ANGLE RING

[Lathe-Mill]

Hello peeps, I have a question for all you guys, I uploaded a file name ANGLE RING.MC9 to the server, in MC9 files folder.

this was going to be machine on a manual mill, some how is now on my table, and as we know, is due 2 weeks ago, I never seen it before until 5 minutes ago.

without making any angle plates or blocks, what will be the best way to machine the angle on the top of that ring?. May i use a flat endmill?.

any help will be appreciated. thanx peeps.

[savagkd]

Just thinking out loud.

Do you have a sine plate?

[jeff]

I think that if you use a flat endmill, you will have steps,you may have to use a ballnose.

As far as the fastest toolpath goes,others may be of more help than I.

[Jim at Gentex]

I have a sine rotary table that would be perfect for this part, but if you don't have one of those...

 

If you make it from round stock (assuming you do and you have a lathe big enough to hold it) I would do this:

 

-Set your piece of bar stock up on a Bridgeport either lying on its side or standing up and tilt the head to the correct angle.

-Mill or fly cut the entire top surface.

-Take it out of the bridgeport and chuck it in your lathe.

-Turn the OD, bore the ID, part it off at the correct length.

 

HTH

 

P.S. If you don't have a sine rotary table or a big enough lathe you will need to be creative!

 

edit: I went back and re-read. I thought you would make it on a manual machine, not CNC. Sorry!

If making it on a cnc, a ball end mill is the way to go.

[jeff]

I am curious as to which toolpath others say is the best way.

finish flow has alot of retract moves,maybe finish radial is the way to go?

[Jim at Gentex]

Finish radial would be my choice too.

[Lathe-Mill]

we dont have a sine plate, making a fixture may be the only way around, do we have the time?...NOPE

[John Summers]

Is the angle just a plane? If so, make a rectangular planar surface, and cut it 3-axis flowline the long way, and you'll get steps. Then with a large face mill, cut it the short way 'uphill' only. You'll get very low scallops.

[crazy^millman]

I would use a ball em and surface finish contour. I would use the inside and outside of the ring as my boundaries. You should get very little retracts but if you do change the advance settings in the step over to 100000% should slove that on the flowline as well might look at sprial as well for flowline if you wanted to use that but would need to be one solid face to use flowline effectly.

 

HTh

[thoskins]

try surface finish project. Use the blend option. pick the top sufcace as the drive surface and the two arc's at its edges for boundaries. I put your file back in the mc9 folder as "angle ring-a.mc9" with toolpath in it. Good Luck.

 

Tim Hoskins

[Lathe-Mill]

HELLO!!... I didn't got bach to this post earlyer but i was stopped from doing it and now i'm going back at it..

I made a jig plate 15x15 square where the part will be held, i have a 6 inch long sine bar that i found at the shop after so much digging...here is the question,since i never used a sine bar before, someone explained to me how to use it and i think that i need a .022 gage pin under the sine bar....could someone please verify if i have the right pin?

thanx . ( i hope i do)

 

P.S: the part is a 13" dia ring and the angle that it needs is 1.25 deg. on the top face.

[Jim at Gentex]

I think you need a .131 pin.

 

The calculation is the sine of the angle x the length of the sine bar, so the .022 pin would work if the sine bar were only 1" long.

 

In your case 1.25 sin = .0218 x 6 = .1308

 

 

edit: Sorry...I haven't done this in a while either so I could be mistaken. One more thing...

The length of the sine bar is measured center to center between the two round drums, so your bar may be 6" overall but actually is a 5" sine bar. If that is the case, you need a .109 pin.

[Brendan P]

I'm with Jim

.131 pin @ 6.0" sine bar.

Dia. of the part should not make any difference.

[Psychomill]

The quick and dirty way I've done this is just flip the fixture over and cut grooves into the face with a ball mill. Most sine bars aren't very large and trying to clamp it down with a 15 inch plate could be tricky.

 

So, for example, you could take a 1/2 ball mill and cut two grooves across the plate, 10 inches apart. At 10", you just cut the second groove .218 deeper than the other. Then just use 1/2 gage pins in the grooves and toe/strap clamp the plate down to the table.

 

Just my 2 pennies.

[Jim at Gentex]

Psychomill!

 

Jim teh LOVES teh 'quick & dirty' methods!!

[Brendan P]

Psycho,

That is an excellent idea.

[Roger Peterson]

Unless it's a homemade sine bar it is 5" center to center. +1 to psychomill, works well, but don't limit yourself to 10". Round off to the nearest whole number that is doable, clamping will be easier this way. Even though the endmill may not be exactly .500" with a .250" radius and the guage pin you will need to use to fit in this groove may be a .499" guage pin, over 14" it is still going to be more accurate & rigid than clamping to your 5" sine bar.

 

 

HTH

[Lathe-Mill]

WOW...thanx for all your replys, very new and interesting .....now, does it matter where to locate the sine bar?

letf right center of plate?

thanx

[Lathe-Mill]

i mesured the sinebar, center to center is 5", so i need a .109 pin gage.

thanx

[Jim at Gentex]

I would use Psycho's method and clamp it down resting on 1/2" dowel pins in the grooves. Like Roger says, this will be the most rigid setup you'll get.

 

If you do use the sine bar, it shouldn't matter where you place it as long as your jig plate is parallel to the sine bar.