Drilling Conic Holes

Something like this?

http://www.hales.com.au/product.php?product_id=209

If I understand correctly the small side of the taper is to the side from where the machining can be done.

You therefore would require a dove tail type of cutter.

Ask your cutter supplier what is available for the material you want to machine.

your idea of drilling a 9mm hole and then finishing by moving the cutter in circles should work. just remember that the diam of the circle would be limited by the shaft size of the cutter. that is almost a 3mm diam circle with 6mm shaft and that will only give 12mm on your 9mm max cutter.

A disk cutter with circles spiraling down and out may also work.

What about drilling a 14mm + hole and inserting a tight fit inside tapering sleeve?

Hello!

thank you so much for your answer!

It helped me a lot!

Well, duh! I missed the reverse taper part (must remember to pick up my neuron from the cleaners).

Can you use EDM? That does the job nicely, albeit a little expensive.

Did I miss something?

Don't you need to know material thickness or angle of taper to choose a process?

What is the material?

Hello!

The material is cast iron!

Thank you!

I tried it in ACAD and if you use circular interpolation, a formed milling cutter (suitable to the taper) and having diameter of cutter 9mm and spindle dia 4mm

However whether it can be rigid enough to do the machining or not depende on the depth and taper angle.

Is the hole blind or it can be drilled from other side ?

We have a component spot faced like this (but only a few mm deep) and we use formed cutter as shown, Some times we also go for a single point tool, both times with interpolation , But the diameter is not so small it is about 1".

You may better consider EDM if the resource is available and feasible

hello!

For the beginning, it's helping me VISUALISING some drawings in ACAD!

I've considered EDM, but I have to limit my manufacturing proccess to cutting one. I try to solve this problem using just milling and drilling actions.

I'm restrained to do this, due to the context!

Thank you!

An old fashioned boring bar would do the job but it would be a small bar & might chatter a lot cutting cast iron.

Georgina,

A lathe and a boring bar may be a good alternative, if you can fit the part into the chuck. The turning can then be done with the compound rest. Custom cutters can give you various offsets if you are forced to create a reverse taper as shown in the CAD picture that was posted. To chuck the part into a lathe it is recommended that all the outer edges of the part are square to the face if a 3 (round parts) or 4 jaw conventional chuck is to be used.

You may need to look at what the advantages are as well as looking at the possibility of turning the part over and machining from the other side, if you have a reverse taper scenario, watch datums and surface availability for clamping.

Tapered milling cutters can be used if a cnc will interpolate, ie. touching the inner circle only on one side, it defeats the purpose of the CNC a bit, unless you would do this for "Lay" or surface finish purposes.

Tapered Reamers are available, but generally are only intended to remove minute amounts of material, ie .040" or less / diameter, these are mostly helpful when finishing a hole, improving the surface finish, or dealing with small tapers and small holes.

A tapered milling cutter plunged into the center of the hole is not recommended, as it may have a tendency to bind at full contact and snap into pieces, for small diameters with the correct speed it may work, again - not recommended.

Paul,

Of course generally the machine shop will supply the part drawn, if it is manufactureable, also this may limit the economics of making the part, as the machine shop may only have certain machines available. If they do all the deciding then we do not need the Junior Engineer! If you were referring to an internal machine shop in a larger plant, then OK.

Let the engineer do the research to design it right first, when he arrives to the machine shop, he doesn`t need to have his parts made twice, perhaps the machine shop just needed the money, or will just go along. Most shops I know are pretty good, but times are tough! Tool-makers are known for their jokes played on unsuspecting Engineers and apprentices. Know what you are talking about to a certain degree will save the wool from getting into the eyes!

Mirco.

My real point is that as an engineer avoid making features like this. There are always several ways to get the same job done. A reverse tapered pocket is a bad decision unless you have an absolute need for it. If it is a thru hole then the taper should be done from the other side and geometry of the part will dictate the holding fixture required for the part. I just can't see the reason for creating a blind reverse tapered hole and the part may need to be an assembly of some sort to accomplish this at a reasonable price. My point is redesign the part and avoid the problem all together.

As earlier said, we do have this design in a few of our products, the depth is very small- milimeters and fusnction is simple- for a o ring seal to seat the reverse taper- may be - (never got the answer from the designers- the original designers have retired) ensures that the expansion is in that portion of the metal and no projection is there and also the snug fitting of the seal - something similar to Circlips

Note the depth is small- and as explained we do in two different ways -

using a microborer with single point tool or with a formed mill with interpolation- depending on the position of the resource at the given moment (the said tools may be engaged in one of the other machines)

the original thread owner never told the depth of the conical hole, hence can not guess the purpose, but this is the likely reason.

In certain designs there may be an extra factor coming in where a flange may seat over and may try to dislodge the O ring, In this case the O ring diameter being more than the minor dia of the cone helps in avoiding the squeeze (my guess) this model is also existing in some of our applications.

Hello giorgiana:

You have had some good advice on this by people who know what they are talking about.........

Can you send a picture of the item that needs to be drilled?

And, if you are the designer can you not design this in (or out!) at the casting stage?

Please send a picture if possible. It would be interesting and be obviously more easy to choose a particular way to do the conic hole.

Take care and have a wonderful holiday!.............

There are taper drills and taper reamers are available in the market. This hole can be done from opposite direction.