Setting up a tapered cutter

[cybeeria]

I am a recent convert to CNC from manual milling and am faced with cutting a tapered hole. I am using a 5 degree end mill. I have done this in the past manually by careful measurement and going slow. My question is how to set up the cutter in the software. Since it is tapered, the deeper I place the cutter, the bigger the hole becomes. Where do I measure the cutter? Do I just pick a spot on the cutter and measure it and go from there? Is there an elegant solution to this? I need to make many repeated cuts that will have to survive a couple of tool changes so some clever way of determining depth(and width) of cut would be very helpful.

Thanks for the help!

Bill

[HuFlungDung]

I usually use the tip diameter of the cutter as the reference diameter. This can be difficult to measure it it is a 3 flute though. I typically assume that the stated tool diameter (from the catalogue) is exactly correct.

Then, offset the profile of the tapered hole by the radius of the tool at its tip. You can then break or divide up this offset line to create your Z levels. Be sure to check that the horizontal X (or Y) component of the offset equals the radius of the tool tip. If you do a parallel offset by the full amount of the tool radius, chances are that the horizontal component will be too long.

If it is a more complex issue, posting a picture or a dxf of what you have accomplished so far in cadcam would be helpful.

[Isoprenia]

I find that CAD is very handy to do the trigonometry, assuming the angle on the tool is accurate, I start with the end diameter, accurately drawing or modeling in a good cad system I find often helps thinking through the logistics of complicated cuts. It isn't always necessary to draw the entire part, just a detail of the featrues you are working with. Dimensioning usually does all the trig, and provides enough info.

hope this helps

ps great avatar and handle Hu Flung Dung

[Geof]

I have "calibrated" tapered cutters and tapered holes using a steel ball. Just write a short MDI program to interpolate a hole about twice the middle diameter of the cutter in a small piece of stock which has been faced off. Set the end of the cutter at the faced surface for your Z zero. You are not worried about getting it exact but you do want a size so that a standard sized steel ball will drop partway into the tapered hole. Measure how far the ball protrudes above the top surface. You can calculate the hole diameter and depth at the point the ball makes contact and from this you can calculate the Z position and radius for a particular diameter at any point down the taper. In addition you can calibrate all the extra cutters and determine a correction to the Z zero which is based on the end of the cutter. Now when you replace a cutter you just have to correct the Z zero for that cutter.

I don't know if this can be considered elegant; I do know it does not take as long as its sounds and it works.

[Dawson]

I find that CAD is very handy to do the trigonometry, assuming the angle on the tool is accurate, I start with the end diameter, accurately drawing or modeling in a good cad system I find often helps thinking through the logistics of complicated cuts. It isn't always necessary to draw the entire part, just a detail of the featrues you are working with. Dimensioning usually does all the trig, and provides enough info.

This is what I do also. I'll draw up the tool assuming it will be as ordered, then get a side view and transform the cutter until it's diameter matches the model. Dealing with cutters that aren't ground to a point takes more work like described in the thread above me. To simplify production I require all tools be ground to a point unless they are specials. I try to avoid the specials, but I have 1 job currently that uses them. In this case I have 2 cutters, one for roughing +.005 and one for finishing. We've had the same tools for the last 3 years (100 parts or so).

The fun comes in getting a 100deg c-sink to have a finish diam. of +/-.005 on slightly contoured surfaces with a 3-axis mill. Most of the time we get it close, then use a hand drill with a micro-stop.