and with the tight tolerance for that counterbore you have an impossibly challenging problem here...one picked up chip and you're fucked.

This is one of those high risk features that can trash the whole job in a heartbeat, and there is no way to sneak up on your size with a counterbore...you have to hold your breath, grab your cojones and go for it, and then find out whether it's fucked up or not when you pull the tool and inspect the bore.
I personally HATE shit like that, so I feel for you.

I'm with the guys who advocated burning these with a sinker if there's any way to farm these out. this job is already being farmed out to me by another shop, rather not do that if i can help it
Burning it makes the job predictable and easy to control.
You can whisker out the diameter in tenths if you want and it's just a matter of editing the trode orbit...one or two lines of code, that's all.
You don't have to care how big the trode turns out...just make it whatever is convenient and then write the orbit to accomodate what you made.
It'd also cost less than making and qualifying a tool like this...you can just lay the 48" long part down sideways and orbit a 3/8" trode in Y and Z from the back side... easy peasy.
You do need a substantial sinker to get the whole part in the tank though, or else leave the tank door open and defeat the interlock and dam your cutting zone...lots of stupid shit to do no matter how you tackle it.

On a last note, whoever designed this thing and dropped it in your lap needs a dope slap.
It's a ridiculously difficult design.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
replies in bold
 
If you want it made in carbide, and are willing to pay the price, I can think of some people who will make this for you, though they'll probably do it with no guarantees of it working how you want.

MITGI: Super Fast, high quality tooling. 2 week turnaround with ALTIN coating. It's good stuff, but it's not SUPERB stuff. I use them when I need good tools quickly.
Schwanog: They'll make it in somewhere between 3-6 weeks, it will be higher performance than the MITGI tooling.. For 8 parts in aluminum, probably not necessary.
Ceratizit: Same as Schwanog, but they'll likely take between 4 and 12 weeks, depending on workload.
GWS Tool Group: They'll make a nice tool, somewhere between MITGI and Schwanog in quality/performance, but the lead time can be whatever they feel like, and they may or may not hit it anyway.
MAFord: Same as GWS, but less expensive and possibly slightly higher performance.
Ultra Tool: I've never gotten anything quite like this from them, but have had other custom carbide round tools that worked well. They're about MITGI quality/pricing, with slightly longer lead times.
Pan American Tool: May be willing to make it for you in HSS, I've used them for custom reamers before, and they work well with decent turnaround and surprisingly low price (I'm used to paying for custom carbide tooling)

Out of all the above suggestions, I'd probably start with MITGI, solely because you're cutting 8 parts in aluminum and don't need the highest performance tools in existence.
 








 
Back
Top