Dowel holes reamer or interpolation?

Hello

Thank you for reading my question

I would like to know what is your preferred method to drill dowel holes

On the job I am machining now I have 2 blind dowel holes Ø3 x 8mm deep on aluminium

The tolerance about positioning, is not stated on the drawing, we only have a general tolerance box in which it states +-0.1

These 2 holes are not aligned and they are also on 2 different heights (surfaces) one is about 5 mm higher than the other

Since we do not have a proper tolerance on the positioning, I think these 2 holes are independently from one to an other, I mean I do not think we have a part that fit on it, with the same holes positioning, but this is only my guesswork (deduction).

In my company they always interpolate this kind of dowel holes with a 2.5mm carbide slot-mill, and we drill it 2.8 first, even on holes deeper than 8mm, the reason why they do in this way is because they are worried that with the reamer we will not get the right position.

What is your preferred method to drill dowel holes?

I did drill the same kind of dowel holes, on a steel 14mm deep through.

Even in this case they had programmed with interpolation with 2.5mm slot-mill, and I decided to do it with the reamer instead, and it worked very well, and in this case we also had a proper tolerance on the positioning, 0.02mm circular rad.

I think if you check the run-out of the spot-drill and the reamer, regarding the drill even though it will not run very through, should be ok, since it will follow the spot-drill.

And also make sure the spindle inside and the holders are properly clean, with the reamer should always be ok to machine this kind of dowel holes.

What sort of holders do you use for the spot-drill? Do you use collets?

What sort of run-out would you consider ok to machine this kind of holes?

Any suggestion according this matter will very appreciative

Thank you in advance for your help

Hoezap,

welcome to the world of geometrical tolerancing and true position.

You are right to say that since the drawing does not call for a positional tolerance and if the holes are positioned off of an edge or face datum, they should be independent of each other. Ultimately your contract is the clients drawing.

If the drawing box say +/-0.1 then your hole centre will need to be within a rectangular tolerance band equal to that. Unless there is a note specifically asking for the two holes to be positioned relative to each other or you have dimensions to that effect, they can be independent.

Now here is why you use interpolation for holes on machines that are good:

Traditionally toolmakers on manual machines would clock up a workpiece then spot drill, drill a hole something like 0.5-1mm undersize, run an undersized endmill into the hole to get accurate position and finally follow up with an accurate reamer. Reamers are very flexible and very prone to breaking if you get the feeds wrong and they do not dictate the position of a hole. That is why there is a thing called a floating reamer chuck.

With CNC machines now, you do not need to do all the steps above, a single endmill can do all those. This also allows you to use any endmill you want for a hole by using cutter compensation. With CNC machines now being able to get H7 accuracies without issue, it makes no sense to drill and ream. There is however the issue of cylindricity when interpolating. Any backlash will cause your hole to not be perfectly round. If the drawing has an (E) denoting envelope in the dimension, you may be stuffed, if not then fair game.

On my home machine I will still do the old fashioned way to be honest but when I go to suppliers, I demand the new way to minimise my costs.

If you want low runout tool holding then you should consider collets. I personally have shifted to ER collets for everything as I could not find cheap keyless chucks that would give me the same confidence. If you want even better runnout, then you go for shrink fit holder. The collets I stock and use are all to DIN 6499 / ISO 15488 Form B that calls for a runout of 0.01 or better if I remember correctly. Your spindle should be better than that though since you are running 2.5mm endmills which will require high rpm.

Quote:

---

Originally Posted by komatias

Hoezap,

welcome to the world of geometrical tolerancing and true position.

You are right to say that since the drawing does not call for a positional tolerance and if the holes are positioned off of an edge or face datum, they should be independent of each other. Ultimately your contract is the clients drawing.

If the drawing box say +/-0.1 then your hole centre will need to be within a rectangular tolerance band equal to that. Unless there is a note specifically asking for the two holes to be positioned relative to each other or you have dimensions to that effect, they can be independent.

Now here is why you use interpolation for holes on machines that are good:

Traditionally toolmakers on manual machines would clock up a workpiece then spot drill, drill a hole something like 0.5-1mm undersize, run an undersized endmill into the hole to get accurate position and finally follow up with an accurate reamer. Reamers are very flexible and very prone to breaking if you get the feeds wrong and they do not dictate the position of a hole. That is why there is a thing called a floating reamer chuck.

With CNC machines now, you do not need to do all the steps above, a single endmill can do all those. This also allows you to use any endmill you want for a hole by using cutter compensation. With CNC machines now being able to get H7 accuracies without issue, it makes no sense to drill and ream. There is however the issue of cylindricity when interpolating. Any backlash will cause your hole to not be perfectly round. If the drawing has an (E) denoting envelope in the dimension, you may be stuffed, if not then fair game.

On my home machine I will still do the old fashioned way to be honest but when I go to suppliers, I demand the new way to minimise my costs.

If you want low runout tool holding then you should consider collets. I personally have shifted to ER collets for everything as I could not find cheap keyless chucks that would give me the same confidence. If you want even better runnout, then you go for shrink fit holder. The collets I stock and use are all to DIN 6499 / ISO 15488 Form B that calls for a runout of 0.01 or better if I remember correctly. Your spindle should be better than that though since you are running 2.5mm endmills which will require high rpm.

---

Dear komatias

Thank you very much indeed for your Great Teaching

an other issue you get with the interpolation is the hole will be conical and you will have to finish it with a reamer any way


for a Ø3mm hole 8mm deep you can go straightly with 2.5 slot-mill as you say, and even though you will have to reamer it by hand to make it cylindrical, you saved time at the end… would you agree with me?
But with a Ø3mm 14mm deep, you need to grind the shank to interpolate it and reach this depth
I did always use reamers, if you’ve got a spot drill that run true and the same with a reamer it works

Nothing great but thanks for the compliment.

you right that you risk making the hole conical. but that is why you would run a number of spring passes. Personally I do not like to run slot mills in plunge mode as you get birdnesting even if you peck drill. With 2-3mm endmills though you are correct, if you do not need to have an accurate position, spot, drill, ream.

Thank you!