peck rigid tap

[fourperf]

Hi Guys, I didnt want to hijack the other thread so I thiught I would start a new one.

When you peck rigid tap does that have to be reflected in your post or is it something only at the machine.

Thanks

Mark

[cam1]

Hi:

check this out

http://www.haascnc.com/cncmag/answer...&ArticleID=562

[fourperf]

thanks for that but how would the block read differently that a normal g84 rigid tap cycle. Is it in fact a G84?

thanks

mark

[DSL PWR]

Just use multiple G84's to deeper depths.

[Geof]

Originally Posted by fourperf thanks for that but how would the block read differently that a normal g84 rigid tap cycle. Is it in fact a G84? thanks mark

It is just G84, you have to have the REPT RIGID TAP Parameter set and you can be lazy; write one G84 line then just a string of increasing Z depths.

[Donkey Hotey]

Originally Posted by Geof It is just G84, you have to have the REPT RIGID TAP Parameter set and you can be lazy; write one G84 line then just a string of increasing Z depths.

Dang, you're right! It's modal. I saw the other method and filed it away in my brain but you're right: it's even easier than multiple G84s. Thanks Geof!

[Geof]

Originally Posted by Donkey Hotey Dang, you're right! It's modal. I saw the other method and filed it away in my brain but you're right: it's even easier than multiple G84s. Thanks Geof!

You can do the same with G82 and G83 (and a lot of other canned cycles I guess) if you have a lot of holes withe different depths; just put a Z along with the X, Y coordinate.

But with the Haas editor it is so easy to select the entire G84 line, copy it multiple times, and then just step down changes the Zs.

But don't copy it too many times or you will get the corrupted program error I described in a different thread.

[pit202]

will be fine if there cut be an Q parameter like in drilling

[Donkey Hotey]

Yes, I agree: it should not be any harder than doing a peck-drilling cycle. I really do wonder why they haven't done it. They have customized enough other codes to be proprietary to Haas controls. This wouldn't be any different.

[Geof]

Originally Posted by pit202 will be fine if there cut be an Q parameter like in drilling

Give them time, give them time.

[fourperf]

Hey Geof, would you mind posting how the code would look to peck tap 1 hole (say 3 pecks) for a numbskull like myself. Thanks a lot geof

mark

[Geof]

Originally Posted by fourperf Hey Geof, would you mind posting how the code would look to peck tap 1 hole (say 3 pecks) for a numbskull like myself. Thanks a lot geof mark

When I mention above how easy it is to copy lines with the Haas editor I mean you can write one line then just copy it and change the Z values.

G84 Z-.3 F50. R.1
G84 Z-.55 F50. R.1
G84 Z-.75 F50. R.1
G80

Or just write one line and follow it with the different Zs

G84 Z-.3 F50. R.1
Z-.55
Z-.75
G80

One thing that is a bit of a pain when you want to peck tap is doing an array of holes.

For spotting (G82) and drilling (G83) you can activate the canned cycle then go to a subroutine with all the hole coordinates, the same subroutine for both canned cycles.

You could also activate the G84 at the first Z depth and go to the subroutine.
Then the next Z depth and go to the subroutine.
Then the final Z depth and go to the subroutine.

And waste a lot of time with the machine running back and forth.

For production programs what I do is have two subroutines. The first has all hole coordinates with a second subroutine call to a tapping subroutine:

X1. Y1. M97 P3000
X2. M97 P3000
X3. M97 P3000
etc

-------
P3000 G84 Z-.3 F50. R.1
Z-.55
Z-.75
G80
M99

It is a little tedious to write when you are dealing with a lot of holes but it is worth it because the program runs faster.

This is where the Q value would be very, very handy....Nudge, Nudge to you guys at Haas.