spindle speed for 5mm tap

slowmotion · Oct 2, 2019

I am rigid tapping some 5mm holes in 6061 in blind holes to 11mm depth. No coolant, just tapping fluid on the tap and in the holes. I programmed the speed at 500, forgetting that the retract speed is twice that. It worked fine but is that too fast for safety? If I break a tap, it'll be extremely difficult to get out, given the location. I am using an Emuge Tin spiral tap in my tapping head.

Larry Dickman · Oct 2, 2019

you're rigid tapping in a tapping head?

Mike1974 · Oct 2, 2019

What machine? Sounds like maybe a Haas with 2x retract speed.... 500 is fine, depending on what you want to accomplish- never breaking a tap and getting good holes, getting more cycle time..? You could go faster probably, but if it ain't broke don't fix it....

Milland · Oct 2, 2019

My experience is that TiN is not a great coating for Al work, due to the surface chemistry of the coating attracting a thin transfer of aluminum. Now you have an aluminum surface cutting the Al stock, which is not ideal. Maybe your tap lube is good enough to prevent the buildup, but I'd either use a bare tap, one that's been nitrided, or perhaps a chrome coating.

Tichy · Oct 2, 2019

In Alu? You're way slow on the speed, but as above posted that's fine if the cycle time is no problem. Maybe add a Q value but for heaven's sake it's Alu, it's like cutting butter.

If I had to care about the cycle time in that material, well, I've run stainless steel at 1000+rpm. It's not like you'll break taps due to your speed-demoney ways of going half that

Mtndew · Oct 2, 2019

slowmotion said:
It worked fine but is that too fast for safety?

It all depends on your setup, how you're holding the tap, the runout, the machine and the hole size.
On my Brother mill, I would tap at 6,000 rpm in aluminum.

Tichy · Oct 2, 2019

Mtndew said:
It all depends on your setup, how you're holding the tap, the runout, the machine and the hole size.
On my Brother mill, I would tap at 6,000 rpm in aluminum.

Yup, I'd go 4k rpm conservative but I'm no specialist at Alu.

slowmotion · Oct 2, 2019

Sorry, it's a Bilz chuck, tension/compression. Machine is a VM20. I had a feeling that coated was not the best choice for alum but it's what I had. These holes are 5" down a 4" bore and close to the wall, the tool holder barely clears radially and depth wise. I'm paranoid of breaking a tap in a very inaccessible location, reason for my question. Low volume so cycle time isn't a concern.

Mtndew · Oct 2, 2019

slowmotion said:
Sorry, it's a Bilz chuck, tension/compression. Machine is a VM20. I had a feeling that coated was not the best choice for alum but it's what I had. These holes are 5" down a 4" bore and close to the wall, the tool holder barely clears radially and depth wise. I'm paranoid of breaking a tap in a very inaccessible location, reason for my question. Low volume so cycle time isn't a concern.

View attachment 266395

Another thing you could do if you're worried about the tap breaking is to only start the tap in the machine and finish tap it by hand.

Milland · Oct 2, 2019

Hell, most reliably of all just threadmill it. Makes the risk of a broken tap "zero".

Tichy · Oct 2, 2019

slowmotion said:
Sorry, it's a Bilz chuck, tension/compression. Machine is a VM20. I had a feeling that coated was not the best choice for alum but it's what I had. These holes are 5" down a 4" bore and close to the wall, the tool holder barely clears radially and depth wise. I'm paranoid of breaking a tap in a very inaccessible location, reason for my question. Low volume so cycle time isn't a concern.

View attachment 266395

Do you tap a 1" deep or 5" deep hole?

Either way I didn't get that from your post. 1" is 25mm. 5" is 127mm.

With the standard Fanuc cycles I'd program G84 Q7 (in millimeters). That should make it dead sure. I can't see any reason for less than 1k rpm however.

slowmotion · Oct 2, 2019

Tap depth is only 11mm, the holes are located 5" down into a 4" bore, see pic. I know I'm being paranoid but the blocks I'm working on cost around $8K each. I'd rather not mess one up.

G00 Proto · Oct 2, 2019

1000 RPM and disable the speed doubling on retract. It will cause you more hours of heartbreak than it will save over the course of a year (your mileage may vary). When I'm really concerned I use Moly-Dee (even on aluminum). That stuff is a miracle tapping fluid and you only smell like elk piss for a couple of days after using it.

Benplarina · Oct 22, 2019

I have one question for some of the people suggesting 1000 rpm or greater. I cut aluminum daily as i do fixtures, but I don't dare go past like 250 rpm for my 5/16-18 tap (mind you the purchaser won't spend the money on quality taps). What my question is, is how fast do you feed the tap at that high of rpm to have the tap not pull out of the tapping head? by my calculations, at 6000 rpm on a 5/16-18 tap your feed would be 333 IPM. I guess that doesn't really sound high but I don't think my machine moves that fast. I might attempt it on my next job.

AARONT · Oct 22, 2019

Mtndew said:
Another thing you could do if you're worried about the tap breaking is to only start the tap in the machine and finish tap it by hand.

Or if it has repeat rigid tapping, he could peck tap it. But at only 11mm it shouldn't be necessary.

Mtndew · Oct 22, 2019

Benplarina said:
I have one question for some of the people suggesting 1000 rpm or greater. I cut aluminum daily as i do fixtures, but I don't dare go past like 250 rpm for my 5/16-18 tap (mind you the purchaser won't spend the money on quality taps). What my question is, is how fast do you feed the tap at that high of rpm to have the tap not pull out of the tapping head? by my calculations, at 6000 rpm on a 5/16-18 tap your feed would be 333 IPM. I guess that doesn't really sound high but I don't think my machine moves that fast. I might attempt it on my next job.

The pitch of the tap is the feedrate.
I switched to G95 for tapping a few years ago to prevent errors and it's paid off. So if it's a 5/16-18 tap then my feed is F.05555. This allows me to change the RPM at will and not worry about having the correct IPM feedrate.

As for the tap pulling out of the tapping head, if your tap is pulling out, then you're not holding it correctly or have the wrong type of holder.

If you have collet holders for your machines, I suggest getting tap collets. The kind with the square in the bore for the tap to seat.

TeachMePlease · Oct 22, 2019

Benplarina said:
I have one question for some of the people suggesting 1000 rpm or greater. I cut aluminum daily as i do fixtures, but I don't dare go past like 250 rpm for my 5/16-18 tap (mind you the purchaser won't spend the money on quality taps). What my question is, is how fast do you feed the tap at that high of rpm to have the tap not pull out of the tapping head? by my calculations, at 6000 rpm on a 5/16-18 tap your feed would be 333 IPM. I guess that doesn't really sound high but I don't think my machine moves that fast. I might attempt it on my next job.

Well, for example, I pulled the spec on a Brother Speedio S700 and their posted max feedrate is 1181 IPM...

Benplarina · Oct 22, 2019

Mtndew said:
The pitch of the tap is the feedrate.
I switched to G95 for tapping a few years ago to prevent errors and it's paid off. So if it's a 5/16-18 tap then my feed is F.05555. This allows me to change the RPM at will and not worry about having the correct IPM feedrate.

As for the tap pulling out of the tapping head, if your tap is pulling out, then you're not holding it correctly or have the wrong type of holder.

If you have collet holders for your machines, I suggest getting tap collets. The kind with the square in the bore for the tap to seat.

I tried it out with G84 at those speeds and feeds and it works out. I just never attempted trying it that fast, Now I know it works. Thanks.

and I will definitely try out that G95 method if my machine will take that.

its an odd name, Quaser, with a Fanuc Series oi-md controller on it.

Hardplates · Oct 22, 2019

I don't know why people are so afraid of rigid tapping. I've seen far more taps broken by hand than by machine. Every tap I've ever broken while rigid tapping has been my fault, not the machines. Wrong size tap hole, worn out tap that should have been pulled from service or a bozo move of programing the wrong federate.

Throw some scraps in the vice and play around with them, it's amazing how fast you can rigid tap. It's also a confidence booster in your machine. I've never been to worried about broken taps as they are super simple and easy to EDM out. (Old EDM machines are super cheap on ebay) Given the design they just fall apart once the core is burnt away.

Mike1974 · Oct 22, 2019

Milland said:
My experience is that TiN is not a great coating for Al work, due to the surface chemistry of the coating attracting a thin transfer of aluminum. Now you have an aluminum surface cutting the Al stock, which is not ideal. Maybe your tap lube is good enough to prevent the buildup, but I'd either use a bare tap, one that's been nitrided, or perhaps a chrome coating.

Also, for cutting tools, especially in aluminum, the coating will slightly give you a blunt edge compared to plain HSS (ground properly of course). So for alum 'bright' or plain/bare HSS works better in alot of cases.... Zrn is good for aluminum too, but I've not seen taps with that coating.

spindle speed for 5mm tap

Cast Iron

Titanium

Diamond

Diamond

Aluminum

Diamond

Aluminum

Cast Iron

Diamond

Diamond

Aluminum

Cast Iron

Hot Rolled

Plastic

Stainless

Diamond

Diamond

Plastic

Stainless

Diamond

Similar threads