Smart questions
Smart answers
Smart people
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Member Login




Remember Me
Forgot Password?
Join Us!

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips now!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!

Join Eng-Tips
*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Donate Today!

Do you enjoy these
technical forums?
Donate Today! Click Here

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.
Jobs from Indeed

Link To This Forum!

Partner Button
Add Stickiness To Your Site By Linking To This Professionally Managed Technical Forum.
Just copy and paste the
code below into your site.

mkp520 (Mechanical)
23 Mar 09 14:22
Hi Guys,

I am a young engineer, looking for some help from your practical expertise.

Is there any best relation tap depth and blind hole depth? And how it vary for Aluminum and steel?

Example, If I want to have a tap of 1/2" deep then how much deep the hole should be?

Regards,
mkp.
KENAT (Mechanical)
23 Mar 09 15:14
Common rule of thumb is to allow 3 thread pitches extra for the 'tap drill' over the thread depth.

Can't recall when or where but someone posted a link or a pdf of common thread tap tools.  I have a print off and while it varies a bit it shows about 5 thread pitches deeper.

If specifying on a drawing you usually only specifly the minimum full thread depth required, with if necessary a note such as 'do not break thru', it's not normally corrrect to specify tap dia or depth.  However, it's still good practice the consider the tap depth to ensure you aren't asking for bottom taps etc whereever possible.

A resource like machineries handbook will probably have the information you need.

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

mrainey (Industrial)
23 Mar 09 18:33
Machinists will be grateful if you give them as much leeway as possible.  Make sure there's a good reason for the drill depth limits you specify.  Don't call for a max depth based on a formula.
 

Software For Metalworking
http://closetolerancesoftware.com
 

gerhardl (Mechanical)
26 Mar 09 4:29

As the others have stated, you normally go the other way around, and start with the total construction and fastener type, and any standards applicable:

You first select the fastener type out from standards if applicable, commercial available bolts and screws, necessary bearing force and 'normal practice' - you have to start somewhere.

Next step would be to control if the selected solution is strong enough, or could be done with another number of fasteners, or another dimension.

Supplier could then normally advice or state minimum threaded part necessary for different materials, if this is not already stated in standards.

Check again that total depth for 'normal machining tools' does not break critical depth.

If necessary specify limits: threaded part not less tahn x, total depth not more than y.

Check that standard type commercial type fasteners are available and suits in length both your machined part and are available to suit in length and dimension also the (standard?) counterpart(s).

Typical example: Not through-going threaded holes for flanges with screwed in standard threaded (both ends) pin bolts to fit standard counterflanges together with flange sealings. All this will include standard dimension and number of bolts, lengths to suit standard thickness of flanges and somewhat variable thickness of flange sealings.

BillPSU (Industrial)
26 Mar 09 14:02
Wherever possible or reasonable use a through drilled hole and give a minimum thread length callout. A blind hole requires the tap to pull the chip out of the hole, meaning it is a spiral fluted tap. The most expensive tap and probably the weakest. There are three different chamfer lengths available in taps bottom, plug, and taper/hand. Bottom has 1-2 thread pitch chamfer, plug 3-5 tpc, and taper/hand has 7-10 tpc. A bottom tap will have to cut the material with the highest chip load. Tapping very tough materials such as stainless(depends on the stainless) and ETD 150 can be nearly impossible with a bottoming blind hole.
I also want to caution you having to great of tapping depth greater than 3 x basic diameter can become difficult because of thread drag on the tap. I had to tap a .5-13UNC thread through a 2.5" thick flat bar. To reduce thread drag I used a interupted thread tap to help out with the thread drag. The tap was an extended spiral point interupted thread nut tap.
 
EdDanzer (Mechanical)
26 Mar 09 21:10
My preference is to through drill and use spiral point taps for most materials in short run parts. For blind holes 3X the diameter is as short as is practical with spiral point taps. We tend to thread mill or single point holes with drill hole depth limitations. In higher production volumes some materials can be thread formed, reducing the drill depth. This web site has additional good information. http://www.emuge.com/taps/

Ed Danzer
www.danzcoinc.com
www.dehyds.com

juergenwt (Mechanical)
30 Mar 09 19:42
Contact a tap manufaturer. There are taps for every situation and material. Some will pull the chip out on top so very little clearance is needed on the bottom of a blind hole.
Here is one site. It is in German but self explanatory .
Scroll down to page 12 of 64 . The name for blind hole: Sackloecher.http://www.jel.de/kataloge/a1_dt_n.pdf
The page Nr. is 2.6
KENAT (Mechanical)
31 Mar 09 11:03
mkp520, you've got a range of answers above, with varying levels of detail, all of which are pretty much 'correct' depending on your view of point.

Things you need to consider are:

How many are you making?  If making hundreds or thousands then really going to town optimizing manufacturing process makes a lot of sense.  If you're only making one or a handfull, then it's probably better to use a rough rule of thumb to speed the design process (your time costs $) even if it increases machining cost/difficulty a little in some cases.

Are you a desinger or a manufacturing guy, i.e. from what point of view are you asking the question?  If from a design point of view you don't need to get overly concerned with the how, so long as what you're asking for is possible for a reasonable cost etc.  If manufacturing guy you really want to be able to optimize it.  If a small shop where you're effecively both then you need to decide where to draw the line.

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

AviatorJim (Aeronautics)
11 Jun 09 9:06
There are also different taps avaialable require less room at the bottom of the hole (bottoming taps) but they will not start cutting as well.  And it takes longer due to having to clear the chips.  
JonGould (Mechanical)
14 Sep 09 16:51
Tap drill depths for spiral point plug tapping blind holes.

For over 40 years I have waited for a definitive formula that would work well for calculating tap drill depths for blind holes.  For 30 years I have used the simple formula of Thread Depth + Thread Pitch * 9 for threads of two diameters of depths.  This works in most cases and is far better to use than the Blah, Blah Blah, espoused by so called machining, (usually self elevated), experts.

The fact is the volume, stiffness and tenacity of the cut thread wire that is being forced into the hole; determines the amount of volume below the full thread depth that will be required in order not to break a spiral point plug tap.

The vast number of formulas and advice found in articles and training manuals would assure the breakage of the tap in any material other than plastic, cast iron, lead, or aluminum.  One method would be to use the values found in training manuals and/or tap catalogs, and when the tap breaks; increase the tap drill depth until the tap stops breaking.

Most would suggest other threading methods rather than answer this question; however, the fact remains that if it is hard material, using a spiral point tap remains the most cost effective operation for producing a thread.

For 2 x diameter depth threads:  Thread Depth + Thread Pitch * 9

For other Thread depths:   (Thread Depth * (1 + Thread Pitch * 4)) + (Thread Pitch * 9)

This will result too much tap drill depth in large diameter fine pitch threads; however, in the absence of any real scientific imperial data based upon the volume, stiffness, and tenacity of the thread, "chip",  wire being forced into the hole based upon the science of material chemistry and hardness, it is the best that anyone will give you.
 
JonGould (Mechanical)
14 Sep 09 17:25
" For other Thread depths:   (Thread Depth * (1 + Thread Pitch * 4)) + (Thread Pitch * 9) "

Sorry, this should have been:

For other Thread depths:   (Thread Depth * (1 + Thread Pitch * 4)) + (Thread Pitch * 5)
  

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!

Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close