Suggested method of machinng

Topics include, Machine Tools & Tooling, Precision Measuring, Materials and their Properties, Electrical discussions related to machine tools, setups, fixtures and jigs and other general discussion related to amateur machining.

Moderators: Harold_V, websterz, GlennW

Post Reply
charkmandler
Posts: 6
Joined: Sat Apr 29, 2017 8:11 pm

Suggested method of machinng

Post by charkmandler » Thu Nov 08, 2018 7:28 pm

I will be making 30 of the retainers (shown in the photo) to help a friend and I am interested in options for machining. There is a through hole that is threaded, the 'shiny' collar diameter needs to be turned to fit 3/8" holes with a tolerance of -.0005". The basic turning is no issue as I could turn either way round on the end of a bar, with a preference to having the critical diameter outwards so that it is easy to measure. I could use a profiling / grooving insert tool to turn the complete retainer with the compound giving the taper on the inside (the taper stops at about .400" diameter - not clear in the photo).

The main doubt in my head is the best time and way to mill or slot saw the rectangular shape out of the turned one. One method could be to turn the piece on the inside to the bottom of the taper which leaves about a .400" diameter and then transfer the bar to the mill and mill each side. Then return to the lathe and part off. The other method could be to make all the pieces and the clamp a few at a time in the mill vice and mill off. The tapered section will be wafer thin to the edge and could tear, so maybe use the linisher to remove the bulk of the material before milling.

Any suggestions would be welcome, thanks.
Attachments
ET100-1AC.JPG
ET100-1AC.JPG (18.06 KiB) Viewed 349 times

User avatar
GlennW
Posts: 6654
Joined: Sun Apr 15, 2007 9:23 am
Location: Florida

Re: Suggested method of machinng

Post by GlennW » Thu Nov 08, 2018 8:45 pm

Please post a better image, as you can tell absolutely nothing from that one!
Glenn

Operating machines is perfectly safe......until you forget how dangerous it really is!

User avatar
Rich_Carlstedt
Posts: 1445
Joined: Sat Dec 21, 2002 12:16 am
Location: Green Bay Wisconsin USA

Re: Suggested method of machinng

Post by Rich_Carlstedt » Thu Nov 08, 2018 11:47 pm

Closer picture
Material ? type and size ( Flat bar so you do not need to mill ? )
Equipment/tools on hand ?

Rich

User avatar
Rich_Carlstedt
Posts: 1445
Joined: Sat Dec 21, 2002 12:16 am
Location: Green Bay Wisconsin USA

Re: Suggested method of machinng

Post by Rich_Carlstedt » Thu Nov 08, 2018 11:58 pm

As a second thought
For a home shop to produce "repeatable' " tight size ....and a half thou range is tight (!) , consider doing all tight work at the same step/moment.
For example "If" you had the parts finished except for the diameter , say at + .010" , make a fixture in your lathe chuck that is hollowed to match the taper , and has a threaded stud in the middle. spin the part onto the thread until tightened then come in with a sharp HSS toolbit to get diameter. Spin off part , replace and repeat.
By not adjusting the cross-slide or tool-slide gives you the best chance for repeat control and consistency
Material is also critical
Rich

charkmandler
Posts: 6
Joined: Sat Apr 29, 2017 8:11 pm

Re: Suggested method of machinng

Post by charkmandler » Fri Nov 09, 2018 4:23 am

Material is EN8 - I have a good lathe with a DRO and turning the diameter to a fine tolerance is not a problem. I also have a well equipped vertical mill with DRO.

As I mentioned in the post, I do not really have a problem with the turning - listed my suggested method as I'm very open to suggestions and learning. My main issue is with the milling of the sides and when / how to do it and not let the job take longer than it should.

Interesting using flat bar that could be milled to size and then turned. I would have two concerns based on wanting to do the complete turning operation in one 1) when machining the backside of the part the continual knocking of the rectangular bar will knock the sharpness of the tool out and over 30 pieces will consume time. 2) Using a 4 jaw chuck I can centre the rectangular bar when setting up but when loosening 2 jaws to move out for the next piece over a few pieces the absolute centre will be lost and repeatedly centring will take time.
Attachments
Vin - Rocker Feed Bolt - Nut.pdf
(211.88 KiB) Downloaded 46 times

User avatar
Bill Shields
Posts: 5147
Joined: Fri Dec 21, 2007 4:57 am
Location: Somewhere in the World
Contact:

Re: Suggested method of machinng

Post by Bill Shields » Fri Nov 09, 2018 7:24 am

I would do it in a Swiss type (or Turn-Mill machine), but then that is how I think.

User avatar
tornitore45
Posts: 1568
Joined: Tue Apr 18, 2006 12:24 am
Location: USA Texas, Austin

Re: Suggested method of machinng

Post by tornitore45 » Fri Nov 09, 2018 8:00 am

Since milling one part is the most time consuming operation, starting with a long flat bar would be my choice.
As soon as the piece is parted off, I will center drill or turn the round part so the stock can be advanced in the 4 jaws chuck and still have a centering reference. If you are worried about interrupted cut, use two tools, one beefy to rough where resharpening does not affect repeatability and one very sharp to finish.
Mauro Gaetano
in Austin TX

John Hasler
Posts: 970
Joined: Tue Dec 06, 2016 4:05 pm
Location: Elmwood, Wisconsin

Re: Suggested method of machinng

Post by John Hasler » Fri Nov 09, 2018 8:11 am

With 30 pieces to do it is certainly worthwhile to make jigs and/or fixtures. I'd want to turn round parts in a single setup and square them up last. With the right fixture you could do ten at a time. Perhaps address the tearing problem with sacrificial fixtures. Do you have a grinder?

User avatar
GlennW
Posts: 6654
Joined: Sun Apr 15, 2007 9:23 am
Location: Florida

Re: Suggested method of machinng

Post by GlennW » Fri Nov 09, 2018 8:48 am

Using what you have to work with...

7/8" Round bar
Drill, tap, turn small diameter, and part off to rough length.
Soft jaws on lathe chuck.
Hold by small diameter, face to length and then cut taper.
Soft jaws on mill vise properly surfaced and bored to accept small diameter of part.
Run around perimeter with mill. One roughing and one finish pass. I'd use a smaller dia carbide (new sharp) end mill at high spindle speed.
Glenn

Operating machines is perfectly safe......until you forget how dangerous it really is!

User avatar
Rich_Carlstedt
Posts: 1445
Joined: Sat Dec 21, 2002 12:16 am
Location: Green Bay Wisconsin USA

Re: Suggested method of machinng

Post by Rich_Carlstedt » Fri Nov 09, 2018 10:37 am

Multiple setups using flat bar is simple if you make a fixture to hold the flat bar in a 3 jaw chuck (assuming you have a accurate chuck)
The fixture looks like a Clam shell and holds the flat bar repeatedly on center in a 3 jaw chuck so you eliminate that variable. Then you just turn to size and tap . No milling required. Because of the rigidity of the fixture ,it totally captures all 4 surfaces , vibration is minimized. The flat bar should be to finished thickness to eliminate the mill

Take a 2 inch diameter aluminum round by 3 inch (ie.) bar and reduce part of it so it looks like a top hat.. make it 1.800 OD for example.
The rim of the hat is a stop .
Reverse it and using the "stop" against your jaws Bore a hole to the same size as plate thickness . It must be accurate ! AND mark the chuck key socket you use to tighten it--- VERY Important for repeatability...only use that socket! . Take the Aluminum fixture and saw cut it in hall so the hole becomes a half hole -NO precision necessary "
Put the two halves in your mill with the saw cut facing up and lay a dowel pin in the exposed hole ( (looks like a half round keyway ). Indicate the dowel so the mill and the dowel match X and Y axis ! Now mill it to your flat bar width ( say 1.000 inch , ) ACCURATELY to .500 on either side of the centerline and to the exact depth of the bored hole. You now have a split collet of sorts to hold the bar and the rest is history.

Rich
Retired Manufacturing Engineer

In machining, the more setups you do to a part, the more error exposure
in machining, the more tools you use, the more concern for wear and accuracy variables
In machining , keep it simple. The more knobs turned, the more difficult the task
In machining , the choice of raw material and size determines the effort required to complete the project
Repeatability and simplicity ares KINGS

A friend of mine said this
"You know machining is 90 % setup !"....................Yepp !

RSG
Posts: 960
Joined: Fri Feb 04, 2011 9:59 am
Location: Ontario, Canada

Re: Suggested method of machinng

Post by RSG » Fri Nov 09, 2018 10:59 am

What GlennW said!!!!!

Fastest, easiest method......
Vision is not seeing things as they are, but as they will be.

charkmandler
Posts: 6
Joined: Sat Apr 29, 2017 8:11 pm

Re: Suggested method of machinng

Post by charkmandler » Fri Nov 09, 2018 6:08 pm

Thank you Glen and Rich. My preference is with Rich's one setup method so that accuracy will be guaranteed although I am never a fan of turning rectangular material. Glen's method will be easier and although there would likely be about .0005" of run out using soft jaws, that is not critical so long as the surface is square to the other side - which it would be as its pushed up against the soft jaws. There would me more work with the milling afterward but I recon both methods would take similar time (factoring in the slower rate turning the rectangular section). If I have time, I might be tempted to make half by one method and half by the other as an learning exercise - there goes any time saving.

Thank you very much for advise and ideas. I did a lot of machining of one off parts for vintage / classic racing motorcycles in the 80/90's and then had some time off. All of that work was pretty much self taught, resulting in reliable and winning engines, although some of my machining methods were slow. Now with the internet and advice such as above I have a chance to learn techniques outside of my limited thought process. Thanks again, Mark.

PS - will be doing this job in a few weeks time and will let you know the results.

Post Reply