I am having trouble tapping stainless steel (400 series). I have tried several
things and now using a coated through tap in my blind holes as these seem
to be the only ones that don't break. What I was wondering is, is how do i tell
if the gain ect. is set properly on my spindle drive as I do not understand the
set up info at fagor. I use a fagor 8055 control with ac fagor drives and spindle orientation.? any help appreciated.

Why type of tapping oil/fluid are you using? For stainless, we use MollyDee.

Tapping stainless is a beeaatch! weve had the tool companys come in a set us up with their super wounderfull unobtainium taps, they seam to work great until the tooling guys leave the building! :D

After all the taps weve tried in stainless what ended up working the most consistantly was the basic 2 flute spiral point tap Uncoated (made for aluminum) with MOLYDEE.

we were doing 250 holes in each plate to the tune of 50 to 100 plates. We could get almost 3 plates before the tap broke but we changed the tap at each plate. (seamed a no brainer $4.00 tap vs as 500.00 plate, cost in time for repair was figured at around an hour) of course this was a 6-32 tap. So your app. might be different.

Moly dee seams to be used alot , we have also started peck tapping
useing increasing z values after the g tap cycle
but this is for 3/8-16 roll from tap in 316l

good luck

how do you peck-tap?

Basically program it to tap the same hole several times using different depths.

G85 X1.0 Y1.0 Z-.625 F9.9 R0
G85 X1.0 Y1.0 Z-1.25 F9.9 R0
G85 X1.0 Y1.0 Z-1.90 F9.9 R0

G85 is actually for boring/reaming - as we use tap-a-matics alot - but you get the idea

yes Dab has it right , sorry for the late reply, working the weekend shift,
like a drill cycle, a tap cycle is also modal, untill a g80 is called so adding z values after the can cycle wil repeat at each value

You might try nudging the tap drill size a bit larger, maybe trying for 60% thread instead of 70%. If you can get approval for this, it takes quite a bit of load off the tap.

I like the Ridgid NuClear thread cutting oil for heavy duty work like this. I've not tried this MolyDee stuff, though.

Keep the rpms about 25% slower than you would for tapping steel. Stainless does not transmit heat very well.

i tap a lot of stainless, and i have had to do a lot of blind holes and have had the best luck using molydee and a slow spiral flute tap with a 3 thread chamfer or lead, and the cutting face hook or rake angle has to be 10-15 degrees. in deeper hole applications greenfield has sold me taps with a interrupted of releived thread and they have worked great. all the taps i buy are either greenfield or emuge, nobody else has shown me a better tap than these two companys

also i usually run between 20 and 40 sfm when i tap, my parts are usually 60-70% thread

i also have had the best luck with spiral flute taps and found osg to be the best choice per part from a cost perspective 316 ss this was

My nifty little tapping guide says 10-15 SFpM for 400 stainless.

A place I used to work had a different slant on things...
Threads per Inch times 10 equals RPM. (24 TPI = 240 rpm)
Their logic behind this was pretty convincing... The pitch determines the actual size (surface area) of the thread; a smaller thread (higher tpi) can run faster than a larger thread (lower tpi).
This really suprised me at how well it worked, but I can't remember for certain if it was 300 or 400 stainless.

But the nifty tapping guide has never failed me!

ghyman, we use the same method. Every now and then they (the programmers) feel like mixing things up and running the taps at a percentage of the x10 rule (slower or faster depending on material).

The best thing about that method, is that no matter what size tap, the feedrate is always the same. 10.0ipm. For some reason though, we always use 9.9 ipm.

In 95% of our hard metal (SS and Titanium), and sizes of 3/8" and over we use form taps.

The 9.9 IPM is probably to allow the use of a compressable tap driver (rather than a solid driver.) By running the feedrate slower, it allows the tap to "find it's own best way" into and out of the part, instead of having the machine just JAM it into the hole. Tapping is a brutal operation, every little bit of assistance helps!

Increasing the tap drill size will help. Drilling the tap drill hole deeper or through will increase the chip clearance below the tap and allow you to use a spiral point tap. If you cannot do any of these get bottoming heavy duty spiral flute tap. I've never tried slow spiral versus fast spiral taps. Heavy sulfurized cutting oils has always been the best tapping lubricant but in today's "clean" world it is not considered acceptable. There are many different lubricants which can do the job.

try express taps and moly dee as cutting fluid. express taps require a larger tap drill.

how do you peck-tap?

Depending on your control, you can usually put a "Q" on your G84 line. Q=incremental depth of peck until z depth is reached.