Fadal gcodes for retract Z home

[Mike Whitten CAD/CAM Contractors]

Hello,

 

I am wondering what the best codes to use to retract the Z axis home on a Fadal using format 2. I can't have anyone try it for me and the customer is 300 miles away. The machine uses "Tool Lengths" like a Horizontal mill and large Z work offsets. They tried G49 Z0 in the past and get a crash. I think this will not work on a fanuc type system either.

 

All I need is a Fadal equivalent of "G91 G28 Z0" or "G53 Z0". One or both of these may work but I am hoping for someone that has seen it work.

 

Thanks in Advance!,

 

Mike

[Guest]

This is my line out of a very proven Fadal post with an 88HS control

 

code:

---

pbld, n$, sg00, "H0", "Z0.", e$

---

[Steve Zirtzman]

This is the beginning for one of our Fadal programs:

%

N2 O2055

( FADAL VMC 4020 / 620-55 .NC )

(STEVE Z / 10 - 25 - 06 / 09:12 )

N10 G0 G40 G80 G17 G90 Z0 H0 E0

T1 ( #4 HSS CENTER DRILL............. )

( CENTER DRILL ALL HOLES.... )

N11 M6

N12 S1800 M3

N13 E1 G0 X-10.005 Y-4.855

N14 H1 Z3. M8.1 L12

N15 G81 G98 X-10.005 Y-4.855 Z-.2 R0.1 F3.

N16 X-9.505 Y-5.9535

N17 X-7.755 Y-4.855

N18 X-8.505 Y-2.005

N19 X-8.63 Y-.7035

N20 X-5.505 Y-1.005

N21 X-.755 Y-.755

N22 X-.755 Y-5.6963

N23 G80

N24 G81 G98 X-.945 Y-3.605 Z-.1 R0.1 F3.

N25 G80

N26 M9

N27 G0 G40 G80 G17 G90 Z0 H0

N28 M1

T2 ( 5/32 HSS NACHI TWIST DRILL...... )

[Mike Whitten CAD/CAM Contractors]

It would seem that "H0 Z0" would cancel the offset and send the machine to Z0. Since there is a Z work offset applied from the gage line to the top of the part ( maybe like Z-15.00), the machine would try to send the gage line to the top of the part resulting in a crash.

 

Thanks for the help,

 

Mike

[Rick Henrickson The Boeing Co.]

did you try it?

[Mike Whitten CAD/CAM Contractors]

I am very sorry Rick. I am in kind of a stupid situation where I can not try it. These people are telling me that there is not a way to do this and that they have tried everything. Their work around for M0's etc is to just do a tool change everytime. They want special posts without retracts even on M0's

 

 

Thanks,

Mike

[crazy^millman]

Have you tried G49 Z0??

[Mike Whitten CAD/CAM Contractors]

Ron,

 

They know for sure that will not work as they did try that many times.

 

I always use G53 in my Fadal fmt2 posts and have never had a problem. Fadal also reccomends G53 Z0 but they said it may be better to put a G49 after the G53 Z0 line.

 

Thanks!,

Mike

[TheePres]

I use "G49 H0 Z0" without a problem both format #1 and #2.

We also use large work offsets (3.00+-)

[Guest]

Michael,

 

It seems to me all of these suggestions would likely work, so that got me thinking.

 

Now, I don't know if this is possible, never tried it. Could they have their CS position set wrong?

[Mike Whitten CAD/CAM Contractors]

TheePres, Thanks

 

John,

I am not sure about the CS position, I can only guess it is correct. I do have a question for you though. If G54 Z is set to the top of the part and you did an MDI of "Z0", then wouldn't the machine ram the Head into the part? If no, why not, if yes then why would it not do the same thing if programmed. They are setting the G54 Z just like a Horiz mill. IOW, it must be like Z-15.

 

Just trying to get to the bottom of this thats all.

 

Thanks!

 

Mike

[Colin Gilchrist]

Sounds like a cold start position error to me.

 

Couldn't you just set one of the work offsets to a "safe" position (H6 maybe?) and call it at the program end before cancelling height compensation?

 

They must have something really screwed up because Fadals aren't that difficult.

[Justin Beebe at Folsom Tool]

The code that works for us between tool changes is:

 

G53 Z0

E0 X0 Y0 Z0 B0 H0

T#M6

 

We us format 2 and have a large Z workoffset so we can set our tools off the table and have them automatically offset to the center of rotation of our rotary axis.

 

Hope this helps,

 

Justin

[Mike Whitten CAD/CAM Contractors]

Thanks Colin and Justin.

 

I appreciate the input.

 

Mike

[Andy]

If the cs was set wrong would it not try to change tools at the erroneous cs Z position.

That would be nice!!!!! I am not willing to try that one on mine.

[Bryan Johnson]

here are my results using Format 2

CS position and Tool Change position are set same for Z

Z-10. in the fixture offset.

 

G0 H0 Z0

will send Z 10” below the tool change position (not good)

 

G0 G28 G91 Z0

Will send to Tool Change position regardless of Z offset, (good)

[jmayo]

G90 H0 Z0 Works fine for us here

John

[Mike Whitten CAD/CAM Contractors]

Thanks Andy, Bryan and jmayo for the input.

 

I am going out of town until tonight. Have a great day all.

 

Thanks,

Mike

[TonyL]

This is what I used on a Fadal 88HS controll

 

T4M6(.3125 DRILL

E1 X0 Y0 S2200 M3

Z0.1 H4 M8

G83G98R+0.1Z-1.22 F40. I1. J.8 K0.25 L0

XY

G80G0Z1.M5M9

G91 G28 Z0

G90 G80 G40 G17 G0

 

Tony

[Mike Whitten CAD/CAM Contractors]

Thanks Tony

 

Mike

[Kennamichael]

G90M5

G53Z0

E0X0Y0Z0H0

M30

%

 

there's the end of our programs.

 

G0Z1.

G90M5

G53Z0

M1

(0.093" BULL ENDMILL)

T2M6

G0G90S3000M3E1X-.0998Y1.2672

H2Z1.

 

and that's for a toolchange

 

hope this helps...

[racingman]

This may sound stuipd but do you know if they were using a fixed cycle?

[Mike Whitten CAD/CAM Contractors]

Thanks for the code Scotty.

 

Brandon,

Welcome to the Forum! and thanks for the input. What are you referring to by "Fixed cycle"?

 

 

All,

It looks like a Fadal is like any other standard machine with Fanuc type gcode. You must always use a "G53 Z0" or a "G91 G28 Z0" when you utilize Z work offsets and Tool lengths ( many people say positive offsets).

 

Thanks everyone.

 

Mike