If you only had a cnc mill would you run these?

S

Shawn_Laughlin

Aluminum

Joined

Mar 28, 2019

• Jan 6, 2020

• #1

These are all machined from a bronze casting on a cnc lathe but, was wondering if you had one of these to make or something similar in shape and you only had a mill do you think you could machine the part efficiently.

I look at it and don’t see how it couldn’t be done. The only thing that I think would be troublesome is it has flange grooves. Looking at the picture you will be able to tell where those grooves are located. I have ideas on how I could do the grooves using a mill with rotary table or a machine with full on 5 axis capability but, while having tons of experience working with metal, I still have much to learn about the machining side and is exactly why I came here to get advice.

So if you only had a cnc vmc 3,4 or 5 axis and did not have cnc lathe would you attempt it?

 

G

Garwood

Diamond

Joined

Oct 10, 2009

Location

Oregon

• Jan 6, 2020

• #2

I don't know about many thousands of production parts, but I've done a few hundred parts at a time with similar features and made shop rate doing it.

Mill can thread the outside NPT, but milling the surface "tapered" will be iffy.

Milling surface finishes are always significantly different looking from lathe turned finishes. The parts that I did looked "cool" according to the customer with the milled finish. If you have a customer expecting a lathe finish and he gets a milled part there might be issues. Functionally it's probably fine though.

I mill retaining ring and o-ring grooves with woodruff cutters and slitting saws. You can kinda hog with a HSS saw in aluminum and hold good size.

 

A

AARONT

Stainless

Joined

Feb 19, 2013

Location

Madison, WI

• Jan 6, 2020

• #3

Certainly could. We do some similar shaped parts(different features) in rotaries. The one on the left would for sure be a one op part in the rotary. The second part would most likely be 3 ops with 4th axis, 2 ops with 5th. You would just need a custom trepanning tool(think "c" shaped) to get that undercut face groove on the flange for the 4th axis. I'd quote the tool out and bill it to the customer. 5th axis should be able to spin the part so you could turn the groove in.

 

S

Shawn_Laughlin

Aluminum

Joined

Mar 28, 2019

• Jan 6, 2020

• #4

Garwood thank you very much because I had not thought about the lathe vs mill finish. On this part I don’t think it will matter but for future reference it’s priceless. I have a manual lathe and still didn’t think about it.

Thank you for bringing up the taper for threads bc I was thinking about last week and I forgot to ask. Do you see it as a major or minor problem cutting the taper for the male threads?

What about the female threads? The female threads range in size from 1” to 2-1/2” and I would think rigid taping with a 2-1/2” pipe tap would be an “experience”. And since they are npt the hole would have to be tapered also.

 

G

G00 Proto

Hot Rolled

Joined

Feb 18, 2013

Location

Dirkdirkistan, ID

• Jan 6, 2020

• #5

Yes, and I could beat the lathe quote all day long. I would fixture twenty at a time on a tombstone on the forth axis. All of them could then be done in one operation if you are smart about the fixture. All of the undercuts and angles would be custom form tools. Thread mills make better threads than single point on the lathe and faster. Only pain the ass would be the fixture design, and I would build two of them and load one with the other one was running.

Factor in the brass recycling bonus money. That will keep you in beer and fritos for the entire project.

 

kustomizer

Diamond

Joined

Aug 17, 2007

Location

North Fork Idaho

• Jan 6, 2020

• #6

Tapered endmills are an off the shelf item with many suppliers, I use them on several projects. I cut the surface with the tapered endmill, cut the thread and cut the taper again on soft metal to get rid of the burr.

https://www.mscdirect.com/browse/tn/Milling/End-Mills/Tapered-End-Mills?navid=12106245

 

C

Comatose

Titanium

Joined

Feb 25, 2005

Location

Akron, OH

• Jan 6, 2020

• #7

For the ID threads that size think thread mill, not tapping. Tapered thread mills for pipe threads are an off-the shelf item, and if it's just a few, single pointing can taper too of course.

 

Cole2534

Diamond

Joined

Sep 10, 2010

Location

Oklahoma City, OK

• Jan 6, 2020

• #8

kustomizer said:

Tapered endmills are an off the shelf item with many suppliers, I use them on several projects. I cut the surface with the tapered endmill, cut the thread and cut the taper again on soft metal to get rid of the burr.

https://www.mscdirect.com/browse/tn/Milling/End-Mills/Tapered-End-Mills?navid=12106245

Click to expand...

Last NPT threads I milled I helixed into the bore at the same pitch as the thread. Logic was that any ID imperfections would be cleaned up by the threadmill without requiring a cutter that I didn't have on the shelf.

As for the OP- sure I'd bid them. Not sure I can do it as fast as the horizontal with a tombstone, but it's definitely possible.

 

S

Shawn_Laughlin

Aluminum

Joined

Mar 28, 2019

• Jan 6, 2020

• #9

AAROT thank you. Your confidence gives me confidence that it can be done. I think I will eat the tool cost bc I work for the company that has these made and I feel fortunate enough that bc they are giving me all of their work it and I will have parts to make for as long as they are in business,”hopefully a long time” it’s allowed/allowing me to start a business and have steady work.

Anyways knowing the vmc is very capable I now know I need to get a little larger capacity machine than what I was about to buy.

 

S

Shawn_Laughlin

Aluminum

Joined

Mar 28, 2019

• Jan 6, 2020

• #10

Man This is my first day back since Christmas eve and all morning had been ugh I’m ready to go home but with each comment I read my day is getting better and better. Thread milling has been suggested a lot so I guess need to do some learning. A tapered end mill should’ve been a no brainer but all I was seeing was milling the taper with a ball end mill. The tapered end mill will be much quicker. Thanks man

 

Last edited: Jan 6, 2020

Cole2534

Diamond

Joined

Sep 10, 2010

Location

Oklahoma City, OK

• Jan 6, 2020

• #11

Shawn_Laughlin said:

Man This is my first day back since Christmas eve and all morning had been ugh I’m ready to go home but with each comment I read my day is getting better and better. Thread milling has been suggested a lot so I guess need to do some learning. A tapered end mill should’ve been a no brainer but all I was seeing was milling the taper with a ball end mill. The tapered end mill will be much quicker. Thanks man

Click to expand...

Watch this before you buy a tapered EM- YouTube

 

V

Vancbiker

Diamond

Joined

Jan 5, 2014

Location

Vancouver, WA. USA

• Jan 6, 2020

• #12

Threadmilled thousands of larger NPT threads in Ryerson EZ-Cut 20(kind of like 12L14 in plate form) with full form NPT threadmills. Never tapered the hole prior. Just drilled and threadmilled.