304SS Milling Strategy Needed

JBNimble · May 25, 2019

I have a very specific hole type I have to make in 304SS and I'd like some knowledgeable advice before I even start.
The 304 is 1/2" thick. I need a through hole 1.66" diameter, and a counter bore 1.875" diameter by 1/4" deep. There are no geometry obstructions, so I can use a very short tool. I have up to 4000rpm available, with lots of torque, and the spindle is very rigid. This has to be done with ONE tool, which will surely be an end mill. Should I do the through hole with a helical path, and then the same for the counter bore, both from the top down? Or should I do a smaller helical bore and then do concentric arcs to work my way out to the finished diameter for both features more like a high speed machining approach? Based on your suggested method, what diameter end mill should I use? 0.030" radius is tolerable for longer tool life. My goals are reliable process, good tool life, and good surface finish. This is low production, so I don't mind spending more on the right tool if I can get confident direction up front. Ask questions if required.

G00 Proto · May 25, 2019

Your answers are going to be all over the map with this question. No matter what, it isn't going to be fun or fast. Personally, I would use a 1/2" Carbide End Mill (you are going to have a fairly short tool life and these are pretty cheap). I would helix in at the center and then do a high speed tool path out to diameter on the thru hole, then come up and get the counterbore with a standard 2D contour. Doing concentric circles is fine, but you are going to wipe out endmills when it transitions from one diameter arc to the next (going to substantially higher angle of engagement compared to the arc tool path).

Plan B would be to run a fixture bolt down the center of the bore, and then do a helix down on the 1.66 Diameter hole (slug is constrained). Then do the counterbore.

Quite frankly both of these are substandard. This would be a great application for a big ass carbide spade drill, followed by an endmill to clean up the bore and make the CB.

litlerob1 · May 25, 2019

I'd use a 1/2" (16mm) bull nose Endmill, since it's a through hole the bigger the corner the better. I would use a 3 or 4 flute-not more. IT doesn't really matter what toolpath you use, this is very minimal Material removal. I suggest the size simply for the price and availability. Flood coolant and generate the hole through first so the chips have somewhere to go.

R

JBNimble · May 25, 2019

G00 Proto said:
Your answers are going to be all over the map with this question. No matter what, it isn't going to be fun or fast. Personally, I would use a 1/2" Carbide End Mill (you are going to have a fairly short tool life and these are pretty cheap). I would helix in at the center and then do a high speed tool path out to diameter on the thru hole, then come up and get the counterbore with a standard 2D contour. Doing concentric circles is fine, but you are going to wipe out endmills when it transitions from one diameter arc to the next (going to substantially higher angle of engagement compared to the arc tool path).

Plan B would be to run a fixture bolt down the center of the bore, and then do a helix down on the 1.66 Diameter hole (slug is constrained). Then do the counterbore.

Quite frankly both of these are substandard. This would be a great application for a big ass carbide spade drill, followed by an endmill to clean up the bore and make the CB.

For a 1/2" end mill, what size hole should I make for the initial penetration?

G00 Proto · May 25, 2019

JBNimble said:
For a 1/2" end mill, what size hole should I make for the initial penetration?

I have never done any studies or brain squeezing on that topic, so I don't really have a meaningful answer. I know I would like it less than one inch to make sure I don't create a cutter killing slug, and big enough that it didn't re-cut chips and cut too much on the center of the endmill. If I had throw a number out there I would probably be around a .725" hole. That keeps the center of the endmill out of the cut, but still has some room for chip evac. Hopefully one of the cutting tool experts will jump in and give their input.

jjxtrider · May 27, 2019

I used to do a ton of these in both 304L and 316 , but I often used a spade drill or indexable just under the hole size and then a 1/2" carbide endmill to finish out the hole and c'bore . As far as tool life , without doing the helical entry and using a drill, or cutting slots starting from an edge, I have filled 3 55gal barrels with chips on the same endmill with it just showing the coating wear but still cutting ok( they then go to the "abuse" side of the endmill stash to cut lasered edges ect.. where damage is higher that can nick edges or wreck endmills easier . My favorite endmills were Data Flute SSi5's -.30r-C11 coating DataFlute - A Heritage-Cutter Company - Dataflute , you can get the 5/8loc version (2300-2600rpm & 35 to 45imp @ .055-.125 RDOC,@ 2xADOC), Gorrila HP4's as well are as long lasting but loose some speed due to 1 less flute .

The one question mark is the initial helical hole , never liked to do it in SS so generally drilled with an indexable or spade if the hole hadn't been laser cut already . I'd try to drill at least 1", bigger drills get so slow and power hungry so not always time beneficial depending on mill , then go full depth of flutes and helical out to 1.650 , then up to c'bore debth and same helical to -.01" and then finish cycles(or go straight to finish diameter on both if not critical diameters)By adjusting stepovers you can get it to do a light finish passess or do a spring pass right after it roughs each debth so you don't need separate cycles, all depending how accurate the machine and hole specs.

.

9finger · May 28, 2019

I’d predrill 1/2-3/4” splitpoint drill, or carbide fancy pants drill of some sort, trocoidal mill to depth, full depth on both, 1/2” 7 flute variable helix, 0.02” radial stepover (bullnose if possible) max rpm, 150fpm, with0.005” stock to clean for a finish pass at standard f/s.

litlerob1 · May 28, 2019

9finger said:
I’d predrill 1/2-3/4” splitpoint drill, or carbide fancy pants drill of some sort, trocoidal mill to depth, full depth on both, 1/2” 7 flute variable helix, 0.02” radial stepover (bullnose if possible) max rpm, 150fpm, with0.005” stock to clean for a finish pass at standard f/s.

Jesus, why would you "trochoidal" Mill the hole, if you have a hole?

R

9finger · May 28, 2019

litlerob1 said:
Jesus, why would you "trochoidal" Mill the hole, if you have a hole?

R

Fair enough, not the right term. I was trying to make it easy if he's using CAM software, which any decent software would discard the oscillations of true trochoidal milling, but would be under adaptive clearing or trochoidal, rather than contour or profile, with a little less clicking. In short, I'd go full DOC, 10%ish radial, and rip through it full speed.

litlerob1 · May 28, 2019

I wouldn't use tiny ass step over. I would generate the 1.66" Diameter in 2 step overs, and Finish on the Second one--after making the hole through with the same Endmill. This material is only 1/2" thick. You need to get the material cut and the Tool out of there. Were talking about maybe a 4 Minute part. Trochoidal Toolpaths can lick 'em nuts. 10% step over? Dude it's .488" per side!!! He's not Milling out a pump housing for the Titanic.

CAM jockeys are stuck and never seen real Machinists, Machine real parts for real Dollars per real time minute, just to feed their families.

R

Gibbs
Mastercam
NX

Delw · May 28, 2019

litlerob1 said:
I wouldn't use tiny ass step over. I would generate the 1.66" Diameter in 2 step overs, and Finish on the Second one--after making the hole through with the same Endmill. This material is only 1/2" thick. You need to get the material cut and the Tool out of there. Were talking about maybe a 4 Minute part. Trochoidal Toolpaths can lick 'em nuts. 10% step over? Dude it's .488" per side!!! He's not Milling out a pump housing for the Titanic.

CAM jockeys are stuck and never seen real Machinists, Machine real parts for real Dollars per real time minute, just to feed their families.

R

Gibbs
Mastercam
NX

Butt Butt thats what the cool word was like 5 years ago to make someone look like they knew what they were talking about

Also I prefer the Term " Cam Pirates" not because someone may have pirated it, but simply because thats what we call all the Wannabes pro bass fishermen with patches all over there fishing jackets

9finger · May 28, 2019

litlerob1 said:
I wouldn't use tiny ass step over. I would generate the 1.66" Diameter in 2 step overs, and Finish on the Second one--after making the hole through with the same Endmill. This material is only 1/2" thick. You need to get the material cut and the Tool out of there. Were talking about maybe a 4 Minute part. Trochoidal Toolpaths can lick 'em nuts. 10% step over? Dude it's .488" per side!!! He's not Milling out a pump housing for the Titanic.

CAM jockeys are stuck and never seen real Machinists, Machine real parts for real Dollars per real time minute, just to feed their families.

R

Gibbs
Mastercam
NX

Guess it depends on tool holders and rigidity. I've got manuals that'll handle heavier cuts than some of my CNC's just because they are massive, rigid, and all glorious cast iron. I've found on a lot of the CNC's I run, tool holding is the weak link in just how much MRR you can achieve.

Maybe I'm not a real machinist, by whatever your definition is, but I've managed to keep food on my family's table for a long time before I bought CNC machines,with a 1932 southbend, 1918 LeBlonde, 1968 Hardinge horizonatal, and a sloppy old bridgeport, all while being crippled.

SeymourDumore · May 28, 2019

litlerob1 said:
I would generate the 1.66" Diameter in 2 step overs, and Finish on the Second one--after making the hole through with the same Endmill. This material is only 1/2" thick. You need to get the material cut and the Tool out of there.

That!
1 1/4 LOC EM, rough with the upper half, retract and finish with the lower half, retract some more and then onto the C'bore.
Done-in-one!

Of course, now that I am a cocky sum'bitch with TSC, I'd drill to 1 5/8 with an insert drill.
Heck, for a 1/2" material I'd drill it to 1 5/8 even on the non TSC machine.

DMF_TomB · May 29, 2019

304 can vary a lot. if work hardened or cold rolled and full of slag hard spots i have often seen cheaper 304 go through a lot of tooling. literally you can go through 1/2 dozen end mills on one big hard spot of slag.
.
sure if annealed and if its got no hard spots you can machine a lot of it with no problems.
.
just saying thats why you got a few saying no problems machining and others who had a lot of problems machining 304. and hard spots of slag doesnt really care about feeds and speeds. seen tooling go dull in a second many many times.

jjxtrider · May 30, 2019

litlerob1 said:
I wouldn't use tiny ass step over. I would generate the 1.66" Diameter in 2 step overs, and Finish on the Second one--after making the hole through with the same Endmill. This material is only 1/2" thick. You need to get the material cut and the Tool out of there. Were talking about maybe a 4 Minute part. Trochoidal Toolpaths can lick 'em nuts. 10% step over? Dude it's .488" per side!!! He's not Milling out a pump housing for the Titanic.

CAM jockeys are stuck and never seen real Machinists, Machine real parts for real Dollars per real time minute, just to feed their families.

R

Gibbs
Mastercam
NX

Spoken like a true "cam fearist" I work with a guy that sounds the same, Btw , I have machined ss for 28years ,didn't get into using software till 6 or 7 years ago, how you suggest will have poor tool life, very poor (at least on those Haas pos),then try to work for someone that complains about why tools don't last. I'm guessing you've never actually tried any of that stuff or did an honest comparison as to which one is actually quicker ,I've proven them out a bunch of times, all depends on machine/tooling rigidity as too how much stepover is doable without a bunch of vibs, what endmill ect... If a person automatically assumes, then they stay in the 80's.

I doubt it would even take 3 minutes, done tons of same type of stuff(that's how I could post numbers with no need to look anything up)so very familiar with timelines.

SeymourDumore · May 30, 2019

jjxtrider said:
Spoken like a true "cam fearist" I work with a guy that sounds the same yadda yadda yadda blah blah blah .... at least on those Haas pos...
I'm guessing ... blah blah blah ... you've never actually tried..... or did an honest ... yukk yukk yukk ....
I've proven them out a bunch of times,... ( You' Da Man!)
If a person automatically assumes, then they stay in the 80's....

I doubt it would even take X minutes!
Done tons of same type of stuff... so very familiar with timelines.

Well then, We all have the answer from the jixer!

litlerob1 · May 30, 2019

jjxtrider said:
Spoken like a true "cam fearist" I work with a guy that sounds the same, Btw , I have machined ss for 28years ,didn't get into using software till 6 or 7 years ago, how you suggest will have poor tool life, very poor (at least on those Haas pos),then try to work for someone that complains about why tools don't last. I'm guessing you've never actually tried any of that stuff or did an honest comparison as to which one is actually quicker ,I've proven them out a bunch of times, all depends on machine/tooling rigidity as too how much stepover is doable without a bunch of vibs, what endmill ect... If a person automatically assumes, then they stay in the 80's.

I doubt it would even take 3 minutes, done tons of same type of stuff(that's how I could post numbers with no need to look anything up)so very familiar with timelines.

Hahaha, I used Catia and Mastercam V3 (not X3). I comfortably use 3 suites of CAM. And have used about 6 more. Don't make assumptions about me.

R

BTW Tooling is what we call perishable. Balance is the goal in general, but not the rule. Do the Math and figure out the balance. But you might work for someone who is going to cry because the job took too long, then when you do it fast enough, bitch about Tooling costs, then when all that is dealt with, bitch about the unsanitary restroom. 304 is not and never has been something to baby, get it cut and get out.

G00 Proto · May 31, 2019

litlerob1 said:
Hahaha, I used Catia and Mastercam V3 (not X3). I comfortably use 3 suites of CAM. And have used about 6 more. Don't make assumptions about me.

R

BTW Tooling is what we call perishable. Balance is the goal in general, but not the rule. Do the Math and figure out the balance. But you might work for someone who is going to cry because the job took too long, then when you do it fast enough, bitch about Tooling costs, then when all that is dealt with, bitch about the unsanitary restroom. 304 is not and never has been something to baby, get it cut and get out.

Rob has proven to be a pretty competent guy, so I respect his opinion on this. I'm still in the camp of running a highspeed toolpath with smaller radial stepovers on my machines, but on the original poster's machine (slow RPM, tons of torque, and no tool changer), I would be tempted to try it like Rob. Funny story... years ago I had 5 big 15" diameter 1.25" thick turned parts out of 304. They were supposed to come out of plate, so I requested it to be waterjet cut into round, then go into lathe. Owner decided not to spend the $50 on waterjet. Told me to make it round on a Haas. I was pissed and about ready to quit anyhow. So I loaded up a 1" cobalt rougher and buried it full depth, then increased the feed until the spindle was at 99% figuring either the cutter or the Haas would burn up. Nope, made it through all the parts in record time... owner came by smug as hell and said "told you so". I guess he did

Wsurfer · May 31, 2019

I did a similar 304 job recently. 1.5" bore 1 " deep (through). I used. 1/2" cobalt drill through the center, then dropped a 3/8" end mill down the hole and HSM my way to final diameter. Did it in 2 depths. I used 5% step over based on a article i read on HSM advisor on milling SS . Worked fine, but I only had to do 2 parts, so can't comment on tool life.

memphisjed · May 31, 2019

call allied tool, have tool holder made with t-a inserts for drill and standard inserts for counter bore. If they work on our drill line - which is beyond flimsy in machinest standards (rigid as heck in steel shop standards)- then they will work on mill. They will even tell you which inserts are best and coolant/feed for that specific tool. one tool, no pre-drill, no tool path (feed changes, but one shot thru).

304SS Milling Strategy Needed

Plastic

Hot Rolled

Diamond

Plastic

Hot Rolled

Aluminum

Aluminum

Diamond

Aluminum

Diamond

Stainless

Aluminum

Diamond

Diamond

Aluminum

Diamond

Diamond

Hot Rolled

Cast Iron

Titanium

Similar threads