Value of CNC Machines

Hey JR,

That sounds like half my customers. I am at one right now I could use your help with. The machine is a Ganesh semi swiss machine. The material is A286. The part gets turned down from .787 to .35 x .38 deep. There is a drill operation and a 1/4-28 double lead tap operation. There is some milling, and sawing as well but my 2 problem areas are rough turning, and tapping. Any ideas?

A286/A287 is also called 347 Stainless.

M. A. Ford makes a line of drills that worke very well in 347 SS and form/roll tapping with oil is the ticket. Cut taps are problematic.

Thanks JR,

Definitely using oil. I am going to try the Ceratip. And I think I will bore the hole before tapping.

Its good to have a tooling guy back JR.

Any comments on the Ganesh machine and the Ganesh organization? I've got a buddy in a prototype shop in SLO that is considering a CNC lathe from them.

Might be nice to comment in the thread: Comments on Genesh Machinery

Thanks, Steve

snipped-for-privacy@earthlink.net wrote in news:9320829d-c342-4b82-8536-72d48a94bdc7 @p10g2000prf.googlegroups.com:

Sandvik GC1105 grade insert for turning.Small machine & small part so I would probably use a CCMT3121-MF or something like that for roughing,

Tap at around 8 SFM. Maybe 10 SFM with a coated tap. Don't pussyfoot around when drilling the hole. A-286 will work harden some.

Use cutting oil if possible.

Thanks Dan.

Garlicdude wrote in news:ILednbbhatPpkhfVnZ2dnUVZ snipped-for-privacy@posted.southvalleyinternet:

I have a couple of cutomers that have them and have seen them running out in the field. I asked one guy in Cincy how the service and support is and he said "WHy? Are they offering that as an option now?" But they really like the machine. They run 24/7 mostly unattended. The machine sounded quiet and smooth, rather unlike most of the Chaiwanese machines in that price range. They are cutting an fairly open tolerance brass part on it that used to be run on a Brownie. So nothing real difficult.

OTOH, we replaced one locally that the customer ended up sending back. They couldn't get their part running on it.

The difference is in the abilities of the people programming, setting up, and troubleshooting the thing. If your buddy is a hands-on guy that can figure things out on his own then it might be worth a shot. Otherwise he should buy a better supported brand.

I don't think there is one Bill. I turned a 400 pound piece of this stuff into a forty pound part recently and it basically sucks. The one thing I did learn was how to drill it and to form/roll tap it. It's abrasive as hell, extremely ductile and work hardens if you look cross eyed at it.

This is a high production aerospace shop. One operator for 3 to 5 machines. The challenge isn't so much getting the material off the part. The challenge is getting the material off the part as fast as possible with the longest tool change frequency. I've cut all the nasty stuff before, but my philosophy was inexpensive inserts, a corner per part or two and a dedicated operator changing tools. My goal is to minimize the cycle time and maximize the tool change frequency time. If I accumulate as much data as possible I can go into the customer with a plan A-Z and in the end it is what it is.

snipped-for-privacy@earthlink.net wrote in news: snipped-for-privacy@m73g2000hsh.googlegroups.com:

No sweat. Try the Sandvik insert. I've had amazing results with it. They used to have a pdf on their site with speeds and feeds but I couldn't find it. I would start at 200-300 SFM and see how it goes. Otherwise I would run an uncoated tool at 150 SFM.

The "MF" geometry has a tight chip braker, positive rake, and is sharp enough to shave with in GC1105.

"John R. Carroll" wrote in news:fM1jk.17396$ snipped-for-privacy@nlpi069.nbdc.sbc.com:

If you form the threads rather than cut them just be aware of the work hardening, I ran some threaded A-286 parts about 8 years ago using an axial thread rolling head. I couldn't get rid of the taper. As best as I could figure the material would work harden and by the time the rolls got to the end of the thread the head would flex open a bit. I couldn't make good threads to save my life. I had thread rolled A-286 several times in the past and it worked great. This thread was just a little too long I think.

I had the Fette guy in to have a look and he gave me a larger head to try. Same deal. They never came up with a fix.

I've always had good luck with roll form taps but I imagine if the thread were long enough you would see the same problem.

Most of what we did was an inch or less deep and from 8-36 through 1/4-28. There weren't more than forty of any one size. Balax is right up the pike so I bought some Emuge's and had them Firex coated. Each hole was checked all the way to the bottom and they gaged properly. I'll keep an eye out for this in the future.

In the mean time I'm stickin with "it sucks" whenever asked. LOL

"John R. Carroll" wrote in news:kr4jk.18694$ snipped-for-privacy@flpi146.ffdc.sbc.com:

I owuld think the first sign would be the tap breaking, but you never know.

Yeah, It's not the worst stuff in the world, but it's far from the best.

.18694$ snipped-for-privacy@flpi146.ffdc.sbc.com:

Dan, I have not form tapped a Double Lead Thread. I would think in this material the torque going into the tap shank at that course of pitch, breakage is very evident. What do you think? Thanks, Jim

JRWheels wrote in news: snipped-for-privacy@e53g2000hsa.googlegroups.com:

I've never form tapped a double start thread either. While it's a fast lead, it's also a shallow thread so it might work. A-286 is ductile and I've found it rolls better than it cuts. But work hardening can be a problem.