I have an RFQ for some somewhat simple parts in 304 stainless. I have no experience machining, but everyone seems to say its a nightmare. Can the 1100 get it done to reasonable quality? I hate to pass on a job. Any advise would be great.
I have an RFQ for some somewhat simple parts in 304 stainless. I have no experience machining, but everyone seems to say its a nightmare. Can the 1100 get it done to reasonable quality? I hate to pass on a job. Any advise would be great.
It is truly a nightmare. Eats tools so bid accordingly. I have several stainless part numbers I run. Hate them all. Very, very good tool paths, speed and feed are vital. Dont be afraid to sacrifice cycle time for tool life. Youll make up the time in costs saved on tooling.
I've had very good results with 303 stainless on the tormach 770.. 304 was much more difficult and didn't seem to have advantages for my application in testing the mechanical strength. The key to 303 seemed to not feed too slowly and not turn too fast-every tool seemed to have a sweet spot-and you could hear it when it was taking a healthy cut, anything other was not good. very sensitive compared to steel and aluminum
Sent from my iPhone using Tapatalk
I think it seemed that it didn't want to cut; there was more deflection, broken end mill flutes, and I never found a sweet spot for feeds and speeds. The recommended speeds and feeds from gwizard were similar to 303 but not as effective.
Sent from my iPhone using Tapatalk
Give em two quotes; one outrageously high for 304 and one very reasonable for 303.
I've been down that road, and 304 is a PITA. You need a lot of rigidity to keep from destroying tools, and these little machines just don't have it. Carbide tools especially need rigidity or they self destruct qjickly. I'll do 304 if the parts are very small, otherwise its like watching grass grow. One of the biggest complaints on the professional forums, is you never know,what you are going to get. You get cutting parameters dialed in, then the next batch of material is completely different. If you can talk them into 303 instead, that would certainly help.
low speeds, steady feed, good cutting OIL, sharp tools.
Its one of the reasons I have a Darex cutter grinder, and learned to hand sharpen drills, if the tools arent sharp youre in trouble.
I used Ridgid cutting oil in my lathe,
some of it work hardens really bad, varies from batch to batch, even though its all marked 304.
Try to keep it as cold as possible, when it generates much heat it will work harden and gall much easier.
I retired from the Stainless welding machining business, bought the 1100 and some 6061, thought I had died and went to heaven!!
Use 303 if you can, it machines much easier than 304 as stated earlier.
I have heard that the corrosion resistant properties are better in 304 than 303.
I avoid it like the plague here, been spoiled with 6061 ha!!
mike sr
The difference between 303 and 304 is about the same as the difference between 1018 and D2 tool steel.
So, i do not know how some people dare to put 303 and 304 into the same category.
That said, 304 machines a lot worse than D2
The main things to keep in mind is:
1) Do not let it rub. Feed about as hard as said D2, but at lower speed.
2) Use quality tooling.
3) Use cobalt or carbide drills (Always drill with coolant)
4) Use coated carbide endmills. (variable helix, 3-4 flute with corner radius)
5) Unless you are seriously into HSM game and have appropriate machine, run coolant when milling too
6) Try to keep radial engagement below 1/3 of the diameter. Avoid slotting or reduce the cutting speed when doing so.
Because your machine's rigidity might be a problem use 3/8" or smaller endmills.
I do not know your setup, and can not recommend you any speeds and feeds, but here is what i would use for slotting:
This cut would require about 1 horsepower.Material: 304 Stainless Cold Rolled 225-275 HB
Tool: 0.375in 4FL Carbide TiAlN HP/Roughing End Mill
Speed: 145.6 SFM/ 1483.8RPM
Feed: 0.0019 in/tooth 0.0078 in/rev 11.51 in/min
Chip Thickness: 0.0019 in
Reference Chip load: 0.0019 in
Engagement: DOC=0.16 in WOC=0.38 in
http://zero-divide.net
FSWizard:Advanced Feeds and Speeds Calculator
Remember the age old machinists singy song, "304 it's a whore, 303 it's for me"...says it all.
watch my video i posted on PCNC 1100H model thread of my mill drilling stainless steel.
Ha ha. I got my hands on a lot of 304 scrap some years ago and learned to weld on it. Then I stuck with it when learning the lathe and mill. I broke a lot of tools, but I did learn how 304 work-hardens. The key is to cut beyond the work-hardened layer. In 6061 and 7075, you can take your heavy cuts, then take a light "finishing" cut to make it all pretty. Not so with 304! You really don't want to take too light a cut because you'll dull (or break) your tool. I heard it said that when you work-harden with too light a cut, you'll pooch the tool and half of the life of the subsequent tool getting through it.
1. use sharp tools. I like stellite and HSS. Carbide is easy to chip, especially on interrupted cuts, so I avoid it on 304.
2. don't heat up the part
3. take slower, heavier cuts
4. use a good lube.
As stated previously, 303 is a world apart from 304 and machines easily.
Oh, and machinability and weldability are generally inversely proportional. (i.e. a material tends to be one or the other, but not both)
I always heard titanium was a PITA to machine, but having gotten used to 304, it's a snap. Same deal, use sharp tools, good lube, and cooling.
304 can be a good money maker but you have to know what you are doing and you need to have a rigid machine, the light duty tormach can deflect easily and work harden the stainless and you are toast. You might want to pass or sub it out to someone else so you don't lose the job.
While machining, keep it as cold as possible, when it starts getting warm it gets much more difficult to machine, work hardens more easily.
I used Ridgid dark cutting oil on the lathe.
Not all bars of 304 cut the same, some will work harden easily others do not.
Tapping, use a sharp drill to drill the hole, high feed, a dull one will make the hole almost impossible to tap.
316 and 304 pretty much machine the same in my opinion.
Stainless is not a hard material but it is tough.
I used carbide on the lathe as it will cut thru a work hardened spot more easily, I sharpened my own cutters, kind of a must dealing with stainless.
I worked in Dairys and Bakeries for 50 years and most of my polishing adapters and special tools were stainless, steel can contaminate the stainless if it comes in contact with it.
mike sr
I would rather cut 718 Inconel or 6AL4V titanium than 304 stainless.
You can buy GOOD PARTS or you can buy CHEAP PARTS, but you can't buy GOOD CHEAP PARTS.