Yellow Bullet Forums banner

21 - 39 of 39 Posts

·
Registered
Joined
·
472 Posts
140 Degree coated solid carbide. Sumitomo, Guhring or Kennametal. Don't spot drill or peck, it just work hardens the workpiece. 100 SFM and .010"/rev and one drill will last the entire job.
 

·
Registered
Joined
·
576 Posts
140 Degree coated solid carbide. Sumitomo, Guhring or Kennametal. Don't spot drill or peck, it just work hardens the workpiece. 100 SFM and .010"/rev and one drill will last the entire job.
Finally, someone who knows!

To the OP: if you don’t know how to convert SFM to RPM
here is a simple online calculator. Enter Prostreet’s 100 SFM (solid carbide) and your drill diameter. If the rpm that the calculator provides works well for this job then the next time you run 304SS, regardless of tool diameter or if you are milling or drilling, you can use that same 100 SFM, calculate for the RPM and achieve similar results provided you are using a similar cutting tool material naturally. This concept works for all materials. Bear in mind that solid carbide rotating cutting tools work best when held in a collet.

NOTE: The calculator asks for workpiece diameter. In your case you would input your drill diameter. Same thing for endmills.

 

·
Registered
Joined
·
1,253 Posts
140 Degree coated solid carbide. Sumitomo, Guhring or Kennametal. Don't spot drill or peck, it just work hardens the workpiece. 100 SFM and .010"/rev and one drill will last the entire job.
I was going to suggest these but he does not have through spindle coolant. They do make make them without coolant through, but not sure how good those would live in 304 x1000. Keep an ear on the sound and watch your spindle load if you can monitor that. My favorite one is the Kennemetal. They shoot a hole in 718 165ksi Inconel like a cobalt drill in 1018. Garr also makes good ones. They are super expensive compared to a Cobalt drill until you calculate the hours saved not only by the speed of the drill, but also by not having to spot drill or change a tool for a very long time. You might be able to use your current coolant pump and an auxiliary tool holder to drive coolant through the drill, however these types of drills run best at around 700psi-1000psi which most standard cnc mill pumps do not come close to. You might get by since you are only going 1/2" deep.
In regard to the Allied spade drills, they have a drill shank with an auxiliary coolant collar on it so you can drive coolant through the tool. Depending on diameter tolerance, hole position tolerance, and if you can get a short enough shank, you might be able to skip the spot drill, but the tolerances mentioned will need to be liberal.
 

·
Registered
Joined
·
14,453 Posts
Sumitomo SMD detachable tip, or soild carbide. Get a Sumitomo rep to make a recommendation and he will bring a sample or 2 for you to test. We did this to solve a problem in 4140HT, the rep sold us the one we tested first and liked at a discounted price, then offered the other 2 he brought along at half price so he wouldn't have to take them back.
 

·
Registered
Joined
·
412 Posts
I’m still waiting to hear how deep a hole he has to drill.
I read the Op as a through hole in 1/2" 304 but no hole size . I'm just a manual job shop hack so can't help with production machine set-up or tooling . But I have a steady repeating job that has 5 -1/4" through holes in 304 . Don't have a holder for spades under 1" so just use a stub cobalt jobber . I use cutting oil and easily get over 200 holes a sharpen . Break through is where it takes the drill out so have to ease up feed there , I do it by ear to hand like has already been said , guess that is programmed with cnc . I also sharpen more tip angle like was already recommended , leaves less rag to have to clean-up .
 

·
Registered
Joined
·
1,253 Posts
I read the Op as a through hole in 1/2" 304 but no hole size . I'm just a manual job shop hack so can't help with production machine set-up or tooling . But I have a steady repeating job that has 5 -1/4" through holes in 304 . Don't have a holder for spades under 1" so just use a stub cobalt jobber . I use cutting oil and easily get over 200 holes a sharpen . Break through is where it takes the drill out so have to ease up feed there , I do it by ear to hand like has already been said , guess that is programmed with cnc . I also sharpen more tip angle like was already recommended , leaves less rag to have to clean-up .
The break out just needs steady feed rate. Really hard to do manually even in auto feed.
 

·
Registered
Joined
·
412 Posts
manic I'm not sure what your saying but don't doubt you have your way of drilling that works for you . To me manual drill feed means moving the spindle by hand or cranking the knee or table on a mill. I rarely if ever use auto feed for drills smaller than 1/2 ". I like to use heavy chip load while drilling to get the chip out and with ss not work harden then back it off as it breaks through .
 

·
Registered
Joined
·
1,253 Posts
What you get with a manual mill at the breakthrough is not just from getting easier to push through for the quill handle, but the whole machine, quill, head to base, and knee to base all of a sudden relaxing when the drill point starts breaking through. When you slow down at the breakout you are compensating for that whether you use the quill or the knee. The knee has the longer leverage but the quill is more convenient. We just put ground ball screws on our Bridgeport for the X and Y axis and that makes milling more like a cnc, but the heavy Z axis work will still flex the machine if you lean on it. Can't really take all that out of it. The backlash for X and Y after the ball screw retrofit is .0007". With the original ACME screws it was like .080"! Also tossed all the plastic lubrication lines and plumbed it up with brass lines and compression fittings. Looks like I put a Fogger kit on it. lol Most of the plastic lines were clogged up due to the ID being so small. This 1960's era Bridgeport is one of the nicest ones i have had my hands on now.
 

·
Registered
Joined
·
412 Posts
cool I've never had the pleasure of running a tight bridgeport , only flogged ones . the first brand copies not bad when new . on the drilling thing , thinking about it drilling small holes has to be one of the harder jobs for me you know the jobs that you have to be on your toes , but if my 1/4" drill is loading up my machine It's time time for a fresh bit or a trip to the grinder but I get what your saying
 

·
Registered
Joined
·
46 Posts
Discussion Starter #34
Thanks for all of the responses. For those that asked, I'm using a 4 year Hurco VMC that has a 10k spindle and Mastercam to program it. It's 1/2" diameter holes going through 1/2" thick 304 stainless. I'm certainly not new to this, but you never know when someone else will come up with a better idea and I'm always looking to improve.
 

·
Registered
Joined
·
298 Posts
At my old job we worked in 304 & 316 stainless daily. We didn't use any fancy drills. We would use regular HSS drills sometimes with Ti coating. As long as your speeds and feeds are correct with plenty you shouldn't have a lot of issues.
 

·
Registered
Joined
·
14,453 Posts
Iscar replaceable head drill and be done. One head will do all the holes and then some

+1 Iscar is good. I have tons of the older Chamdrills, use them for 90% of our work. Chamdrills don't stand up to our 4140 HT parts, the head comes out of the body under high temps, that's why I switched to Sumitomo.The newer Sumocham style like at this link should fix that but I haven't tried it yet.
 
21 - 39 of 39 Posts
Top