[digits]

Hi, I did a quick search, but I couldn't find an answer...

Is it possible to mill a 70mm diameter, 100mm deep hole in a block of Al (6082) with an X-1 sized mill?

I've never used a boring head before, but from what I have read, you have to start with a full depth pilot hole, and then bore it out slowly. Does this really mean than on an X-1 I'd have to bore up from a 10mm drilled hole to 70mm using the boring tool, adjusting it a tiny fraction of a mm per pass? Or can I get some sort of long endmill and just rough out the hole, and then just bore the last few passes for accuracy?

Thanks.

[phantomcow2]

Do you have the stock motor?
You should be able to use a 1/2" drill without an issue in aluminum. Drill that first, thats like 12.5mm.
Then see if you can find a set of drills with a 1/2" shank but increase in increments of 1/16". Go as large as you can, upping 1/16" each time. 1/8" might be okay.

Then, bore. The X1 should be able to do it. Just be aware that you will need a good size boring bar to get that depth and keep rigidity. See if you can find something with 5/8" boring bars.

Also, remember that you will need to take smaller and smaller passes as your diameter increases. I hope you are patient.

[sanddrag]

It's not what the machine can or can't do, it's the amound of time it can do it in. On the smaller machines you'll have to take lighter cuts. The method described above is good. But as drills get larger they get longer and you'll run out of vertical height. So you may want some large endmills to plunge straight down with, but finding ones with like a 5/8 shank is not going to be easy probably and it is going to be expensive. You could CNC the thing and do the hole with like a 1/2" endmill.

[itsme]

Hi there,

I've got a feeling that you might run out of z-axis for something like this.

I was recently drilling holes in a 130mm long aluminium block. Once the block was gripped in the vice, the top of it was at least 150mm above the table. I managed to get away with drilling a 6mm hole, holding the drill bit in a 6mm collet. When it came to anything else, where I needed to use the chuck (because i didn't have the correct collet size), it was hopeless. A 10mm bit was hopeless. Even in a collet, there wasn't enough z to get the bottom of the drill to clear the top of the work piece.

It's probably not impossible to do what you want, but I've got a feeling it would be a good challenge.

Regards
Warren

[digits]

Thanks for the replys guys

I have to admit that I haven't even got my X-1 yet, but I am planning to CNC it from the off. I guess I would need an end/slot-mill with a 120mm long shaft to cut this hole out without a boring head - and it seems I would run out of Z-axis with such a long mill

I think a boring head on its own would work, but it'd need about 200 passes to get from 10mm to 70mm dia, with a manual adjustment of the cutter after each pass - which kinda defeats the object of CNCing it in the first place!

I guess I may have to go back to the drawing board on this part...


EDITED due to lack of coffee before posting

[Deviant]

More than likely, you couldn't use a vise and get that depth. I'm not sure what the z travel is on the x1. But on my x2. When you figure the vise, material, boring head+boring bar. The z axis gets used up fast.

You could prolly get by with drilling out the part then inserting the boring bar into the part and mounting it in the vise. That way you don't have to actually clear the part with boring bar. I had to do that with my mill and a long drill bit. Inserted it into the part, then opened the drill chuck all the way. I was about to tilt/ease it into the chuck then drill the hole. I hope that makes sense.

You may have to bore it in stages. Which could cut down on your accuracy. Unless your very careful. Use a short boring bar to bore the top and a long boring bar for the bottom.

If this is a one off part, it might be easier to have someone on the forum make it for you.

*edit*

Blah, I meant to add that you can try mounting it directly to the table. Just make sure you don't drill/bore into the table. Maybe a piece of sacrafice material on the bottom.

[digits]

More than likely, you couldn't use a vise and get that depth. I'm not sure what the z travel is on the x1. But on my x2. When you figure the vise, material, boring head+boring bar. The z axis gets used up fast.

You could prolly get by with drilling out the part then inserting the boring bar into the part and mounting it in the vise. That way you don't have to actually clear the part with boring bar. I had to do that with my mill and a long drill bit. Inserted it into the part, then opened the drill chuck all the way. I was about to tilt/ease it into the chuck then drill the hole. I hope that makes sense.

You may have to bore it in stages. Which could cut down on your accuracy. Unless your very careful. Use a short boring bar to bore the top and a long boring bar for the bottom.

If this is a one off part, it might be easier to have someone on the forum make it for you.

*edit*

Blah, I meant to add that you can try mounting it directly to the table. Just make sure you don't drill/bore into the table. Maybe a piece of sacrafice material on the bottom.

Thanks, that all makes sense

The hole doesn't actually go all the way through the piece, so I was planning to clamp it down to the table.

I don't really have to make this in one piece - but I do need the bore to be as smooth as possible - it is a mounting for an air-flow sensor, and any turbulance will do nasty things to the readings

I am getting more and more tempted to start off with some 3.5" 1/4" wall tube and then just bore that out the last few mm - a 50mm boring head would fit right inside. I'd have to add some other milled parts on the outside of the tube to get my sensor mounts etc, but it might be less work overall...

[phantomcow2]

Your idea to start with 1/4" wall tubed is by far the way to go. YOu will have a lot patience left in the reservoir, and taking a tiny and slow cuts for a good finish won't be so annoying.

[digits]

Your idea to start with 1/4" wall tubed is by far the way to go. YOu will have a lot patience left in the reservoir, and taking a tiny and slow cuts for a good finish won't be so annoying.

Thanks - I've seen the thing professionally CNC milled in one piece and it just looked amazing! I'd be more than happy though with something that was quicker and cheaper to make that needed 2 or more parts though

I guess my next stupid question was going to be how to mill the outside of the tube to the required dimensions, but I guess I just have to turn it on its side and mill it front and back?

[digits]

Now that I've actually got my mill (though I've not milled anything yet!), I can see what people mean about the Z-axis disappearing. With an ER25 collet chuck and short 6mm mill, there's about 175mm between the end of the mill and the table. Add an milling vice and that drops to about 130-140mm of Z.

What I was wondering is has anyone tried raising the whole Z-axis about 50-60mm above the current mounting point? There is currently enough Z-travel to put the cutter about 50mm through the table, so apart from mounting and stability issues, I can't see any downside to this modification - am I missing something?

Cheers.

[dcprecision]

What you possibly may consider is using a 3/8" dia solid carbide boring bar in a smaller boring head. Carbide bars are 5X stiffer than steel ones so the finish is typically far superior. The rule of thumb for good finish is to bore 2x deeper than the bar dia with steel bars and 10x bar dia with carbide max. This rule is for steel parts,, you can go at least 30% deeper with aluminum parts.

If you make this as a 2 piece job,, sounds like the tube would lend itself better to lathe work rather than mill.

[digits]

What you possibly may consider is using a 3/8" dia solid carbide boring bar in a smaller boring head. Carbide bars are 5X stiffer than steel ones so the finish is typically far superior. The rule of thumb for good finish is to bore 2x deeper than the bar dia with steel bars and 10x bar dia with carbide max. This rule is for steel parts,, you can go at least 30% deeper with aluminum parts.

If you make this as a 2 piece job,, sounds like the tube would lend itself better to lathe work rather than mill.

Thanks - I was wondering if it's actually possible to interpollate larger bores with a boring head by spyrialing the cutter under CNC in X-Y and Z just like a long endmill. That way, I wouldn't have to stop and adjust the boring head on every pass...

I have no room for a lathe - and I'm saving my pennies for some aluminium to mill

[dcprecision]

I don't think that a boring head will work well in a spiral cutting mode and an end mill offers superior stiffness... Also,,I think that a lot depends on the rigidness of the machine itself....The further the head is away from the table the more flexible it gets.. Thats why a riser block on the column may not be a good idea. My suggestion is first to drill a 1/4" pilot hole then to use the largest screw machine length drill bit you can hold, probably 5/8. Then go to cnc with a 1/2" end mill to cut within .015 of final diameter and to finished depth. Then finish the wall id with a boring head. This way you can go through each step with as many parts as you are making then set up for the next tool. Once the boring head is set up,, you dont have to change its setting so you get repeatable accuracy. The finish will be very good because you can take a light cut with the boring head with the x y axis locked down for max rigidness.

There is no compromise for high quality tooling when doing professional quality work so anticipate having to invest a bit of money there,, probably more than you invested in the machine itself. Carbide insert tools are the way to go with boring bars and solid carbide bars are by far the best. Cost is about $ 150.00 for a carbide bar and a couple of inserts.. Another $ 75.00 + for a boring head, about $ 20.00 for a 5/8 drill bit and another 35.00 for a high quality carbide 3 flute 1/2" end mill.. so a $ 300 tooling investment is needed to make this step work... You may consider sub-contracting the boring head operation if you are not making very many parts initially. You could also rough out the holes on your mill to save money.

[philbur]

I'm not sure he would need to go to the expense of a carbide boring bar with carbide insert. The hole is 70mm diameter so using a boring head to only finish the hole, as you suggest, means he could use a home ground HSS "round" cutter directly inserted in the side of a 50 mm diameter boring head. That would be a very stiff stup.

Regards
Phil

I don't think that a boring head will work well in a spiral cutting mode and an end mill offers superior stiffness... Also,,I think that a lot depends on the rigidness of the machine itself....The further the head is away from the table the more flexible it gets.. Thats why a riser block on the column may not be a good idea. My suggestion is first to drill a 1/4" pilot hole then to use the largest screw machine length drill bit you can hold, probably 5/8. Then go to cnc with a 1/2" end mill to cut within .015 of final diameter and to finished depth. Then finish the wall id with a boring head. This way you can go through each step with as many parts as you are making then set up for the next tool. Once the boring head is set up,, you dont have to change its setting so you get repeatable accuracy. The finish will be very good because you can take a light cut with the boring head with the x y axis locked down for max rigidness.

There is no compromise for high quality tooling when doing professional quality work so anticipate having to invest a bit of money there,, probably more than you invested in the machine itself. Carbide insert tools are the way to go with boring bars and solid carbide bars are by far the best. Cost is about $ 150.00 for a carbide bar and a couple of inserts.. Another $ 75.00 + for a boring head, about $ 20.00 for a 5/8 drill bit and another 35.00 for a high quality carbide 3 flute 1/2" end mill.. so a $ 300 tooling investment is needed to make this step work... You may consider sub-contracting the boring head operation if you are not making very many parts initially. You could also rough out the holes on your mill to save money.

[dcprecision]

Mounting a cutter from the side may work, but it is close,,, the boring head will be about 50 + mm in dia with no offset and the cutter must extend below the bottom surface of the head to reach the bottom of the blind hole.... a custom ground cutter may be needed. Owning a good boring bar is not a bad investment for any holes less than 50mm in diameter...

[digits]

Wow, thanks for all the advice guys :cheers:

I won't have my metal for about a week, but I'm going to have a go at boring a deep 70mm hole in a square sided tall candle - I shouldn't be able to damage any of my tools with that, and I'll be able to recycle the wax and try different strategies

[mugabe]

Just got my boring head and made some tests . On X2 when head is shifted for greater diameter , it become unbalanced and machine vibrates at some rpm's in the middle. Should try to insert some counter weight to balance the head. I did not attach machine properly to the base - that could be another reason for vibration.

[Pres]

You got the right idea!
Make sure that boring head is balanced - or go VERY slowly (rpm wise).
Pres

[mugabe]

Thanks .

Will look for something like rod (to be inserted into the boring head horizontal hole) and balancing ring on it with locking nut to fix a ring on that rod. BTW, does someone sense the vibration of machines with some kind of electronic accelerometer for precision machine tuning/balancing attached to the spindle?

I ordered the cheapest boring set from little machine shops to study boring and that one is definitely not for alu. Lubricating help a lot but still is not the perfect (is not as perfect as it could be on machine with 35 microns spindle playing ) I so a number of pages on internet where it is advised to use cutting tools with TIx plating and/or core carbide mills with different shaping than for other metals. Is it possible to use indexable bore mills or go for something special and may be expensive ?

[lerman]

To rough cut a starting hole, try a forstner bit. I've gone to about 2-1/2 inches in diameter in aluminum without much trouble.

Ken