Tapered Hole

[feinddj]

Is there any easy way to drill a tapered hole without getting a tapered mill? I have been trying a two rail sweep in Aspire and I am not seeming to get the right result. the hole starts at 2.023 inches wide and has a 4 degree taper with a hole depth of .5 inches.

Help is appreciated.

David F

[Brady Watson]

You could do a stepped taper if you offset your 2.023 circle to the inside a few times & then do an inside profile cut on each individual circle at whatever depth you are comfortable with.

If you need an ultra-smooth result, then - no...you really can't do this without a tapered bit.

-B

[tmerrill]

Hi David,

Creating the tapered hole in Aspire is easy, but as Brady said the challenge will be the cut quality trying to machine near vertical sides with a 3D toolpath.

There would be two approaches in Aspire, the 2 rail sweep as you said plus the Create Shape tool which would be my preference for something like this.

Pictures should show the setup and results, plus you can download the file here if you want to take a look at it:

http://dl.dropbox.com/u/8954669/Hole.crv3d

Tim

[garyc]

David...
An off the shelf solution (that violates your "dont buy a tool" rule) is to use a Ballnose EM that tapers from 1/2" (shank) to 1/4" (ball) in 1 1/2" CEL. Has a taper of 3.58`. Over 1/2" depth, not tooooo far off.

[feinddj]

Thanks for the thoughts. I think I will go with Brady's method and then sand to smooth. Don't you just hate taking a simple job and then finding that its really hard?

[srwtlc]

I was drawing this too while Tim was and came up with the same approaches. My question for the Vectric crew though, is (I know that it has to do with the pixel makeup of the wall of the hole), could there be a way to force an offset type toolpath to maintain a Z level for each pass around the wall? As it is, and I've run into this on some platters that I've made, that as the toolpath goes around for each pass, the Z level changes many times making for a jerky jiggly cut and highly excessive cut times when it would work to stay at that Z level for that pass and so on for each level. Kind of hard to explain, but if you develop an offset toolpath of the hole and zoom in on the visible toolpath, you can see that it is jagged or zig-zaggy up and down. Guess you would call it a Z level finish toolpath.

Agree with Gary, though it may cost more for the right tool, the time involved in a 3D toolpath (especially if many are needed) would eclipse the cost.

[donchandler]

If you pocket out a 1.75 id hole then run this program you will have your tapered hole. This is easy to do in the old vector program.

[srwtlc]

Way to go Don. I thought about pulling out the old 'swiss army knife' VectorCam too, but no one knows what were talking about anymore when we do. ;)

[myxpykalix]

Not understanding your toolpath description "you can see that it is jagged or zig-zaggy up and down" I was wondering if it might be easy to program a very tight spiral toolpath as if you were cutting threads, that would run the toolpath around the perimeter of the wall in a circular toolpath pregressively going down as it does. That would seem like it would keep the wall clean?:confused:

[srwtlc]

Sorry Jack, you would have to open Tim's file in Aspire and generate an 'Offfset' 3D finishing toolpath to see that result.

[feinddj]

Don,

How did you make this? I need to cut several of these and have just spent a fair amount of time doing it with 1/8th inch steps in Aspire. Would love to know how to do it another way.

David

[garyc]

Or....
A hand coded file that does a spiral down inside the small diameter at the bottom. Starting at the bottom do additional step paths .015 higher and .002 larger diameter until you exit the top. (If my math serves me right)

[Brady Watson]

Why the adversion to using a tapered bit? That would be straightforward, consistent and accurate.

You really don't want to use a ball end mill for this because you will wind up with a 1/2 ball radius at the bottom that you'll have to mess with and clean up.

If you have a 2.023" circle at the top of the material block and you taper it towards the center 4 degrees over 0.5", then the circle at the table/bottom of the material would be 1.953" in diameter, for a difference of 0.070" in diameter. You are really only shaving off about 1/32" around the entire circumference to get that taper.

This means that if you cut the 'top circle' at 2.023" at a 1/4" deep, and then cut the bottom 1.953" circle at 1/2" deep, you would only have a 1/64" step/waterline mark in the middle...which is next to nothing to clean up.

Unless I am missing something...this is pretty straightforward with a square end tool.

-B

[bobmoore]

I would take an inexpensive 1/2" end mill with a 1/4" shank and have my tool shop grind a 4 degree taper on it, like a reverse dovetail bit. Bob

[feinddj]

As with many things that I get asked to do, the client is picking this up on Sunday afternoon, a one day turn around for the piece, requested after 5 on Friday. So no time to order tools or even have a machine shop modify one. The job is done, the client will be happy and if I have to do again, I'll charge more.

[myxpykalix]

Next time you need to add in the cost of "tech support", because I don't know about these other guys but i want my nickel payment!:rolleyes::D

[feinddj]

All contributors must show up for payment of their nickle in person. Heck, I might even buy you a beer.

[donchandler]

Don,

How did you make this? I need to cut several of these and have just spent a fair amount of time doing it with 1/8th inch steps in Aspire. Would love to know how to do it another way.

David
I did it in Vectorcam 9. real easy to do.
I don't have Aspire or Partworks and from all the comments here on things like this, I don't think I am missing much.

[bleeth]

Regarding the jumping z at borders or sharp inclines:
Sometimes running a couple smoothing passes on the relief will help this immensely. Another "trick" I use when it it a raised relief is to inset my outer vector border a tiny bit and use that vector to define my cutting area. That way the software doesn't know it is cutting to the edge. That couple thousandths is usually not critical on most projects.
Solving that for an offset "bowl" cut would be a nice hit.