Hi,

Being very new to machining, I have very little idea what to expect. I bought a Sherline 2000 CNC mill several years ago and did not have the time to use it much. Now I am retired or retarded or something like that and have more time...lol

I just replaced the computer and bought Mach3 and a new driver box. I have most of this up and working except for the limit switches.

Should I reasonably expect to cut a 2" X 4" X 1/8 T shaped flat part from 303 ss ?
Thanks,

Billy

Should I reasonably expect to cut a 2" X 4" X 1/8 T shaped flat part from 303 ss ?

Hi Billy,

What you have is basically a hobby style machine, it is far from being an industrial model but...
Taking it steady with lots of coolant (to avoid hardening) you should be able to profile cut 303 SS but remember that cutter size, spindle speed, chip loading and feed-rate all need to be very closely controlled.

SS is not a material I would want to machine with a Sherline but I am sure there are many members here that have and will sing it's praises.

Tweakie.

Hi,
SS is very tuff material to cut, it work hardens like hell.

The temptation is to go for extremely light cuts but it doesn't work, the tool just gives the material a 'damn good rub' and work hardens it.
I would be looking to get a feed rate of 0.5-1 um per tooth per rev.  With a 1/8 inch two flute endmill spinning at 6000 rpm for a surface speed
of 56m/minute which is right for austentitic stainless you'll want a federate of 12mm/min for a chip load of 1um per tooth per rev. Very slow, you
can up the feed rate but the risk snapping the tool.

Another temptation is to increase the rpm, if you up the surface speed against stainless you will fry the tool. You'll want coolant anyway but if you try to spin
too fast it wont stop the tool from cooking.

I don't know what sort of torque your spindle has but it will want plenty, if it stalls the mill will overdrive a stalled tool and snap it before you can blink.
Ask me how I know.... In the end I made a high torque low speed spindle based on a 1.8kW AC  servo and a RegoFix ER25 collet holder.  Even though
the servo and drive was second hand it cost me $2000NZD to make it. It makes mincemeat of steel and stainless. Problem now is......rigidity; trying to
hold the thing steady!

Thanks guys,

I  don't normally have much need to cut stainless. I do have the need to cut small parts out of other materials from time to time.

In this case, the part in question operates in a machine that pots flowers. The issue is the the fertilizer is highly corrosive. The parts that came with the potting machine were made of steel and have corroded to the point they are failing. They cost $80 each and there are 48 of them....painful...lol

These parts are not very precise and look to be cut originally with a water jet or perhaps with a plasma cutter. I can get them cut locally on a water jet for a whole lot less than 80 bucks which is what I will do if I can not cut them effectively.

It was clear to me soon after I bought this machine that it had a very limited use. I have used it a good bit to cut circles in aluminum and steel chassis for electronics projects I mess around with. I guess the good news is the knowledge I am acquiring about CNC machining with this little mill will for the most part be useful when and if I buy a larger machine. Crashing a fast high horsepower mill looks like a really bad thing to do on a Saturday morning...lol Perhaps it is a good thing I have this mill to learn on.

I got the Mach3 software up and running and got the limit switches and E switch working. I have a basic configuration in the software which seems to work ok. There is a world of things I do not understand at this point but little by little I will wade through it.  

Thanks to  both Tweakie joeaverage from down under for how to cut SS on any machine.

Billy

Hi Billy,
kool. Stainless is a challenge. You've really got to bore into it...if your too timid it work hardens to hell and then you'll be in real trouble.
Get yourself some good carbide endmills. Funnily enough the hardest grades are not what you want...you need tough endmills with a strong core.
Its likely you'll break them before the coatings give you any real advantage so until you've had some practice save the dollars on coatings.

I get a lot of really small endmills and drills for circuit boards. This outfit sells Kyocera Tycom, a good brand cheaply and I've bought hundreds off
him. I would suggest something in the 1/8 to 1/4 size. If you have a torquey slow spindle go for 1/4, a higher speed but with less torque go for 1/8.
If you have less than about 0.5 ftlb (0.75Nm) don't bother unless you want to break untold endmills.

http://stores.ebay.com/carbideplus/

Do you have cooling...you'll want it ...lots  and lots of it. More to do with flushing chips out of the cutzone than cooling....nothing but nothing buggers you
up like recutting chips no matter what the material, but you'll absolutely not get away with it in stainless.

Craig

a couple things on these "hobby" machines, at least as I see it.  to me they are just machines, and they are limited by their size to smaller cuts, but surface footage and feed per tooth should still be maintained.  I say this without having run a sherline.  but I have a large Bridgeport, and a round column gear head rong fu mill.  and I have run a 6" spindle cincinnati vertical with 6" spindle, a machine that id guess weighed in excess of 6 tons.

the Cincinnati would hold a 10" facemill, take a cut 3/16" deep the full width, and throw chips that actually made a clinking sound when they hit the floor.  moving to the Bridgeport 20 years later, I could run a 3" facemill on it, but was limited to cuts about .090" deep.  but I could still maintain the proper surface footage and chip load per tooth for the cutter being used.  running the rong fu, the round column is less rigid, and my depth of cut went to about .030", once again I still tried to maintain surface footage ands chip load.  the same applies to the lathes ive run, a 48" chuck engine lathe made chips that clunked, the 17" I have now is limited to about 1/8" depth of cut, and the 7" hobby lathe I have I limit to about .030 depth of cut roughing.  but I still set my surface feet and chip load to the tool, and also to the material being cut.

just a guess on my part but if I were cutting that "T" id start at 1000 rpm, .020 doc, and .004 feed/rev for a 4 flute carbide mill (4 ipm).  if it worked well, id increase the doc until the machine began to protest, then back off a little.  multiple roughing cuts leaving maybe .010 on the surface for a finish cut.  again this is a guess, others here have sherlines and may chip in.  and a couple other things, to minimize chatter, use a sharp end mill vs a radius corner one, and avoid the biggest sin I see often posted, the shortest mill extension possible makes the least chatter and vibration, so many times ive seen pics of a 1/4 end mill with 1" of flutes hanging out 2" when a stub end mill with 1/4 of flutes sticking out a half inch would have worked so much better.  theres a nice speed feed calculator on littlemachineshop.com.  start easy, bump up til you see a problem beginning, then back off one!  and good luck!

Hi guys,

This is the part I want to cut. Material issues aside, I don't know how to write the G Code properly. I can write the code for a T shape but don't yet understand how to write the code for the angle just yet.

The length for the hypotenuse is 1.5607.
a=0.250
b=1.500

Disregard the holes.

Perhaps someone could give me a heads up on how to write the code.

Thanks,

Billy

Billy,
All good advice on cutting stainless.  I had a Sherline spindle, 1/8" is it for stainless. but it works.  One more, use the shortest cutter mounted as short as possible, as this makes a big difference for a small machine.

The problem with hand coding the angles is that you need to know exactly where the end points are.  This is really tough working from paper.  The next thing is you have to deal with tool radius offset, using G40, G41, G42 and specifying the tool radius, then using a short move to get it applied after calling the tool offset number.  This is not something for the novice programmer.  

So the other option by hand is offsetting the part outline by the tool radius and programming that path.  On a small machine on hard material you may have to adjust the tool path for deflection and that means rewriting all your code.

I worked as a CNC programmer coding by hand, and I can tell you that life is too short for that crap in this day and age.  So get an inexpensive CAM program like CamBam so you can enjoy the machining.  I have two seats of CamBam, one for my homebuilt minimill and one for the big machine at work.  CamBam has a rudimentary drawing capability so you don't need a Cad program for stuff like this part.  CAM is what really makes CNC practical.

Thanks Gary,

I just about got the programming figured out. I did not consider the tool deflection issue. As this part does not need to be very precise the tool deflection will not make any difference  most likely.  I am sure CamBam would do the trick. I will go check it out.

I am trying to program by hand just for the purpose of learning and understanding G Code.

Because all this is for my own needs, I am not pressed to get it done in any hurry.

Thanks,

Billy

Hi Billy,
deflection induced inaccuracy may not matter much but snapped tools sure do!

You have to use small tools because your machine doesn't have the power and rigidity to handle bigger ones.
Small tool are a lot less stiff than big ones with flexure bordering on breakage.

Craig