[tobyaxis]

Hello Everyone,

Anyone here try tapping 3.5M x .6 threads .16 deep bottoming in soft copper plate 1/4 thick? This is what the Boss wants so helicoils are out of the question.

First problem: When Drilling with a #30 stub drill the holes blow open to .137 diameter. I've tried slowing the speeds and feeds but the drill still packs with chips. Also tried using a 1/8 drill, and still no dice. The machine is a Cat40 HAAS VF-3 in very new condition.

Next problem: Roll Tap (Form) or Cut Tap? Which would be best?

All work has to be done on the CNC Mill in large quantities, and all ready scrapped 5 parts.

First time machining Soft Copper. Lost and Confused, and the Boss isn't happy either.

Thanks for the Information in Advance.

tobyaxis :drowning:

[kalmah]

First question:

- Which kind of drill do you use ??
Carbide, Coated carbide, HSS
- What is the lubrication ??
Cutting oil, Emulsion oil, Dry

For the drilling, there is two case:
If the lubrication is oil, a standard carbide drill works(be careful concerning the cutting oil, it can oxyde copper). It's better if the helix angle is 30-35°.
If the lubrication is emulsion use coated carbide drill with a low friction coefficient coating (DLC as exemple)

Don't hesitate to use pecking cycle.

For the tapping roll tap is a good solution when material is difficult to cut and soft.

[JFettig]

I've never really had these kinds of problems with copper, always used coolant and whatnot. I always use cold forming taps in copper(all my small holes) and they work great. They also bottom really well.

Is the drill your using center cutting, are you spotting it before drilling?

last time I cut copper I think I used a .11" drill, 3000rpm and about 6ipm taking .05 pecks(I took such a small amount at small feed because I couldnt screw this part up) and it came out very well.

What size pecks are you using?


Jon

[lgreeves]

Carbide is good for drilling soft material, use recommended surface feeds. Thread milling makes nice threads but a roll tap is the best choice of the two.

[kalmah]

OK you have never had these kind of problem with standard copper. A lot of drill works with standard copper.

Your copper, I suppose it's electrolytic copper, right ??
For your information it's more difficult to cut than standard copper. If the chip adherate to drill, the hole diameter 'll be too big. It's a standard problem with electrolytic copper.

Your cutting parameters are a little bit low but it's OK.

I've drilled electrolytic cooper without pecking cycle (lubrication: Emulsion oil) but the drill was coated with a new DLC coating. The drills diameter was closed to your case and the depth was 4xD. The results was very good.

If the surface has a good roughness and it's flat, I use standard carbide drill. it's not necessary to make a center hole. But for your case, I think that a center hole is necessary before drilling.

In my opinion

- Try to make a center hole before drilling
- Increase the cutting oil flow
- Use coated drill with high helix angle (as exemple: http://www.nachi-fujikoshi.co.jp/eng...ill/0501a.html)

PS: I don't work for nachi. I try to help you :cheers:

[tobyaxis]

Thanks for the fast response guys.

The Parts are for some kind of electronics assy. They get gaskets too.
I have no idea what for, but this is what they want.

The chips did pack the drill quite quickly.

Spot 1/4 dia. hss.
I used a #30 drill HSS 135 split point stubby for 3.5m x .6 Roll Tap.
Starting Spindle Speed was about 3500rpm and the Feed 7ipm.
Then down to 1000rpm and 2ipm.

I wanted to keep the chip load arount .001 to .002 per flute.

The peck was Q.1 and then down to Q.05.

Coolant was Water Soluable, not sure which brand.

The depth has to be .170, .01 different from my first post.

That Job has been put on the side so when it comes back I have to be Ready for it. At this point I'll try anything. I grabbed a sample to bring home to try in my garage, just an Enco R8 spindle Bench Mill.

I'll try all the suggestions made in this Thread

Thank You Everyone Very Much

TobyAxis :cheers:

[Rustybolt]

First off you want the hole a little big. As you found out dead soft copper tends to grab. In tapping copper 75 or 80 % threads are ok.If you try to to tap full threads you,ll break a lot of taps. I have had best luck with brand new regal-beloit gun taps, although any quality tap should do as long as it's sharp. Run your drill as fast as you can and peck cycle. I've used high sulfer and hich chlorine cutting oils, both to good effect, but whole milk seems to work best.

[M-man]

Check out the PRODUCT SELECTOR at this site http://www.dormertools.com/
It will get you the rigth tools and cuttingspeed for your machining operation.

[tobyaxis]

The Company I work for is cheap, the have millions but buy chinese drills.
????????????????
My Boss isn't a machinist either. Most management fails to realize that being a Real Machinist takes time and skill. Books do not tell everything. As for tooling. High production runs require good tooling (Precision Twist Drill, Sandvik, Seco Carboloy, Isscar, OSG, GreenLeaf to name a few). This isn't a real machine shop either. As far as Material for Fixtures and Hard Wear for Set-ups, none.
Looks like I've been handed a bag of rotten apples with instructions to make them ripe again. (chair) Ha Ha Ha. Started this job 3 weeks ago, and it looks like one more week. Already looking. Anyone looking for a Machinist in the New York Area?

Thanks Again Everyone, I used 90% of all the suggestions in my garage on the Mill and they worked nicely. :banana: (nuts) (group) :stickpoke

tobyaxis(still learning, the hard way)

[robertg991]

We used to use a product called Rapid Tap but don't think it is available any longer. Try some Tap Magic which I think still is. These are small 4 oz cans. To keep the drill from grabbing may have to flatten the flutes just a bit. These are old time solutions and may not work with cnc's. Haven't cut any soft copper in a very long time and all done with conventionals!

Good Luck,
Bob Garner