A Fadal post question

[Bill K]

After a co worker retired , I now run the fadal that he used to run, so I'm new at this machine. The control is Fadal CNC HS88 this is one of there low end machines and is about 7 years old. We run format 1programing

The post that he ran was called " MPFADAL.PST " This post is old and goes back the Mastercan V7.

So today I tried the latest post that came with Mastercam v9 This post is called MPFADAL1.PST

The first operation that I ran was tapping. the drilling went ok, but the tapping didn't. The tap started ok, but when it reached the bottom of the hole it appeared to rapid retract.

This is the line of code (N9G84G99X-.25Y3.Z-.5R0.25F160.Q.0313P2000)

This was for a 10/32 tap. The feed & speed I have set is 5 IPM at 160 RPM

I'm not sure what's going on here, but I don't want a rapid retract, and I don't see a way to turn it off.

Is it possible that this post isn't compatible with this machine/ control ?

[Kannon]

Bill,

Double check to make sure you are using the tapping cycle! I accidently drilled and followed with a tap and forgot to change it from drill to tap!

[Bill K]

I'm using the tapping cycle

[Trevor Bailey]

There could be two tapping cycles. One is a G84 for a tapping head/floating tap holder and then there should be a G84.1 for rigid tapping. The G84.1 goes on the line with your location moves. G84.2 should go on a line AHEAD of the location move with the spindle speed.

[Steve Biehl - Cimquest Inc]

Bill,

it looks like you used the 'Rigid tap' cycle. Did you mean too? The 'P' is the retract feed percentage.

[Steve Biehl - Cimquest Inc]

yep, Trevor's got it. I'm backwards. You used the 'floating' tap cycle not rigid.

[Bill K]

BTW. As it did this rapid retract, it pulled the tap out of the holder, and broke it going to the next hole.

[Bill K]

We have always used Rigid tapping with this machine.

[Kannon]

Bill,

I dont know how close the Haas is the the Fadal, but I do recall there was a parameter in our mill to speed up the reverse. It did to us the same as you mentioned.. broke the tap pulling it out of the holder. I will try to find the setting and see if maybe the Fadal has the same.

[Bill K]

In regards to floating vs rigid. I only see one chose in the drilling cycle menu, and that is TAP.

[Kannon]

Bill,

In the Haas it has a tap retract multiplier in the settings screen. setting 130 if the setting is set to 1 it retracts the same speed going out as in. If it is set to a 4 it is 4x faster on the way out then the way in. Double check and see if yours has a multiplier. When we messed with this setting and increased it was when we were breaking taps like you mentioned.

 

Good Luck,

[Paul Decelles]

Um, perhaps I am way off base but wouldn't it be easier to post a tapping cycle using your old post and then compare the output to see what the difference is? I mean if the code was ok from the older post then it should be pretty easy to see what is wrong with the code output from the new right?

[Steve Biehl - Cimquest Inc]

Bill,

the stock MPFADAL1 has 'Rigid tap' as its 8th cycle option.

 

This is driven by the post text file. You should have a MPFADAl1.txt file.

[Bill K]

I don't see any settings or multiplier's in Mastercam.

[Kannon]

I apoligize Bill,

These settings for us are at the machine in the settings screen. Probably not gonna be the problem if you were tapping on it before.

 

Sorry for the mix up!

[bpa123]

are you using a floating tap holder(tapamatic)or are you ridigid tapping with the tap in a solid holder?

[billystein]

it looks ok to me except the p command. I have never used it in tapping cycle. also you dont need the g99. I dont think it does anything wrong but I never use it. the f160. should be the same as the spindle speed

[Bill K]

Steve

Steve,

I do have the post text file MPFADAL1.txt along with MPFADAL1.PST

The screen shot that you show doesn't look anything like the one that I was seeing until I brought the text file in with the post file.

Now I see the same options that you had in your last post. I think we are now getting some where.

[Bill K]

Steve,

This is the code that I'm getting now that I have the text file in place using MPFADAL1.PST

One thing that I'm wondering about is the retract feed%

 

 

N0 O0000 (BK )

N1 ( CREATED ON 04-25-05 AT 2:30 PM )

N2G20

N3G0G17G40G49G80G90H0E0Z0

N4 ( TOOL - 1 DIA. OFF. - 0 LEN. - 0 DIA - 0.25 )

N5T1M6

N6G0G90S160.2M5M90E1X0.Y0.

N7G84.2

N8H0Z3.M8

N9G84.1G98X0.Y0.Z-.5R0.25F160.Q.0313P2000

N10G80

N11M5M9

N12G90H0Z0.

N13E0X0Y0

N14M2

[Thad]

Bill,

 

I'm going from memory, but I believe a "100" P value will get you out of the hole 2X as fast as you went in. P200 would be 4X as fast, and so on. Your 2000 value may appear to be a rapid move at that rate. If you want to come out of the hole as fast as you went in, just eliminate the P value.

 

The ".2" on your RPM is only required if you tap above 2500 RPM. The ".2" forces the machine into high gear.

 

A G98 will return your tool to Z.25 (R plane) and a G99 will return your tool to Z3. (clearance) in this example, after tapping the hole.

 

Just a side note...you may want your H to match your T.

 

Thad

[Bill K]

Thanks everyone,

 

Its working ok, I'm not breaking any taps.

The code in my last post wasn't exactly correct.

Here it is with the correct numbers, with a 0.1 feed%

 

N0 O0000 (BK )

N1 ( CREATED ON 04-25-05 AT 3:24 PM )

N2G20

N3G0G17G40G49G80G90H0E0Z0

N4 ( TOOL - 21 DIA. OFF. - 0 LEN. - 21 DIA - 0.1875 )

N5T21M6

N6G0G90S160.2M5M90E1X0.Y0.

N7G84.2

N8H21Z3.M8

N9G84.1G98X0.Y0.Z-.5R0.25F160.Q.0313P100

N10G80

N11M5M9

N12G90H0Z0.

N13E0X0Y0

N14M2

[Trevor Bailey]

Glad all is working.

[crazy^millman]

Bill look at this code:

code:

---

%

O3122*FIX

(PROG'D BY PROGRAMMER? ON APR-26-05-12:27 )

*OPERATOR

*MC9 FILE LOCATION - K:CNC-MILLPENTBB-GE3-FILESGAAUHK31214-1 MARK 4-23-2005.MC9

*NC PROGRAM LOCATION - K:CNC-MILLNC-FILESFADALFIX.NC

*T16 | 1/4-20 TAPRH | H16 | D16

G0G17G40G80G90

T16M6* 1/4-20 TAPRH

*MAX | Z.1

*MIN | Z-1.

G0G90E1X0.Y0.

S366.2M5

G84.2

H16Z.1M8

G4 P500

G8

G84.1G99X0.Y0.Z-1.R0.1F366.2Q.05

G80

G0Z.1

M9M5

G49Z0.

X0Y9.5Z0E0

M00

M02

%

---

Now there are 2 things in my posted code that are not in your posted code.The first and most important on a Fadal is the G8 this one thing gets over looked by more people that anything. This as explained here: Fixed Fadal Cycles

quote:

---

Program a G8 (No Ramps) for the tap operation. This allows the tool to feed at a constant rate in and out of the hole.

---

Now the others has to do with F not having .2 at the end of the spindle amount and the reason for this is to make the machine go into high gear as stated here from the above page:

quote:

---

When using the G74 and G84 cycles, the spindle should be programmed for the high gear range. This will provide better spindle reversal for tapping. This is accomplished by programming a “.2" at the end of the S word or F word. For example, S1000.2 or F1000.2 sets the spindle speed at 1000 rpm in the high gear range.

---

My post has them in it and I would look to adding them into your post. You can contact your dealer or we can help you