Drilling on center

[sandrewb]

Hey My first Post

I need help drilling 2 holes, 1 from each end and them meeting on center. The first hole is 7.2mm diameter and 16mm long. Second comes in from the other end when the part is flipped around and is 8mm dia and 47mm long. Using carbide drills.
Not sure what the material exactly is but its gumy and the part is previously made by extrusion then we turn and drill it. Using a hyundai lathe.
As you can tell im kinda new to this and any help would be awsome.
Thx.

[christinandavid]

Is it feasable to drill the 7.2mm hole from the same side as the 8mm hole?

DP

[sandrewb]

Not sure if i can. The part needs to be turned on both ends and located off the center of the part. Also at the moment settings are 3000rpm with a .2 feed... No pecking and making a good chip isnt happening. Should it be faster?? slower?? and is not pecking a bad idea here?

[christinandavid]

If the part is an extrusion then the material may possibly be too ductile to chip if it gets hot. It will get hot if you are running at 3000rpm with no peck unless you have good thru-coolant. I would peck, personally.

Are you having concentricity issues also? Start the hole at a lower feedrate to give the drill a chance to find its centre.

DP

[neilw20]

If you really want the holes to line up center drill before you do the 7.2mm and peck drill if the chips are not coming out nice.
3000 is way too fast but may work if coolant is controlled well.
Inspect the chips to see how well it is cutting.
You really need to drill through with the 7.2mm - get a longer drill.
Does this material need carbide? Consult a tooling supplier for the best drill to use.
The speeds and feeds best found by consulting a tool supplier who knows his stuff.

[sambo67]

I agree with Neil , if possible drill the smaller hole thru then flip part. Rpm really to fast and carbide drill to costly when really not needed

[wildwestpat]

Hi Sandrewb

1. Check that the tailstock is correctly aligned with the head stock. The center height also has to be correct as well as the lateral offset. Make sure the bed is clean and the tailstock guides as well and the tailstock clamp is hard on. Any errors are magnified and the holes will not join up also the drill may be broken as it breaks through on the second drilling as the 'holes' do not line up properly. The errors are magnified by the depth of cut. (I am assuming that you have sussed out how to centre the work on the opposite sides. This is a bit of a problem as the alignement is both on center as well as the axis of rotation - my suggestion is to facing off the parts between centres using a half centre in the tail stock - face off both ends this way to the correct length - leave the center dimples in place for the drilling operation.)

2. Use an appropriate sized center drill with minimal over hang on the tail stock which should be tight to the bed and have the clamp on the feed on sufficiently to make advancing the drill a bit of an effort. Once the hole has started cutting on the parallel part of the drill for a few mm the clamp can be let off a little but do not touch the tailstock / bed lock.

3. Make sure the drill is correctly sharpened for the material being cut and the swarf if being ejected properly. You will possibly have to keep withdrawing the drill during the operation to lubricate and clean off the swarf.

4. Some extrusion materials are not easy to machine as they are very soft and wrap the cutting edge of the drill. Attention to the drill tip angles should help as should the use of lubricant and suitable feed rates and speeds.

5. The diameter to depth is approaching 1:10 which is going to be difficult as a one shot drill from the first side. The double approach would be better if the depths were equall as this reduces the diameter to depth ratio to 1:5 which is going to be easier but still demands care.

6. An end mill of smaller diameter say 5mm used as a pilot for the twist drill might be a better solution.

Hope this helps - regards -Pat

[sandrewb]

Hey thanks for all the help guys. Im kind of the second man on the job so what i say doesnt go but i can make suggestions. Just got home now and reading posts. Today I slowed the feed rate down to start the hole then sped back up to finish on the long 8mm drill. Also RPMS increased to 4500. Havent did a whole lot of testing on the part yet but we will see what comes of it. We definitly are having concentricity issues and thats the problem. This isnt a 1 time part its a very high quantity part that needs to be produced accuratly everytime. I mentioned about going all the way through with the 7.2 drill first then coming back with the 8 but they were worried about the edges of the 8mm drill wearing to fast. This is on a CNC lathe so if 3000rpms is to much and its been increased to 4500rpms.. Please give me some new ideas on feeds and speed to give a shot. Thanks for your interest and advice.

[packrat]

<SNIP> We definitly are having concentricity issues and thats the problem. This isnt a 1 time part its a very high quantity part that needs to be produced accuratly everytime. I mentioned about going all the way through with the 7.2 drill first then coming back with the 8 but they were worried about the edges of the 8mm drill wearing to fast. <SNIP>

I would drill the 7.2mm through and then Ream the 8mm diameter and depth in the same set-up. The 0.4mm per side is about the right amount of stock to remove on that size hole with a reamer, so no worries about wear. And that would also get the bores concentric.

cary