PDA

View Full Version : milling a tapered pocket



plunger
01-21-2011, 03:05 PM
I would like to try and make a 10 impression mould for a small urethane part. I need to machine 10 holes in a rectangular steel plate which is 16mm thick.The problem is the holes are tapered and have about a 7 degree taper to them. How do you machine a tapered hole on a milling machine?
Regards eugene

Toolguy
01-21-2011, 03:12 PM
Get an end mill with the taper you need, use like any other end mill. Common tapers run from 1/2 degree to 15 degrees. Those are used all the time in mold making.

plunger
01-21-2011, 03:23 PM
The size of the hole is about 36 at the small side to 40mm on the big side Could I perhaps make such a taper endmill. I will be using aluminium plate for the mould

photomankc
01-21-2011, 03:24 PM
Manually:

Tilt the head after the main pocket is milled out and finish the edges with the tilt set but that would produce some type of left-over the corners I think.

Tilt the part with angle blocks or sine vice or something instead of the head same as above.


CNC:

3D capable CAM, with ball-end end mill and small step-overs to generate a ramped side. This would have rounded internal corners but the surface would not be perfect.


Edit: Yes, forgot they make the tapered end mills.

Toolguy
01-21-2011, 03:50 PM
You can make your own tapered endmills out of regular straight ones with a tool & cutter grinder.

Machinist-Guide
01-21-2011, 03:58 PM
I think the most practical thing to do is as ToolGuy said. Get a tapered endmill.

strokersix
01-21-2011, 04:15 PM
Many years ago I made several tapered endmills with radius on the end from regular ones with a spindex under surface grinder, then freehand grinding the radius and clearance. Not perfect but got it done. I had steadier hands, better eyes, and enough determination then. Just saying it can be done. I still have them in fact and they do occasionally find a use.

I've found when freehand altering multi flute cutters it's better to do just one flute and grind away the others. Eliminates trying to get multiple flutes all identical.

plunger
01-21-2011, 09:02 PM
i dont have a surface or toolgrinder. Also a 40mm endmill is a pretty big endmill.Is it not possible to make this out of drill rod.
If I had to tilt the mills head over at 7 degrees and use a rotary table would I not be able to drill a tapered hole like that?. I am on a learning curve with milling set ups..If this would work how would I register the hole to the parallel hole to be consistent 10 times over
In other words if I had to drill a normal hole of say 35mm through the plate then how do I set the mills head over because now it would have moved over in relation to the cut I have just made?

Toolguy
01-21-2011, 09:13 PM
If you are just making tapered round holes rather than a shaped cavity with tapered walls, you can easily make a tapered reamer out of drill rod on the lathe and cut straight flutes in it with the mill and harden it. With more back clearance you might be able to mill with it too. If you drill or bore the holes to a little under the small size, then run the reamer at a slow RPM with cutting oil you should come out just fine. Then just set the quill stop to be the same depth for all 10.

PixMan
01-21-2011, 09:27 PM
Are you looking for 7 included angle, or 7 per side. I'd look at Conical Tool Company for the mill you need. Excellent stuff.

http://www.conicalendmills.com/default2.htm

SGW
01-21-2011, 09:44 PM
You don't need a 40mm end mill, just an end mill with the correct taper http://www1.mscdirect.com/CGI/NNPDFF?PMPAGE=485&PMT4NO=101400871&PMT4TP=*ITPD&PMITEM=04153102&PMCTLG=00
and a rotary table. It's complicated a bit because the diameter of a tapered end mill depends on where you are along the taper, but it's no big deal.

Center the rotary table under the spindle, and center the workpiece with the to-be hole centered under the spindle as well. Zero and lock X and Y.

Drill, say, a 10mm starter hole.

Swap the drill for the tapered end mill. Lower it into the hole. Unlock X, move until the tapered end mill begins cutting. Lock X again. Note the X position for future reference. Using the R/T, mill around the periphery of the hole.

Now, whichever you can do most accurately, either raise the quill or lower the knee to get the end mill out of the hole so you can measure the diameter. Figure out how much more you need to cut to get to 40mm diameter and add that to the current X position to get what your final X value will be. Don't forget that you need to add the RADIUS amount.

Lower the end mill back in the hole to exactly the same depth as it was when you did the first cut. Continue moving over the X axis and going around the hole with the tapered end mill using the R/T until you get to the X value you computed for a hole 40mm in diameter.

(If 'twas me I'd check a couple of times as I was going along to be sure it was progressing as I expected.)

dewat
01-21-2011, 11:34 PM
I hope I'm not suggesting anything too radical here, but I've made tooling out of case hardened cold / hot rolled. I see you changed the mold material to aluminum, if it's only 10 holes ( although large) and you mill at a low feed and speed it might work. It wouldn't take too much to make a smaller test tool and give it a try.

.

dewat
01-22-2011, 12:13 AM
I remembered making this tool about 3 years ago, for what I don't remember, it tapers from about 12mm to 25mm,

http://i81.photobucket.com/albums/j218/dewat/taper004.jpg

metalmagpie
01-22-2011, 01:53 AM
Know anyone with a Wolhaupter boring head? Those can bore tapers. Or, you could set up your part on a lathe faceplate and do the (short) tapers by running in the topslide.

You could mill a round hole, then slew a BP head over your 7 angle, put a small end mill in, get your part located on a rotary table, and mill your taper in one complete turn of the RT per hole. If you have a DRO it would be easy to then index to the next hole.

If you had a tapered endmill and your ODs were critical it would be tricky to plunge just so far and no farther. Actually, I think the easiest way to do this would be with a custom-ground tool. Have a T&C shop make you up a tapered reamer to size and angle, but one with a lip which would stop the reamer from going down past the desired size. Then just index to your drilled holes, and feed the reamer down until it seats solidly on the lip, then lift it and go to the next hole. Often times a custom ground tool is worth the expense.

metalmagpie