What's new
What's new
By:
Advanced search…

Help with choosing the correct tooling.

A

Anthony3076

Plastic
Joined
Jul 17, 2018
I've run into a situation that I haven't really been in before and would really appreciate the help with finding a tool that I could use for this job. I need to bore a 6" hole through a 3" thick, 24" diameter S.S. circular flange. Normally this would be something I would do on the lathe but because the hole is offset from the center I have to do it on the mill instead. I have a prototrak DPM2 conversational mill with R8 collet, so basic cnc operations are easy, but my dilemma is finding a tool i can use to get through the 3" depth. My first thought was to use an index-able end-mill;However, I haven't used index-able end mills much, so I'm not sure they would have the reach to cut through the piece. I don't want to spend ungodly amounts of money on a new tool because its only two pieces and I won't have to do this again for a long time. Any input on tooling would be greatly appreciated and if its not too much to ask, a link to the tooling you recommend would be fantastic as i'm not too experienced with a lot of the index-able cutters.

Thank you for your help,

Anthony
 
I would drill it out with your biggest drill, then use your largest roughing endmill to plunge cut overlapping bolt hole circles until you are near your final diameter. Mill out the scallops and finish with a boring head.

Don't center cut with the endmill, overlap the bolt hole circle enough that you are only using the outside third of the end mill.

Or drill a hole, break your bandsaw blade, thread it through the hole, reweld the blade, and saw out your slug.
 
The bolt hole idea is great and might have to be what I do if the budget doesn't allow water jetting a rough hole into it. And the saw was my first idea although these pieces are upwards of 200 pounds so "man-handling" them would be quite the challenge on the band saw! Thank you for your input though I appreciate it!
 
Anthony3076 said:
I've run into a situation that I haven't really been in before and would really appreciate the help with finding a tool that I could use for this job. I need to bore a 6" hole through a 3" thick, 24" diameter S.S. circular flange. Normally this would be something I would do on the lathe but because the hole is offset from the center I have to do it on the mill instead. I have a prototrak DPM2 conversational mill with R8 collet, so basic cnc operations are easy, but my dilemma is finding a tool i can use to get through the 3" depth. My first thought was to use an index-able end-mill;However, I haven't used index-able end mills much, so I'm not sure they would have the reach to cut through the piece. I don't want to spend ungodly amounts of money on a new tool because its only two pieces and I won't have to do this again for a long time. Any input on tooling would be greatly appreciated and if its not too much to ask, a link to the tooling you recommend would be fantastic as i'm not too experienced with a lot of the index-able cutters.

Thank you for your help,

Anthony
Click to expand...

usually drill a hole through with a spade drill and if hp of machine not high you can use a roughing end mill. to get 2 to 6" flute lengths and reasonable rigidity usually talking 1.5" or 1.75 or 2" dia
....they work better side milling and even if 0.1" width of cut at full 3" depth usually can get feed up to 3 to 6" per minute feed
.
a multi row carbide insert mill that can cut over 4" depth of cut might be better for stainless, but they are not cheap. normally a big brand name one like 1.5" dia would be over $1000. obviously they sell bigger dia and longer ones but price is even higher. literally bigger ones can be $5000 to $15000. and need a lot of horsepower to run to capacity.
.
cheaper brands might be available but beware cheap carbide inserts. often 1/2 price carbide inserts are not worth it. literally can fail within minutes and leave a extremely bad finish. and it you end up using 10x the number of inserts to do a job even at 1/2 price you are not saving any money
 
if you use a boring bar its going to take a long time. but if you got a boring bar and cannot afford spending over $1000 on new tooling than many do it the slow and cheaper way.
.
still the more you drill and or mill out the less boring you need to do
.
be aware larger drills and mill require a lot of horsepower and ability to hold the part. it aint going to help having a very large tooling if it going to need 20hp and your machine only has 5hp. or if part starts moving in vise or fixture that can be a big problem if it destroys a $2000. carbide insert mill
 
depends on your boss. some bosses dont mind buying tooling to save time and other bosses would prefer you dont spend more than $10. to do a job even if it takes all week.
.
if you send it out and have somebody else do it, obviously that will cost money but it might be faster to get job done.
.
literally if you are using a 1 to 3hp mill it will take a lot more time than if you got a 20hp mill. literally a 1hp mill can take 10 to 20 times longer than using a 20hp mill and tooling that can handle the hp. i have seen jobs take 10 hours that could be done in a hour on a bigger cnc
.
its roughly 0.2 to 0.4 cubic inches milled into chips per hp per minute for 304 SS if you got 100 cubic inches thats 500 minutes at 100% usage of 1 hp. inefficent milling paths it can be 5000 minutes to remove the same 100 cubic inches
 
mill 1/2 way from each side so you don't have to use long tooling. I would start with a 1/2" dia. solid carbide rougher. make sure you bolt down the center slug. HARD SCALEMILL ROUGHER I would try this but grind some relief above the flute so you can get down 1.5"
 
A mill with a R8 collet isn't the right tool for the job, no matter how hard you try. Send the job out.

Yes, if I was on a deserted island and that was the only way to fix my ride out I would chain drill the rough hole, use a rougher to get to near size milling from each side, and finish by interpolating the bore, milling from each side. You have the wrong mill. Send it out.

You didn't say which stainless, which tells me you have no experience with stainless. Send it out.
 
Well a hole saw comes to mind to move most but not cheap.
Drill, boring head one way.
Chain drill a bunch of holes around the size and hit it with a hammer to get all that out of there. I like this as you don't cut so much metal and it is fast.
Then relived shank end mill and passes for depth. If picky finish with a boring head.
You can not take this depth on what you have.
Bob
 
For my own information, you have a part that is 24" diameter, and you have a Lathe with only a 3 jaw chuck?? If you have a 4 jaw you can bore eccentric holes.

I'm only asking because I don't think I've ever seen a 3 jaw that size. Pitiful idea IMO.

R
 
You must log in or register to reply here.

Similar threads

S
Another "cant find a tool holder for my inserts thread" *solution found*
Replies
8
Views
666
William Lynn
W
I
Are these shell mills and if so can u get a tool holder for them
Replies
7
Views
454
imported_eric_h
I
E
Need help finding a certain tool.
Replies
6
Views
516
L Vanice
L
M
Help finding source for small piston u-cup seal
Replies
6
Views
313
winger
W
U
Organizing Orphan/One-Off/Extra Tooling- When Index Won't Do
Replies
8
Views
604
Joe Gwinn
J








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top