[saabwagon]

Hello, I am new here.I have a 97 VF1 That has rigid tapping.. I have a few questions from those with more experience. I need to tap some M10*1.5 Holes 1" deep (Currently by hand to full tap depth) in 6061 T6. I can drill the pilot hole as deep as the drill will go but it is still technically blind hole. We need more than we can make by hand, plus we have the CNC might as well use it. Ok knowing this..

First question: What holder is best for this application? Will an ER collet work? Or should it be a dedicated holder with the square positive drive?

Second: Do you have some sample code to get headed in the right direction?
I could not seem to get the metric feedrate conversion right in my head so no way I am sticking metal in metal If you know what I mean..

Here is a quick Video of running some recent parts. http://trolltuner.com/cnc/ We are not a job shop but a performance parts manufacturer. Many thanks in advance. Nick

[HuFlungDung]

Pitch of thread in inches: 1.5/25.4 = .059055

Multiply that by your desired rpm to get the feedrate. Eg., 400 rpm would require a feedrate of 23.622 ipm.

Use a spiral flute tap to auger the chips up and out of the hole as the tap goes in.

Many guys hereabouts would recommend a cold forming tap, which requires a slightly larger tap drill diameter, but there are no chips to contend with.

There is a variable in Haas setup for repeat rigid tapping, in case you find a need to tap each hole in two or more stages.

[lakeside]

try these # below cast data is the same as 6061. dia. info is not relavent also note change in spindle %

[maquiza]

I do tap every day; I use spiral tap with the G code G84. The formula HuFlungDung told you is right. Also my Haas machines came with a metal sticker with the RPM and feeds for steel and aluminum, I use that as reference, but sometimes when you tap harder materials you must lower your RPM and do the formula for the feeds.

[saabwagon]

Thanks!!, One more question.. Best toolholder for the tap? I know the consequences of the tap slipping

So you think a spiral Flute tap is better than over drilling depth and using a spiral Point tap and just packing the chips at the bottom for clean-out later? (We do the latter by hand)

[Geof]

Thanks!!, One more question.. Best toolholder for the tap? I know the consequences of the tap slipping

So you think a spiral Flute tap is better than over drilling depth and using a spiral Point tap and just packing the chips at the bottom for clean-out later? (We do the latter by hand)

I have done 1/2-13 in leaded steel just using an ER32 collet so you should be okay with M10 in 6061. I suggest Repeat Rigid Tapping using a spiral flute to gets the chips out. Less likely to cause jamming and breakage and easier to clean out. Just make sure you have Repeat Rigid Tapping turned on in the Parameters (I think it is parameter but it could be settings) if you want to repeat.

[lakeside]

osg high sprial performance tap the holder you need a ridge tap holder and tap insert holder they are made for this aplication only spring loaded

[pugsley]

Another trick that i use everyday when tapping is to type "G95" on the line directly above the tapping cycle.
What that will do it will leyt you directly imput the pitch in the tapping cycle and not have to worry about varing the pitch according to rpm.After the G80 at the end of the cycle do not forget to type "G94" to restore feed back.

eg
G95
G84 G98 S50 Z-?? R?? F1.5(F0.0591)
G80
G94.

[dertsap]

Another trick that i use everyday when tapping is to type "G95" on the line directly above the tapping cycle.
What that will do it will leyt you directly imput the pitch in the tapping cycle and not have to worry about varing the pitch according to rpm.After the G80 at the end of the cycle do not forget to type "G94" to restore feed back.

eg
G95
G84 G98 S50 Z-?? R?? F1.5(F0.0591)
G80
G94.

this is my preferable way of tapping , if i want to change the rpm i dont need to worry if i forgot to change the feed rate or not , too much to think about in a day

[mishikwest]

Hi Nick,

For your holder, an ER is just fine. Get yourself a square drive (tap specific) collet for it to drive the shank of the tap... you'll be almost certain of no slippage then.

I'm also a BIG fan of thead forming / roll taps. Lot's of advantages, the primary being no chips to contend with AND it makes for a stronger thread via the cold forming action. Somewhat analogous to the grain flow created in a forged part. No chips, so you'll be able to tap easliy within about .050 (or less) of the bottom of your blind hole. (Of course that's not including the drill point angle).

You've got some chatter with that first tool in your video, have you tried a 3 flute cutter?

Also, it's great to see someone tuning the Viggens! Can't belive those hp #'s ! You gonna hit the German DTM series. I'm a euro-car fan too, but an Audi guy.

[dertsap]

have you concidered using sinthetic coolant on that machine , far superior to the biodegrades , lil more pricey to buy but it doesn t go skanky and lasts far longer , running sythetics alone will help big time in tapping ,less tool breakage and wear all around ,

[mishikwest]

We're talking cutting coolant and not grinding coolant, right? I've yet to see a synthetic that has outperformed mineral or vegtable in cutting applications.

I'd be happy to know of any sythetic that runs better than any of the Blaser or Hangsterfers mineral based coolants (in aluminum). Hopefully we're not getting to off topic on this thread , yet.

[dertsap]

CIMTECH is what we used don t remember off hand what grade we used at the last company , i finally talked the present company into it and we are going to phase it in next month , we did tons of steel cast and aluminum and that stuff held up , we had some parts that were typicaly hard on taps , we would up the consentrate a bit and had no trouble , we changed the coolant once a year , and one guy would take all our old coolant and run it thru his system , theres recycling for ya , it holds up to a lot and lasts a long time , but it does gum everything up some after sitting on the table and vises over the weekend ,but washes off once the coolant starts running again
,i don t like the skank or bacteria of the other coolants , concidering i m breathing it in all day and my hands are wet with it all day , i dont need the bacteria
mind you synthetics probably aren t any better for me ,
hazzards of making a living i suppose
if you want exact grade let me know i can find out easy enough

[Traceycnc300]

We tap a good deal of alu. using osg spiral taps holding them with er collets with no problem.To figure feed rate I multiply the metric pitch by .03937 times the rpm to get ipm.works well for me.Example(1.5x.03937x400rmp=23.622ipm)

[saabwagon]

Making parts!.. Thanks for the support.. One thing though. There is no G95 on my machine (Not in Manual Either), Tried G93 but then got weird alarm (Forget now) about not being able to move axis) Anyway using pitch x Rpm and works great. Used a Spiral Flute tap.

In that video, Re the chatter. I got a shorter tool holder and played with the rates and it was quiet.

[MetalZilla]

Making parts!.. Thanks for the support.. One thing though. There is no G95 on my machine (Not in Manual Either), Tried G93 but then got weird alarm (Forget now) about not being able to move axis) Anyway using pitch x Rpm and works great. Used a Spiral Flute tap.

In that video, Re the chatter. I got a shorter tool holder and played with the rates and it was quiet.

I don't have G95 on my machines either:

[eaglemike]

There's an easier way to get proper spindle RPM and feed combinations that I saw mentioned here for metric threads.
Ex: I often tap 6X1 threads. This would mean 254 rpm with a feed of 10.0 inches. I've found that about 1000 rpm works well, so I use 1016 rpm and 40.0 ipm.
For a 1.5mm pitch, start with 254 rpm and 15.0 ipm, maybe 3X this would work well.

I've been pretty happy using thread forming taps in blind holes. Much easier than dealing with chips. Also don't need to dig them out for later processing, such as anodize.....