Tap Depth Vs Blind hole Depth
Tap Depth Vs Blind hole Depth
(OP)
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.
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.





RE: Tap Depth Vs Blind hole 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"?
RE: Tap Depth Vs Blind hole Depth
Software For Metalworking
http://closetolerancesoftware.com
RE: Tap Depth Vs Blind hole Depth
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.
RE: Tap Depth Vs Blind hole Depth
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.
RE: Tap Depth Vs Blind hole Depth
Ed Danzer
www.danzcoinc.com
www.dehyds.com
RE: Tap Depth Vs Blind hole Depth
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
RE: Tap Depth Vs Blind hole Depth
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"?
RE: Tap Depth Vs Blind hole Depth
RE: Tap Depth Vs Blind hole Depth
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.
RE: Tap Depth Vs Blind hole Depth
Sorry, this should have been:
For other Thread depths: (Thread Depth * (1 + Thread Pitch * 4)) + (Thread Pitch * 5)