Hard Coat Anodizing Tapped Holes - Oversized Taps Available? 2

[tommo]

Hi,

We do a lot of Hard Coat Anodizing of Aluminum Parts, Mill Spec Mil-A-8625 Type III.

My question is, as the anodizing builds up the surface of the material, in our case about 0.0015" on each surface, are there over-sized taps available to cut the threads, so after plating, the thread will be proper size?

How do you spec this on a drawing?

My concern particularly relates to 1/4" NPT threads.

Masking the thread in this instance will not work as the thread is for a plug that blocks a coolant passage, and I need the passage anodized for corrosion prevention.

Thanks in advance!

 

[TVP]

tommo,

Oversize taps are not off-the-shelf items, but they can certainly be made and sound like a reasonable option to pursue in your specific case. Regarding masking of threads, is there a way to "paint" the threads locally to create a masking effect, similar to the way steel parts are locally copper plated to prevent carburizing? I am only somewhat familiar with the anodizing process environment, and really only know about silicone plugs, etc. for masking.

 

[prdave00]

OSG offers oversized taps -

http://www.osgtool.com/product_list.asp?type=TAP&type2=SPIRAL POINT&list=280&Page=1.

I've only seen metric or UN threads off the shelf and not pipe.

This link explains about oversized taps designated as "H" taps meaning its pitch diameter is on the high side of basic:

http://www.newmantools.com/taps/taptech.htm.

When I've had parts made and then hard anodized then I've given the shop the option of plugging the hole or buying an oversized tap. They usually go with the latter if they have it available.

For a pipe tap can't you just tap the hole deeper - effectively making the opening pitch diameter larger. Forgive me if I'm not thinking straight.

 

[tommo]

thanks for the links prdave00. I will check them out.

My problem is we get the parts made by an outside machine shop, and they never cut the threads very deep, and after it's anodized - the thread entry isn't as far as I would like.

We only make 'onesies - twosies' and that's why I was looking for some way of specifying on the drawing the actual thread depth I wanted - rather than leaving it to the CAD software designating a distance and machinist tapping to that depth.

Using rubbish fittings from local suppliers the threads work ok, but with quality tube fittings, the threaded section seems to be much larger in diameter.

I think my CAD package calls out a depth of thread, but really - the machinist needs to check the fit of the mating tube fitting rather than relying on depth alone.

Perhaps that's my answer - just send a sample fitting and request that it can be threaded into a specified depth...maybe I should look at screw in thread gages too.

I know thats sounds bleedingly obvious, but in this world - nothing is easy!

But you are correct - a deeper tapped hole should allow more engagement before it binds

Thanks again for constructive input!

 

[masfaris24]

Absolutely Right, what did said mr prdave00, as additional information about it, you can read in this link :

http://coatings-specialist.com/anod...oatings-as-opposed-to-hardened-tool-metallic/

 

[efcmagnew]

Might it be an option to have the threads milled with a thread mill rather than tapped? I'm thinking this could be more cost effective, and you would not be limited to the taps you could find commercially.

Politics is not about making citizens happy, It's about making the right ones happy.

 

[adamgnt]

We regularly spec anodized threads through our machine shop when we want to electrically isolate or protect from the ocean, and they always come back fitting fine. I simply put "(.005 OVERSIZE)" under my normal UNC-2B, depth, etc. callout. I believe they may be using a high H tap, but in general I leave it up to the guys there who have been doing this for many years. I'm also not going beyond a 2B thread class. My gut tells me you're going to have a very hard time finding an oversize pipe tap. Throwing out as alternatives maybe a face sealed connector, or perhaps you can make a small coupler for the two thread interfaces?

 

[arguy]

I currently design parts using 6-32 threads that get hardcoat anodized. I have been specifying them .003 OS (OSG makes the taps and they are excellent, with the hypro7tin in a good machine I have gotten 5000-12000 holes per tap!). has anybody tried just running a 2b tap? my thought is that a GOOD screw would open the hole the needed amount with the soft substrate but not enough to seriously degrade the hardcoat? Because the some of the holes are not deep I need good engagement.

 

[tommo]

Arguy,

My guess is that a screw will not open the hole, it will just break off...

Hardcoat is really hard, and it is more ceramic in nature than mechanical, it's very difficult to get it to yield, it will crack before it stretches.

I will check out this OSG company for taps, thanks for the tips.

 

[johnchrc]

Can't you specify dims/gage depth apply after coating? Or with NPT have them gage 2 turns deep (past normal gage) with std +/- turn. I know for stub acme threads we don't adjust the dimensions. We specify DIMENSIONS APPLY AFTER COATING. Let the machine shop determine the tooling. I never get any feedback that they don't like or need more info.

If it is an NPT or UN thread I would mask the threads but that isn't an option for you.

There are calcs for determining dimensions baased on coating thickness. I have a program that does so for Acme, SA and UN thds.

- CJ