Thad

Carbide drill for 316 stainless - recommendations needed

Recommended Posts

We have a stamped part that we run out of 316 stainless. They want to add another hole to the part. It will eventually be added in the die but we have 500 parts without the hole that they want reworked. I'm hoping to run it with air blast (no coolant). I'm looking for recommendations on solid carbide drills to add the hole. The part is .100 thick and jobber length drill will be used. This *should* be a one time run.

Brand? Coating? Anything else?

Thanks!

Share this post


Link to post
Share on other sites

Walter Titex, Ghuring, OSG come to mind. That thin I would look at a 140 to 150 deg drill point. Might look for the 3 Flute tools more expensive, but they do a good job. Just use each one's Material grade tool selector and then they will call up the right drill and give you speed and feed recommendations. 

  • Thanks 1

Share this post


Link to post
Share on other sites

What's the diameter of the hole?

Are you looking for speed or for one drill to last the part run?

 

 

 

 

Share this post


Link to post
Share on other sites
15 minutes ago, Greg_J said:

What's the diameter of the hole?

Are you looking for speed or for one drill to last the part run?

 

.257 dia. I've been authorized to buy 6 drills.

Speed is obviously a concern, but it's not like we're running 1000s of parts all year long. 

Share this post


Link to post
Share on other sites
41 minutes ago, crazy^millman said:

That thin I would look at a 140 to 150 deg drill point.

No spot, just straight drill in?

Share this post


Link to post
Share on other sites
36 minutes ago, Thad said:

No spot, just straight drill in?

Yes. IT is a sheet metal part how tight you need to hold the true position on it? that thin no reason to spot in my mind especially with a 3 flute drill. 

  • Thanks 1

Share this post


Link to post
Share on other sites
18 minutes ago, crazy^millman said:

Yes. IT is a sheet metal part how tight you need to hold the true position on it? that thin no reason to spot in my mind especially with a 3 flute drill. 

Three flute drill doesn't look an option for us. Also, we're limited to what's offered at MSC.

My concern with whether to spot or not was because of the carbide drill, not the part thickness. Isn't there an issue of blown corners on a carbide drill when spotting the hole first? I'm kinda new to the carbide drill thing and production is not my forte. Oh...and hurry up, Thad.

Share this post


Link to post
Share on other sites
45 minutes ago, Thad said:

Three flute drill doesn't look an option for us. Also, we're limited to what's offered at MSC.

 

Why isn't 3 flute an option?

MSC carries SGS & they make a very good 3 flute drill.

  • Thanks 1

Share this post


Link to post
Share on other sites
5 minutes ago, MIL-TFP-41 said:

Why isn't 3 flute an option?

MSC carries SGS & they make a very good 3 flute drill.

Got a link? I don't see 3 flute drills there.

7 minutes ago, MIL-TFP-41 said:

Why isn't 3 flute an option?

MSC carries SGS & they make a very good 3 flute drill.

Now I see them.

Share this post


Link to post
Share on other sites

When searching for 3 flute drills on MSC, you can really narrow the options down by filtering by 150deg drill point.

if you can use a 6.5mm drill, your options really expand.

  • Thanks 1

Share this post


Link to post
Share on other sites
1 hour ago, Thad said:

No spot, just straight drill in?

Mikron cross pilot. 1.5 D with 170 degree point. No spot, shouldn't need more than 2, probably only one.

They aren't cheap but we use them a lot in hard metals

  • Thanks 1
  • Like 2

Share this post


Link to post
Share on other sites

Thank you all for the help. The tooling order has been placed. Certainly not a well planned out situation, but that's how we roll here. :rolleyes: 

  • Like 1

Share this post


Link to post
Share on other sites
2 hours ago, Thad said:

Isn't there an issue of blown corners on a carbide drill when spotting the hole first?

So they recommend that with carbide you start with a large included angle, then drop to a lesser angle with the follow drill so you just get initial engagement on the point, so less immediate heat build up.

  • Thanks 1

Share this post


Link to post
Share on other sites

Spot small then chamfer after.

 

We use the guring fired carbide a lot in titanium and invar. They are 118 so you can use a 120 spot drill also

  • Thanks 1

Share this post


Link to post
Share on other sites

I'm late to the party too, but my 5c worth... I'm currently running some drilling of 316, 6.5mm diameter. I'm using Sandvik Coromant 861.1 drills. Well, I'm still on the first drill it has currently drilled a total of 9 metres :)

 

  • Like 3

Share this post


Link to post
Share on other sites

Can anyone offer some speed/feed recommendations for plain old uncoated, 2 flute, solid carbide, Hertel, 118 degree drill? I found a Hertel chart that says 80-300 SFM and .005 per tooth for a material type of "Stainless Steel (soft)." I'm not sure where 316 stainless falls in the Stainless Steel (soft) realm. Any advice is appreciated.

Share this post


Link to post
Share on other sites
Guest
1 hour ago, Thad said:

I'm not sure where 316 stainless falls in the Stainless Steel (soft) realm. Any advice is appreciated.

It's on the harder side compared to 304 for example, but not as hard as 17.4 ph for example the 17.4 ph no coolant I drop as low as 75 sfm  /  150 sfm for 316 ss like millman said / 300 sfm for 303-304 

Share this post


Link to post
Share on other sites
13 hours ago, Thad said:

Can anyone offer some speed/feed recommendations for plain old uncoated, 2 flute, solid carbide, Hertel, 118 degree drill? I found a Hertel chart that says 80-300 SFM and .005 per tooth for a material type of "Stainless Steel (soft)." I'm not sure where 316 stainless falls in the Stainless Steel (soft) realm. Any advice is appreciated.

316sst is not necessarily "hard". The molybdenum in 316 does make it a lot tougher and more chemical resistant than 304sst. What you need to watch out for with an uncoated carbide drill is the accumulation of heat to the point that the cobalt can no longer hold on the the carbide at a faster pace. If you start seeing notches in your drill then you will need to cut the rpm. If your drill has a web point you need to either give it a split point or cut the rpm to lessen the heat. I would go 80 to 100 sfm.

  • Thanks 1
  • Like 1

Share this post


Link to post
Share on other sites

Thanky you all. You guys are great! :respect:

Share this post


Link to post
Share on other sites
On 8/21/2020 at 11:21 AM, Thad said:

No spot, just straight drill in?

Rarely would you ever want to spot with a carbide drill. Especially in stainless.

Go to the Guhring site and first select you material. Then size, the reference length. Do not choose a 3 flute for this. You will be looking for a 2 flute 140deg.

All of your options will be listed. Click on the drill then scroll down for your speeds and feeds link. Guhring makes drilling easy.

Share this post


Link to post
Share on other sites

Does anyone have any advice on controlling the burr? The exit burr is quite heavy.

Edited to say that I'm running at 100 SFM and .002 per tooth. (1486 RPM and 3 IPM).

Share this post


Link to post
Share on other sites
6 minutes ago, Thad said:

Does anyone have any advice on controlling the burr? The exit burr is quite heavy.

yank should be able to help you with that 

  • Haha 1

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us