Smallest drill you've had success with on Tormach?

[doublesidedstickytape]

Hello, I have a Tormach 770 and there's a part I'm making where I need to drill a 1mm diameter hole at maybe 5x diameter depth. Part is aluminum. I was using some carbide drills off McMaster and I got through 1 part OK, but snapped both the drills I had ordered on the next one.

I was using G-Wizard feeds and speeds of 10000 RPM and 93.1 mm/min feed with coolant flood.

I was wondering what is the smallest hole you've been able to drill on a Tormach? I was thinking maybe some nice TiB2 coated Harvey Tool drills could get me through the job, I can't really see what's happening but I imagine edge buildup on the drill is a part of it. But maybe the rigidity and runout of the Tormach just won't allow micro-drilling?

Edit: I was using the ER20 TTS toolholders. Last I measured runout I was getting under 0.0005" on the TTS holder and about 0.001" on a short 1/4" endmill tool tip.

Thanks

Similar Threads:

• Newbie- Purchasing Drill Bits for Tormach 770
• Tormach 440 Part Success
• Tormach HSS drill bits
• What's the smallest drill bit you would try to resharpen?
• Tormach PCNC1100 vs CNC Mill Drill

[davidloomes]

Smallest I've done was 1.6mm at 10000rpm and 400mm/min. That was a very ordinary HSS drill for an M2 x 0.4 tap in 6082. Although my drill is bigger than yours, your federate seems very low to me. 93.1mm/min is only 0.00018" per flute/rev and 3 times that would seem like a good idea to avoid the cutting edges just rubbing. I was running at 0.0008" / flute / rev and that's as shallow as I've ever run anything.

Are you using pecking? To go that deep, I'd be looking for a peck around half of the diameter and a full retraction every 2 diameters.

Hope someone else has gone as small as 1mm and can give you more concrete nos.

[popspipes]

I just drilled .062 holes x .250 deep no peck 5100 rpm 2ipm.

I used oil though and not coolant, coolants I am familiar with cool fine, but leave a lot to be desired in the lubrication department.

[AUSTINMACHINING]

I've done. 016" holes on a face tilted 20 degrees from horizontal .25" deep. Spot drill face to guide drill then peck to depth. The drill is so small, can hardly see the flutes. When i fist saw the drill, I thought "no way this is going to work ". But it did :-)

[MichaelHenry]

The smallest I've drilled was 0.025" through holes in 3/8" thick 6061 using a carbide drill bit. Overall there were a few hundred holes drilled and I'm not sure that any bits broke. I used a Royal sensitive attachment in the spindle with an Albrecht keyless chuck to drill around 30 holes in each part with the program in step mode. I'd let the program run until it hit the 1st hole, put it in single block mode, manually drill the hole with the sensitive, single block to the next hole, manually drill, etc. Each hole took less than 30 seconds to drill once I got the rhythm right.

Not my video but this may help explain:

[rajeevdmg]

Hello, I have a Tormach 770 and there's a part I'm making where I need to drill a 1mm diameter hole at maybe 5x diameter depth. Part is aluminum. I was using some carbide drills off McMaster and I got through 1 part OK, but snapped both the drills I had ordered on the next one.

I was using G-Wizard feeds and speeds of 10000 RPM and 93.1 mm/min feed with coolant flood.



I was wondering what is the smallest hole you've been able to drill on a Tormach? I was thinking maybe some nice TiB2 coated Harvey Tool drills could get me through the job, I can't really see what's happening but I imagine edge buildup on the drill is a part of it. But maybe the rigidity and runout of the Tormach just won't allow micro-drilling?

Edit: I was using the ER20 TTS toolholders. Last I measured runout I was getting under 0.0005" on the TTS holder and about 0.001" on a short 1/4" endmill tool tip.

Thanks

I drilled dia 0.3mm in hardened HCHCR steel, thats material used to make plastic molds. Depth was3-4mm. It was around 20years ago and it was my first job on Machinist. It was done manually and we can feel the force being applied to the drill. You feed it and then use a hand blow pump to remove the chips. The holes were used to feed hot molten plastic to the mold cavities of watch components. HSS drills as per my memory as carbide was not in fashion much that time. Am i getting old????
Edit1-machine was MAHO - and it was having a quill for this type of work. Rom i dont remember. But maximum rom will be pretty low as it was fairly old machine but in good condtition. Small Maho CNC machine retrofitted with Fagor control with fancy canned cycles with pics.

[jwatte]

I still like HSS for drills, as it flexes without breaking when there is any kind of side force...

[rowbare]

Look for parabolic flute drill bits. They do a better job of clearing chips.

bob