What's new
What's new

tapping mild steel sheet metal - cutting vs forming tap

MooseKnifeCo

Plastic
Joined
Jul 16, 2021
Hi,

I have a job where I'm going to be tapping about 250 m5x0.8 holes into some 12ga sheet metal. I know that's well below the minimum thread engagement as it's only about 3 threads but it's going to hold small din rails and fans so there won't be much weight at all on the holes (and the hole sizes and metal thickness are pretty much constrained to be what they are). my question is whether I should go with a cutting or forming tap. I thought forming may lead to a slightly stronger hole but I have not used forming taps in laser-cut mild steel. what would you all recommend, forming or cutting tap for mild steel? these will be tapped by hand too, either with a tap wrench or in a hand drill, no mill or drill press.
 
Cut tap. Form tap is harder to run manually, and will push out some material top and bottom thus reducing the thread engagement %. Also, form tap requires precise hole diameter and it sounds like you are unlikely to have that.
 
I'll take the pro forming tap side of the discussion:
I think either the cut or form tap will not be difficult in a hand-held drill motor. Hand tapping would get old fast and would take ten times as long. I do not think the formed thread would be weaker---any pushed out metal will conform to the thread profile and likely would contribute (a little) to the holding power not to mention formed threads as a rule being stronger than cut. I have no study information to compare formed vs cut in this thin metal, so I can not back up this idea with any real facts. In this case strength does not seem to be an important factor. Hole diameter is different for formed than cut, but why does it need to be more precise? I like using thread forming taps. Tap breakage should not be a risk in this application. But forming taps are more resistant to breakage as their profile is more robust.

General random thoughts:
One thing that may be a bit challenging is eyeballing vertical to the sheet. I have never done this, but if I had 250 holes that had to look like they were done in a workmanlike manner and did not want to mess one up, I would find a way to attach a small circular level vial to the side of the drill motor using a little imagination and hot glue. That way I would be confident I was entering the hole at close to 90. I have used various guide blocks to assist in hole verticality. I don't really find them handy as they are tricky to keep close enough to the hole to be useful but also not be in the way. Some folks have more calibrated eyes than others and might do just fine by eye. Deeper holes in thicker metal tend to self-align.

FWIW,
Denis
 
Hole diameter is different for formed than cut, but why does it need to be more precise?
If the hole is undersize, the form tap will have to squeeze too much material into not enough space, and possibly break. Cut tap can just cut that extra material away.

If the hole is oversize, the form-tapped thread % goes way down, and the minor diameter can be below spec. Since this application has only ~3 threads of engagement, low thread % might be quite bad.
 
If the hole is undersize, the form tap will have to squeeze too much material into not enough space, and possibly break. Cut tap can just cut that extra material away.

If the hole is oversize, the form-tapped thread % goes way down, and the minor diameter can be below spec. Since this application has only ~3 threads of engagement, low thread % might be quite bad.
I guess I just drill my holes per table recommendation or a few thou over and never had a problem

Denis
 
If the hole is undersize, the form tap will have to squeeze too much material into not enough space, and possibly break. Cut tap can just cut that extra material away.

If the hole is oversize, the form-tapped thread % goes way down, and the minor diameter can be below spec. Since this application has only ~3 threads of engagement, low thread % might be quite bad.
yes I agree and thats why i wanted to poll some other people, my hole size I spec will be based on the tap type I use and I think the laser cut can hit within the tolerances either tap will need.
 
I would use self-clinching nuts rather than trying to tap sheet metal. Or maybe punch burred holes and then tap like this:
burred_hole.png

However, if you're having another shop do the laser cutting, why not have them also do the threading?
 
I would use self-clinching nuts rather than trying to tap sheet metal. Or maybe punch burred holes and then tap like this:
View attachment 440580
This method is very common for computer cases, electrical boxes, and other sheet metal applications, probably for a reason.

If it were me, I wouldn't depend on the laser shop for a form tap hole diameter. It needs to be dialed in within a couple of thousandths. I would specify undersize pilot holes and prepare two drill motors, one with the appropriate diameter drill and one with the tap. Test with a representative piece of stock. A lot of form tap charts default to high thread engagement, e.g. 14ga drill (0.182") yielding >70% thread for m5x0.8. I think that tapping for high thread engagement on thin stock risks displacing too much material, as @Finegrain stated. Form tapping may also require deburring if components will need to mount flush with the plate.
 
I would use self-clinching nuts rather than trying to tap sheet metal. Or maybe punch burred holes and then tap like this:
View attachment 440580

However, if you're having another shop do the laser cutting, why not have them also do the threading?
pem nuts have been rejected by the higher-ups. they 1 - don't want to sub out that work and we aren't equipped to do it and 2 they are worried they will come loose and spin. In my experience a properly installed pem nut to stud wont come loose but whatever. secondly, the supplier will do the laser cutting but no hand work, they are focused on removing all manual labor from their work so laser cutting is all they will do for us.
 
  • Like
Reactions: pcd
By the way, I wouldn't expect any problem using an m5 form tap in a handheld drill all day long, but lubrication is critical. Anchorlube seems to work well, and is water-soluble if that helps with cleaning.
 
If it were me, I wouldn't depend on the laser shop for a form tap hole diameter.
Laser shops usually don't understand hole tolerances. Or if they do understand lots of them don't care.

I'll bet there will be a hard zone at the cut. Be prepared for that. Check the form tap size tolerance for M5. It's gotta be pretty close to what they recommend or you'll have trouble. The form tap will upset the material at the entry and exit more than a cut tap. Either burr will come right off with a sander.
 
I do this all of the time in steel and aluminum. Put a drill tap in an impact driver and send it through an undersized hole. Dip the tap in some sort of lubricant every so often.

We use dewalt brand drill taps but other brands are typically good, but we've gotten some cheese grade ones too. We have some generic drill lubricant in spray paint lids. It dries up a bit and becomes a gel that sticks to the tap.
 
Laser shops usually don't understand hole tolerances. Or if they do understand lots of them don't care.

I'll bet there will be a hard zone at the cut. Be prepared for that. Check the form tap size tolerance for M5. It's gotta be pretty close to what they recommend or you'll have trouble. The form tap will upset the material at the entry and exit more than a cut tap. Either burr will come right off with a sander.
With machining, the customer tells the machinist what tolerance to make it to and they figure out the process and pricing from there.

With laser cutting, the shop tells you what tolerances the laser holds and the customer has to design to it. Unless the machine is neglected and the kerf hasn't been adjusted, there isn't much you can do to nail a tolerance and there isn't enough money to do anything with a laser other than keep it cutting as much as possible.
 
Apparently nobody read the part about it holding small din rails and fans. Thread engagement smedgmagment. These things aren't going to space. They aren't used as anchor points for fall arrest harnesses. The guy could blue painters tape these components and it would hold just fine.

OP, don't over think this. A bench block, a tap wrench, cutting oil, and a spiral point tap is all you need for success here.
 
If the hole is undersize, the form tap will have to squeeze too much material into not enough space, and possibly break. Cut tap can just cut that extra material away.

If the hole is oversize, the form-tapped thread % goes way down, and the minor diameter can be below spec. Since this application has only ~3 threads of engagement, low thread % might be quite bad.
Just for kicks I grabbed a 5mm form tap while I was out in the shop doing another Imperial small tapping job. Using my dirt-common 18v Makita drill motor, I drilled two holes in 12 ga steel sheet---one at the recommended size for a 5mm form tap and one 10 thou under.

Then I chucked up the tap and put a little high pressure grease on it. I zipped through both holes without hesitation and took maybe 5 to 10 secs to tap each hole. The drill did not even seem to notice as it formed those threads effortlessly in both holes.

Here is a pic of the two holes on the exit side. The properly-sized hole has a bur that you can just see and easily feel and catches the fingernail The undersize hole has a visible burr.
The undersize hole is labeled "-10"

1716401414896.png


If I were tapping those holes, either one would be very acceptable and both would be deburred on both sides with a good deburring tool---the cone shaped ones with the hole through the cone as they make a very clean chamfer. Same for a cut tap hole.

Conclusion: I do not think I'd worry about undersize laser holes for form tapping. The laser shop will hold closer than .010 as they already are said to have experience lasering and subsequently tapping holes. So they know the drill so to speak. And form taps will easily accommodate a hole that does not perfectly hit spec. The form tap will actually do a better job on an undersize hole than a cut tap as the displaced metal will compensate slightly for oversize. Cut taps, not so much.

Denis

Edited out my error of saying I used 20 ga. It was in fact 12.
 
Last edited:
  • Like
Reactions: pcd
Wow, there's a lot of overthinking going on on this one.

Spiral point cut tap in a fast tapping arm and you can tap a thousand holes an hour. We tap 10's of thousands of 6-32 and 10-32 holes in 16 ga stainless sheet for mounting electrical components. Absolutely no issues and you can have some pretty raggedy looking laser cut holes.

Cordless drill on high speed is probably fine too if you have an operator that can poke it in straight.

My favorite tapping arm is a Roscomat Moquitto.
 
  • Like
Reactions: pcd








 
Back
Top