PDA

View Full Version : How to cut an INTERNAL CONVEX radius?



ahidley
08-17-2009, 06:09 PM
How do I cut this internal convex radius? (0.7 inch raduis)
The homemade radius cutter wont fit inside. I have to chuck it on the outside, thus the clearance required is to big.
Can I grind a 1/2 in HSS cutter and use the tool post? Will it chatter?
I dont have CNC.

http://i194.photobucket.com/albums/z80/ahidley/genosADAPTER.jpg

http://i194.photobucket.com/albums/z80/ahidley/genosADAPTER.jpg

Evan
08-17-2009, 06:24 PM
Cut on the back side with the tool mounted behind the pivot point.

JCHannum
08-17-2009, 07:23 PM
I would use a form tool. You can rough the radius by cutting several flat angles with the compound, using the form tool to clean it up. That should minimize chatter.

I can't read the dimensions, but a tool can be ground from a HSS tool or use O-1 or W-1 tool steel, drill to the size remove excess, relieve the hole and harden.

Mcgyver
08-17-2009, 07:24 PM
I can't zoom in enough to see the numbers, but if not too large, grind a form tool

rockrat
08-17-2009, 07:26 PM
I would agree with Jim (he beat me to it). I might have a photo of one around here but they are dead simple.

Let us know what you come up with.

rock~

oldtiffie
08-17-2009, 08:50 PM
The wood-workers will love me for this!!!

Make a convex "radus guage" from a large washer - cut it off to suit.

Rough out the shape/curve as said previously.

Put a "large-ish" bar in yout tool-post as a tool-rest.

Get a file and remove all the file grooves from it back to say 1">2" from the end.

Now, using the file/tool, make a tool similar to the tang of the file - minimun front clearance angle and flat on top. Relive so that only the cutting edges contact the job.

Hone (hand) the faces and edge.

Do NOT over-heat or else you will have to re-harden the file.

Lowest speed on lathe.

Hang onto that tool - tight!!

Now feed it into the job and use your hands, arms and body to move the tool. If you get it right, the finish will be brilliant.

J Tiers
08-17-2009, 09:18 PM
If I have read that print right (the numbers are SO tiny......) the radius on that intake sweep appears to be around 0.7"......

Now, I know some of you have large machines....... but a form tool for a 0.7" radius and "forming" nearly a quarter circle will chatter to death most of the machines people on this forum have.

Evan has the right idea.......

BobWarfield
08-17-2009, 09:24 PM
If I have read that print right (the numbers are SO tiny......) the radius on that intake sweep appears to be around 0.7"......

Now, I know some of you have large machines....... but a form tool for a 0.7" radius and "forming" nearly a quarter circle will chatter to death most of the machines people on this forum have.

Evan has the right idea.......

It's not as bad as all that!

Half the battle is getting the form tool properly ground. They can work surprisingly well when you do, even for things where you think, "that's so much area it's got to chatter!"

In this case, radiusing is simplified because you can use a corner rounding mill cutter as your form tool. That guarantees it has the right edge. If it will cut on a mill, why not on a lathe?

I've seen those corner rounders work extremely well for something like this on a lathe. If nothing else, it is very quick to try and you can take very gentle cuts.

Cheers,

BW

Mcgyver
08-17-2009, 10:03 PM
if it is too large for a form tool, next up would Guy Lautard's coordinated method of ball turning. Do the math to move the tool in a series of x/y steps of maybe .003 along the lathe axis.... then with a fine half round file knock down the steps and finish with emery. I've used this for so long now and with such great results, a radius cutter is one tool I've felt the need to make

BadDog
08-17-2009, 10:44 PM
Or a tracer. Hydraulic if you're lucky, ad-hoc manual if you're not...

BobWarfield
08-17-2009, 11:26 PM
Just tried the corner rounding mill cutter as a form tool. It worked pretty good. Some chatter on my small lathe, but would be easy to clean up with a file or whatever your favorite other approach might be.

The chatter was similar to an annoying parting off job.

I started off with the cutter rotated for a lot of positive rake, but it cut better more nearly neutral.

If you have one of these in the toolbox its real easy to just give it a try.

Cheers,

BW

madman
08-18-2009, 09:10 AM
If you can mastercam or cad out with any program available the form in .125 groove tool widths you can then quite easilly form tool the remainder at a slow rpm without a problem. I have made a few race car items using this teqnique and people who saw it said they didnt know I had a cnc machine??

JCHannum
08-18-2009, 09:54 AM
Without setting the job up, I cannot see how a radius cutter would work. Getting into the ID of the bore would require a bit of an exercise in tool grinding and positioning.

Depending on the accuracy required, Tiffie's method will work as well as any and take about ten minutes. The most time consumed would be in making the radius gage if a standard one would not suffice. I have a couple of worn out files ground for hand turning details. Very accurate work can be done without much involved.

If extreme accuracy is involved, a form cutter would be my next choice, simply roughing a 45* cut across the top of the bore will remove most of the material, eliminating most of the source of chatter. A 0.7 radius is not all that big.

Again, depending on the accuracy required, I would do the radius first if possible, the internal details next to allow room for "adjustments".

It is not a difficult operation, overthinking it complifies it.

Paul Alciatore
08-18-2009, 11:44 AM
Sorry, I misread the print.

Black_Moons
08-18-2009, 11:56 AM
ball turning attachment holding a boring bar holding a small HSS bit... :)

BadDog
08-18-2009, 03:21 PM
ball turning attachment holding a boring bar holding a small HSS bit... :)
Now there is a recipe for chatter... :D

When making a form tool, or even a gage, you can make nice uniform and accurate (smallish) convex shape by grinding close with appropriate tool (cutoff wheel, angle grinder, bench grinder, whatever you have or whatever it needs) and a test gage. You also make a lapping tool to provide the finish shape. Simply turn a piece of soft scrap on the lathe to appropriate diameter for the final shape. Load it with appropriate grit lapping compound, and then run the form tool cutting edge (angled for relief) or gage against that lap. Start coarse, work down as fine as needed. Resulting form tool or gage is approximately as accurate as your lap, assuming you remove the initial grinding marks using the lap. Works best for no more than 90* arcs and with some means to hold work piece stable against the lap (i.e. not in your hand). You can make the initial lap long enough for multiple grits, turn a small v-groove at appropriate intervals and you can load each section with different grits, and re-use later. But don't do the lapping on the lathe. Move the lap to a drill press or the like to do the lapping.

ahidley
08-18-2009, 08:40 PM
In the origonal post I said it was a .7 inch radius.
I also need to make 100 of these.
The accuracy is not critical.
Its a velocity stack for a carburator.

Evan, I dont understand your method.

Hannum or rockrat do you have a picture of the bit that you are talking about?

A milling radius tool may work but I dont have one that big

JCHannum
08-18-2009, 09:31 PM
If you are doing a quantity thar large, a form tool (or two) is probably the best option.

I will try to come up with some pics tomorrow, I have a couple of form tools, but am computer poor right now. My main one took a dump & I need to get some backup programs on this one.

drof34
08-18-2009, 10:59 PM
You could turn something round to a dia. of 1.400" and about a 1/4" or so long( similar to Old Tiffie's idea ). Mount this rigidly somewhere so that it doesn't move ( not on the carriage ) with the radius in a horizontal plane. Mount an indicator from the tool post so that when the tool is oriented to the work, the indicator is oriented to the proper place on the radius with some pressure and zeroed. Engage the carriage feed and all you have to do is keep the indicator on zero using the cross slide. Bear in mind that you will be tracing on the back side of the radius so you will need to use a test type indicator with the face towards you

You will probably be pretty good at it when you get to the 100th.

mechanicalmagic
08-19-2009, 12:09 AM
Have you got a Holdridge or ball turner?

BadDog
08-19-2009, 12:49 PM
You could turn something round to a dia. of 1.400" and about a 1/4" or so long( similar to Old Tiffie's idea ). Mount this rigidly somewhere so that it doesn't move ( not on the carriage ) with the radius in a horizontal plane. Mount an indicator from the tool post so that when the tool is oriented to the work, the indicator is oriented to the proper place on the radius with some pressure and zeroed. Engage the carriage feed and all you have to do is keep the indicator on zero using the cross slide. Bear in mind that you will be tracing on the back side of the radius so you will need to use a test type indicator with the face towards you

You will probably be pretty good at it when you get to the 100th.
That's the manual tracing I was talking about. And yeah, I would hate to do that 100 times. But if rigidly mounted, you could also use it as a limit/stop, and that would take some of the difficulty out of it. Making 100? Likely to do this again? You can pick up a hydro tracer for around $100 (saw one at auction go for $30 recently) and have it for this and other projects (depending on size of lathe).