[cnc2]

Hi guys,

I've bought a pulley stock 200mm long, it's made out of aluminum 6061 T6.

I need to cut 14mm wide pulleys with a bore of 10mm, the problem is that two different machinists(manual lathes) told me they can't do it because they wouldn't be able to get the bore concentric with the pulley's profile(teeth) the most honest of the two told me it'd be 0.1mm out of concentricity at best.

I saw another guy who had a CNC lathe and several manual lathes, he acted like no problem he wanted to do it on a manual lathe, but when I told him about the concentricity issue saying I want it be done on the CNC lathe, we zero the stock with a micrometer we cut one pulley and we check it if it's fine then, we cut the rest, it was like he was caught and he tried to escape by saying the CNC lathe operator ain't here if you want to wait for him...I never saw him.


Can anyone explain how this is usually done by a pro ? (making pulleys out of pulley stock)

What kind of machine/tooling should be used to do it properly ?

Any tricks are welcome, thanks !
cnc2.

[txcncman]

0.1mm? 0.004"? Do you intend to run this pulley in excess of 2000 RPM? 5000 RPM? 0.004" concentricity on a pulley is practically nothing. You do not state OD. Use collet pads to hold OD.

[cnc2]

Thanks for the reply txcncman !

I did not mention that the pulley is used as a jockey pulley(freewheel/tensioner) in a positioning system, a sort of belt driven linear actuator, and I'm afraid this would result in a positioning inaccuracy, or at least introduce vibration in the whole system.

The O.D of the pulley stock shank is 22mm (at the teeth the O.D is approx 21.5mm), I need a 10mm bore to press two ball bearings inside.

I googled "collet pads" and none of the lathes I saw so far had them, one guy has an automatic collet lathe (I think it's an old hydraulic turnomat) he said let me try, but I don't have enough stock to waist it.

The CNC lathe I saw had a weird chuck (three jaw I think) with bronze rollers normal to the chuck placed at 120° from each other between the jaws. (like a six jaw chuck where three of the jaws are rollers) I have no idea if it can do it, it's the best machine I saw so far (in person/locally of course).

Thanks !
cnc2.

[trademark]

I would bore a set of soft jaws in the cnc or manual lathe with 3 jaw chuck
to the same diameter or slightly less than the od of the pulley stock.
you should get less then .001" runout provided the chuck is in good condition
hopefully the od of the pulley and the teeth were cut at the same time.
That way your pitchline of the pulley would match the od.

[cnc2]

how much would a set of soft jaws cost ? or is it possible to make a set from bar stock ?

I see there's still room for hoping

Thanks !
cnc2.

[Shane1234]

how much would a set of soft jaws cost ? or is it possible to make a set from bar stock ?

I see there's still room for hoping

Thanks !
cnc2.

soft jaws are around 200 bucks for a 3 jaw setup. yes, you can make your own also, but you will have that in time trying to make those little teeth. If you can get away without making the little teeth, you might be able to make them. we have made soft jaws out of aluminum for our nardini, it has a 16" 3 jaw head

should be easy for a guy that named himself cnc2

[txcncman]

Your other option is just part them off in the lathe. Then put them on the mill and sweep in the OD to as close to zero as you want it and then then drill and bore the ID.

[cnc2]

soft jaws are around 200 bucks for a 3 jaw setup. yes, you can make your own also, but you will have that in time trying to make those little teeth. If you can get away without making the little teeth, you might be able to make them. we have made soft jaws out of aluminum for our nardini, it has a 16" 3 jaw head

should be easy for a guy that named himself cnc2

I know as much to machining as your avatar knows to fashion (no machine yet)

Thanks !
cnc2.

[cnc2]

Your other option is just part them off in the lathe. Then put them on the mill and sweep in the OD to as close to zero as you want it and then then drill and bore the OD.

I didn't really understand what you meant.

1) "part them off in the lathe" do you mean starting the bore/rough boring ?

2) "Then put them on the mill and sweep in the OD to as close to zero as you want it " do you mean finish cutting it on the mill, it doesn't make sense to me because from what I've been told unmounting/remounting results in a loss of accuracy.

3) "and then drill and bore the OD" on the lathe or on the mill ?

As you can see I don't get it, it'd be cool if you could elaborate.

Thanks !
cnc2.

[DareBee]

I would part in the manual and bore CNC (but manual would work fine as well).
.002 concentricity would be no problem for anyone.

[txcncman]

I didn't really understand what you meant.

1) "part them off in the lathe" do you mean starting the bore/rough boring ?

2) "Then put them on the mill and sweep in the OD to as close to zero as you want it " do you mean finish cutting it on the mill, it doesn't make sense to me because from what I've been told unmounting/remounting results in a loss of accuracy.

3) "and then drill and bore the OD" on the lathe or on the mill ?

As you can see I don't get it, it'd be cool if you could elaborate.

Thanks !
cnc2.

One thing you will have to learn about machining is being able to visualize how to manufacture a part form beginning to end. You will also have to learn, you are the guy on the scene, the man with the plan (the fish in the barrel).

1) I would not do an ID work at this stage because of your concern for concentricity.

2)You would be verifying accuracy during the set up process with a dial indicator.

3)Typo - should have been ID, not OD. (Has been corrected.)

[cnc2]

One thing you will have to learn about machining is being able to visualize how to manufacture a part form beginning to end. You will also have to learn, you are the guy on the scene, the man with the plan (the fish in the barrel).

Very true, and I asked because I couldn't get the picture.

1) I would not do an ID work at this stage because of your concern for concentricity.

2)You would be verifying accuracy during the set up process with a dial indicator.

3)Typo - should have been ID, not OD. (Has been corrected.)

So, from what I understand the soft jaws should be machined concentric to the lathe chuck and this would be better achieved on the mill to avoid any inaccuracy in the lathe itself, right ? so, mount soft jaws on the chuck unmount the chuck and clamp it on the mill table, find center with micrometer and mill I.D slightly smaller than O.D say 21.9mm for a 22mm shank of pulley stock, is that right ?

Thanks !
cnc2.

[tjb1]

Very true, and I asked because I couldn't get the picture.



So, from what I understand the soft jaws should be machined concentric to the lathe chuck and this would be better achieved on the mill to avoid any inaccuracy in the lathe itself, right ? so, mount soft jaws on the chuck unmount the chuck and clamp it on the mill table, find center with micrometer and mill I.D slightly smaller than O.D say 21.9mm for a 22mm shank of pulley stock, is that right ?

Thanks !
cnc2.

No, part off pulley stock. Place in mill, sweep, bore.

Boring jaws on the lathe itself is what would make them concentric, which would be difficult to do on the mill since you aren't going to or easily sweep the mounting location on the chuck.

[txcncman]

Maybe you should take a day and just go watch machining videos on YouTube to help develop your visualization skills.

I am guessing you are not going to machine these parts yourself and that you will have someone else do it since you keep mentioning other machinists and other machines. You can call out any specification you want for the OD to ID concentricity and TIR. The tighter the tolerance you specify, the higher the price. Since someone else will be doing the actual work, you do not need to concern yourself with how it will be done.

[Geof]

....So, from what I understand the soft jaws should be machined concentric to the lathe chuck and this would be better achieved on the mill to avoid any inaccuracy in the lathe itself, right....

No.

The soft jaws are bored in the chuck on the lathe so that they are true (concentric) to the axis of rotation, the spindle axis.

The chuck body itself may not be perfectly concentric to the spindle axis, similarly the hard jaws in the chuck will not grip parts perfectly concentric to the spindle axis. ("Perfectly" means +/-0.0001" out of true) This is why for best concentricity soft jaws are machined under the same conditions they will be used.

[109jb]

Jeepers guys. Pretty complicated solutions. cnc2, just find someone that knows how the heck to use a 4-jaw chuck, or an adjustable 3-jaw.

[trademark]

The process for soft jaws is as follows:

1. Choose a set of soft jaws from your giant heap of used ones on the shelf.
They should already be bored close to the finished diameter you want to
achive
2. Mount them in the cnc lathe
3. Find a suitable dia. plug to put in the back of the jaws so that when you close the chuck on the plug you have stock in the jaws to clean up the bore and back face.
4. You then bore the jaws and back face.
5. remove the plug, insert part and machine.


hope this helps

[Geof]

Using a 4 jaw and dialing in a parts with teeth on the OD is a bit tricky, also the jaws are very likely to damage the teeth.

In addition using a 4 jaw means each part has to be dialled in which adds a considerable amount of time.

Machining soft jaws means that a smooth circular surface makes even contact with the teeth making damage highly unlikely and there is no time wasted dialling in each part.

Overall using soft jaws is the least complicated and least error prone solution.

[underthetire]

Personally, Id just throw the bar in a 5C collet, bore, face, part off. Pull material to stop, do it again. A good 5C nose should hold .0005 TIR no problem..

[cnc2]

Thanks for the replies guys, now I see how it should be done, I thought about milling the pulley bore but I thought it'd introduce inaccuracy through "deflection" of the pulley stock which is 200mm long, I've even thought about sinker EDM but but it'd cost around $30 per pulley bore (10mm dia. 14mm deep) too expensive.

I know that someone else will take care of the machining for me, the main problem is who to choose, the place is full of hungry guys who'd do crap work ruin my stock...waist my time and money. At least now we know how it should be done properly so I can tell the hungry from the pro.

The CNC slant bed lathe had a mill bit in one of the tool holders (turret) (I'm not sure it has its own motor) I think that it might be used instead of the milling machine but I'm not sure.

If we part the pulleys on the stock before we bore the stock, won't the pulleys go flying(or at least damage the bore) when the mill separates them from the stock during the boring operation ?

Thanks !
cnc2.