Qs on reg tapping

Awl--
Will be doing about 500 pcs of a bushing, 1" dia x 1 7/8 long, drilled/tapped thru the long dimension, 1/2-13 reg tap, for my lazy buddy in
Brooklyn. In 12L14, thankgawd... in a fadal vmc, 2 pcs per vise, 2 vises.
Now, even *I* can handle a job like this, but would appreciate a heads up/head start on a cupla points.
1. Can I get away with rigid tapping in a regular ER25 collet, or should I get a "tap collet"?
2. Speed/feed for a stubby drill (proly cobalt, but mebbe reg. HSS), with no separate spotting? I figger 18 ipm or so? It seems like many here go way beyond MHs speeds/feeds. Is it fair to say that because the hole will be tapped, it does not have to be as "clean" as a hole that is being drilled for shafting/sliding? Or would it be opposite, ie, should be even cleaner?
3. With good clearance out the bottom, I should be able to tap this without pecking? How bout a second quick "clean up" cycle with the tap? I noticed a few samples were tight at the far end.
4. IF we use an 11 mm drill, which is about .010 oversized for 1/2-13 (not a critical tapped hole), by about how much can the tapping speed increase? I typically have the rigid speed at S1000.2/F50.0 for 1/4-20, don't really tap that much.
tia.
--
------
Mr. P.V.'d (formerly Droll Troll), Yonkers, NY
  Click to see the full signature.
Add pictures here
✖
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
"Proctologically Violated©®" wrote:

PV:
    We rigid tap all the time using regular ER32 collets.

    18 IPM? Where did you get that number? I would say a range of 80-100 SFPM and .002-.004 inches per flute or 600-900 RPM at 3-6 IPM would be more reasonable.
    If you want to go 18 IPM, you might try one of Iscar's Chamdrill's.
http://www.carbidedepot.com/iscar-application-chamdrill.htm
    They are steel bodies with carbide insert tips. The have coolant through, if you have that feature, but they'll work with regular flood coolant. I was just using one a few weeks ago to drill some titanium pieces, that melted some regular drills.
http://64.251.206.64/iscar-spdsfds-chamdrill.htm
    For a .421 Dia. Chamdrill the chart at the site above says to use about 300 sfpm (low end of chart) and .006 ipr. (also low end). That comes out to about 2700 RPM @ 16 IPM.

    Yes. Peck tapping is really only necessary with exotic materials.

    I see no real advantage to that.

    Run the tap a little deeper if possible. You may be frying the tap trying to run it at 1000 RPM in steel. This is a coated gun tap, right?

    Probably half that would be in the ballpark for tap longevity.
--
BottleBob
http://home.earthlink.net/~bottlbob
  Click to see the full signature.
Add pictures here
✖
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
BottleBob wrote:

Bot - We generally drill 12L14 at speeds approaching what we'd use for brass. 150 to 200 SFM doesn't sound out of line for that stuff to me. 80 - 100 is where we'd be drilling, say, 303 or 416 stainless.
For the last few weeks we've been experimenting with drill feed rates. Remember a couple of years back when we discussed using something like 1.5% (per flute) of the drill diameter? For 12L14, that comes out to: .420 drill @ 180 SFM = approx 1600 RPM @ .012 IPR or 19 IPM.
For drilling almost 2" down, you'd probably want to peck a bit for the chips, but it doesn't sound too far out of line.

I've noticed that the insert drills recommend lower IPR feed rates than twist drills; of course, they make up for it by increasing the SFM.

I've also been doing something crazy lately: I call the tech support folks to ask what taps and feeds they reccommend for various materials. It's too easy to look in a catalogue and say "Oh, that's a good tap for stainless, and it's got a coating. I'll get that one." Sometimes they'll reccommend something that's not obvious, or give you a few caveats.
Add pictures here
✖
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Tom Accuosti wrote:

Tom:
    Actually, I was feeling some anxiety about replying concerning feeds/speeds. That's a subject that seems to be in constant flux with few certainties (closer to an art form than hard science <g>). But PV is a relative newbie to machining with little background information to fall back on, so I thought I'll chime in with some opinions.     THE two things that I tend to change when running one of my older programs are the feeds & speeds. I was running a program that I just did 8 months ago, and I changed the feeds/speeds on a quarter of the tools in the program.

    When doing a few prototype parts, you don't always have the luxury of doing extensive testing, so I'll defer to your experience in this matter. But I'll add what the following charts indicate:
==========================================================Machinist Toolbox
12L14 Drilling 88 SFPM .0013 per flute Feed ===================================================================================================================http://littlemachineshop.com/Reference/CuttingSpeeds.php#Drilling
12L14        Drilling 90-130 SFPM ===================================================================================================================http://www.hannibalcarbide.com/tech_support/feeds_speeds.php
12L14        Drilling 125-175 SFPM =========================================================    So the FPM ratings are all over the place.

    You know, I've noticed that. The lower feed per revolution "may" be because the carbide tips are just twisted on and are held to the end of the drill body by little bumps on the carbide that fit in recesses of the steel. So if you were taking a heavy feed (which would bury the tip "under" the chip), and then pulled out at rapid rates (like in a normal pecking situation) the carbide tip "might" pull off the end of the drill. Just my own unresearched speculation here.

    Heh, yeah. We call the tool guys all the time, to get tooling & starting points on weird materials or operations. As much as I'm normally anti-salesman, they do have their uses... occasionally. LOL
--
BottleBob
http://home.earthlink.net/~bottlbob
  Click to see the full signature.
Add pictures here
✖
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
BottleBob wrote:

That happens a lot here, although lately we've been testing how aggressively we can actually get. The most impressive thing was the 1.25 to 1.5% per flute feed rate for drills. Haven't tried it on teeny little drills yet, but stuff in the 1/4 to 1/2 range have been fun to watch. Anything over 1/2 we're generally using inserts.

But even so, we have found that we can machine 12L14 pretty much almost where we'd machine brass. We still do production, but mostly small production runs (100 to maybe 1,000 pcs) so we have opportunity to fool around with stuff.

On the lathes, we use insert drills with coolant thru, so pecking isn't an issue. On the rare ocassion we do, we manually program one or two pecks, skipping the cycle.
Also, we typically use insert drills with the screw-down inserts, not the spade drill type.

The tech support guys usually don't do any selling, and the sales guys are usually smart enough to not try to answer our questions ;-)
"I never eat tarts before noon," Tom said piously.
Add pictures here
✖
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Tom Accuosti wrote:

Tom:
    Do you program a "chip shear" dwell before pulling out on your peck cycle, to break the extra heavy chip that is in the flute? If not, have you noticed any cutting edge chipping on the end of the drills?

    1,000 Parts??? Just shoot me, and put me out of my misery! Just kidding... mostly.

    The Chamdrills can be used with through coolant, flood coolant, OR both. I was drilling the titanium parts with flood only.
--
BottleBob
http://home.earthlink.net/~bottlbob
  Click to see the full signature.
Add pictures here
✖
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
wrote:

I wonder if it's really necessary to dwell between pecks. To me it seems the short delay when the drill to changes feed direction should be enough to free the chip? Surely there's some deceleration/acceleration time involved as well.
--

-JN-

Add pictures here
✖
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Indeed. If you are turning 1200 rpm to drill, that is 60 rev's / second, or 1 rev per .1 sec. Doubtful if your machine can decel, stop, accel in reverse in less than 0.1 sec
--
Anthony

You can't 'idiot proof' anything....every time you try, they just make
  Click to see the full signature.
Add pictures here
✖
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Anthony wrote:

Anthony:
    1,200 RPM / 60 sec. = 20 Revolutions per second. But I agree, I don't think there is much delay when transiting from feeding to rapiding out of the hole on a peck drilling cycle.
    Just program .001 pecks (as if you were drilling with a .005 drill), and watch your machine run like a tattooing needle.
--
BottleBob
http://home.earthlink.net/~bottlbob
  Click to see the full signature.
Add pictures here
✖
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Excuse my error. I've been bedridden sick as a dog since Friday, and I am not thinking all that clearly. Really sad part is..I checked myself with a calculator before I posted..and have no clue how I came up with that number. Trying tough it out and go back to work today, as I'm just getting further behind every day I'm at home....but not sure how that will work out.
--
Anthony

You can't 'idiot proof' anything....every time you try, they just make
  Click to see the full signature.
Add pictures here
✖
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here. All logos and trade names are the property of their respective owners.