Tapping Blind Holes - Do I need an offset with a bottoming tap?

[longshotsystems]

When tapping a blind hole with a bottoming tap should I use a positive offset from the hole bottom, or can I run it right down to what Fusion sees as the hole bottom? Trying to avoid breaking a tap, and curious what the best practice is here. Cheers!

[RoccoHilton]

as a rule, the depth of the thread is always less than the depth of the blind hole by 1-3 mm, depending on the diameter of the thread

[programming2C78B]

it entirely depends on the hole depth, your tap lead, and how much actual thread you are after....Lead is usually 2x Pitch


the tip of the tap can safely go down to the full diameter depth of a drilled hole. 

[longshotsystems]

When you say lead is usually 2x pitch can you clarify for me as to what lead is? Cheers!

[a.laasW8M6T]

He means the lead-in or chamfer on a bottoming tap is normally 2x the thread pitch in length for a hand tap

For a spiral flute machine tap, normally 3x pitch but it varies depending on tap brand and specification.

for example an M8x1.25 thread needs to be tapped 2x diameters deep.(16mm)

The hole will need to be drilled at least 3x1.25mm deeper and the tap will need to be run right to the bottom of the holes full diameter(not the drill point) 

so you would drill 19.75mm deep full diameter(round it up to 20mm)

you would run the tap to the same depth.

Bit of info on taps:

https://www.sandvik.coromant.com/en-us/knowledge/threading/tapping/how-to-choose-tap-type 

[Don.Cyr]

Attached is an excel sheet from some of my programming notes, you can input thread and tap drill info for a blind hole and it will output the values for the drill and the tap depth for various style taps. Been pretty reliable and accurate for me so far. *Keep in mind, this is based on using a spiral flute or forming tap for blind holes to avoid chip packing*

[Tomas_V_cz]

I don't think it's possible to enter it in general like this. Each manufacturer, even each type of taps can have a different dimension, some taps are to the point and others are flat, some are for blind holes and some for through holes (those usually have a longer non-cutting part) It is ideal to measure them... Those for blind holes have a non-cutting part around 0.5 diameter of the thread.

It would be ideal to have this data entered in the tool table and somehow work with this data during programming. I had a similar issue regarding drilling holes.

https://forums.autodesk.com/t5/fusion-manufacture/drilling-holes-data-about-the-tip-of-the-drill-bit...

[Don.Cyr]

As I mentioned, this was for blind holes using a spiral flute or forming tap. In those cases for the most part, the tip is flat and the mfg. will list the lead (in pitches) for the tap type if it's taper, modified bottoming, bottoming, etc.. you can calculate correct tap depth from that. I agree that Fusion should be able to store this data, but in the meantime that chart is what I use here at the shop and has been reliable. It will also give correct drill depth (to the tip) based on diameter and point angle.

[programming2C78B]

I simply made my own chart, since I already asked about a "lead in length" field to be added to the Tap tool definition page to no avail. You're welcome to copy my info, we use OSG form taps and 120* spot drills. 

[longshotsystems]

Thanks all! In this specific case I am using a 1/4-20 bottoming tap for one set of holes, and the other I'm using a 10-24 form tap (flat bottom) for another set. I have the appropriate drill sizes in some 135* jobber drills, and am trying to determine how much of a positive offset I should add to the tap job to ensure the tap gets as deep as possible, but doesn't collide with the floor or smush against chips. Likely not an issues with the form tap I suppose.

I wasn't sure if Fusion automatically recognized you're tapping a hole and would program the appropriate max safe depth automatically, or if I needed to do an offset from "hole bottom" to be safe. 

[programming2C78B]

you didnt give any depths, but i've never broken a cut tap from chip packing. Peck 1x diameter, and have about .02 beyond the tap for safety and youll be fine 

[longshotsystems]

The 1/4-20 is drilled to .25" + drill tip, which is about as far as I can go before it punches through.

The 10-24 is drilled to .28" + drill tip.

These are mostly holes to hold the part for Op 2. There are 8 of them. They can be used after for accessory mounting (it's the inside of a glove box door). So they don't really need to hold much, but just trying to get enough bite on the threads. Would a 1/4-28 be better in this application?

[longshotsystems]

Or given the limited depth should I shift to a 12-24 size?

[programming2C78B]

1x diameter in thread is plenty for most use-cases.